Mastering Autodesk Inventor 2015 and Autodesk Inventor LT 2015 (2014)

Chapter 6. Sheet Metal

The sheet-metal functionality in the Autodesk® Inventor® program is an extremely powerful toolset, centered on productivity and capturing your manufacturing intent. When you first begin working in the sheet-metal environment, you may feel overwhelmed because the tools and methods you have become familiar with to create other parts in Inventor do not yield good results in the sheet-metal file. However, a mastery of some basic fundamentals in sheet-metal tools can make Inventor sheet metal straightforward and highly integrated with your manufacturing environment. The Autodesk® Inventor LT program does not include the sheet-metal tools discussed in this chapter.

In this chapter, you'll learn to

·     Take advantage of the specific sheet-metal features available in Inventor

·     Understand sheet-metal templates and rules

·     Author and insert punch tooling

·     Utilize the flat pattern information and options

·     Understand the nuances of sheet-metal iPart factories

·     Model sheet-metal components with non-sheet-metal features

·     Work with imported sheet-metal parts

·     Understand the tools available to annotate your sheet-metal design

Understanding Sheet-Metal Parts

The sheet-metal environment was introduced in Inventor 2. Since sheet-metal parts have so many unique requirements, such as flat patterns and manufacturing-specific features, a modified part file is used. The same .ipt filename extension is used for sheet-metal parts, but extra sheet-metal capabilities and data are added. To create a sheet-metal part, you can use the Sheet Metal.ipt template or simply click the Convert To Sheet Metal button on the Environments tab of a standard part file.

To understand how sheet-metal parts work, it is important to keep in mind that sheet-metal design is driven by manufacturing considerations. A basic sheet-metal part consists of flat faces joined by bends. For cost-effective manufacturing, all the bends and corner reliefs are generally the same radius. The sheet-metal template style contains the sheet thickness, bend, and relief information in a rule, and the style is then used during modeling. This saves you considerable time during design because the features automatically use the settings in the predefined style. If you have to make a change, such as a different material thickness or bend radius, you can select a different style and the part automatically updates. These sheet-metal-specific styles are referred to as a sheet-metal rule.

Many sheet-metal parts are brackets or enclosures designed to fit a particular assembly. The sheet-metal tools simplify the process of creating and updating models. For example, you can change a bend to a corner seam simply by right-clicking the bend in the browser and selecting Change To Corner from the context menu.

Getting to Know the Features

The Inventor sheet-metal environment contains numerous specialized tools to help you design components that follow your sheet-metal-manufacturing guidelines and process restrictions. The following sections describe general feature classifications and capabilities that will provide you with a quick road map to the features. Once you understand how the features work, you will be able to build models that capture your design intent.

Starting with a Base Feature

Out of all the sheet-metal tools provided, only four create what are referred to as base features. Base features are simply the first features that appear in the feature history. The following tools can create base features:

·     Face

·     Contour Flange

·     Contour Roll

·     Lofted Flange

Face Tool

The Face tool is the simplest base feature; it utilizes a closed profile to produce a simple extrusion with the height automatically set to the Thickness parameter value. The profile can be constructed out of any shape and can even contain interior profiles, as shown inFigure 6.1. Profiles for face features are often generated from the edge projections of planar faces or surfaces found in other part files, and this capability enables numerous assembly-based and derived workflows.

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Figure 6.1 Face base feature containing an internal profile

Contour Flange Tool

The Contour Flange tool is a sketch-based feature (using an open profile) that has the ability to create multiple planar faces and bends as the result of a single feature, as shown in Figure 6.2. Profile sketches should contain only arcs and lines; if sketch intersections are not separated by an arc, a bend equal to the BendRadius parameter will automatically be added at the intersection, as determined by the sheet-metal rule. To create base features with a profile sketch, contour flanges have a width extent option called Distance, which allows a simple open profile to be utilized to create a sheet-metal condition extrusion of the thickened, filleted profile.

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Figure 6.2 Contour Flange base feature

You can use the Contour Flange tool to create sheet-metal base features; in fact, it is often the fastest way to create them. Although you could create the part shown in Figure 6.2 by using the Face tool and then adding flanges, it would be more time-consuming. Using the Contour Flange tool has one drawback, however: Since you are combining many features, you lose some flexibility for revising the shape.

Follow these steps to explore the basics of creating a base feature with the Contour Flange tool:

1.  Click the Get Started tab and choose Open.

2.  Open the file named mi_6a_001.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder. If you have not already downloaded the Chapter 6 files from www.sybex.com/go/masteringinventor2015, please refer to the “What You Will Need” section of the introduction for the download and setup instructions.

3.  Select the Contour Flange tool from the Create panel of the Sheet Metal tab.

4.  For the Profile selection, click anywhere along the sketch profile.

Depending on where you clicked on the sketch, the preview will show either the outside or inside of the sketch. Also notice that the corners at each end of the 25 mm leg are automatically rounded even though no radius was specified in the sketch. This is because of the predefined BendRadius parameter.

5.  Use the Flip Side buttons (three arrow buttons) to change the preview so you can see how each changes the result. Then set the side so that the preview is to the inside of the sketch profile (as in Figure 6.2) and therefore holding the overall dimensions of the sketch.

6.  Enter 6 mm in the Bend Radius input box, and notice that the corners at each end of the 25 mm leg are updated.

Entering a value in the Bend Radius input box overrides the predefined BendRadius parameter and sets this contour flange feature to always use 6 mm. If the part were set to use another predefined style, bends in this feature would not update to follow the style but would instead stay at 6 mm.

7.  Click the button to expand the Contour Flange dialog box (if it isn't already expanded) and then set the Distance input box to 150 mm.

8.  Use the ViewCube® to change the view so you can see the direction of the contour.

9.  Click the Distance Mid-Plane button so the part is created equally to both sides of the sketch.

10.Click the OK button to create the feature.

In the preceding steps you created a base feature using an open profile sketch and the Contour Flange tool. From this point, you could begin adding secondary features as required. For now, though, you can close this file without saving changes and continue looking at other tools used to create base features.

Contour Roll Tool

The Contour Roll tool is a variation of the Contour Flange tool. To create a contour roll, you sketch an open profile, but you revolve it instead of extruding it. Sketch geometry is limited to lines and arcs, and the Contour Roll tool will automatically add a bend at line intersections. The rolled hat flange in Figure 6.3 was created using the simple sketch geometry shown.

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Figure 6.3 Contour Roll base feature

Follow these steps to explore the basics of creating a base feature with the Contour Roll tool:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_002.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Contour Roll tool from the Create panel of the Sheet Metal tab.

4.  Set the Unroll Method drop-down box to Centroid Cylinder if it is not already. For the Profile selection, click anywhere along the sketch profile.

5.  Select the centerline for the Axis selection.

Note the options in the Unroll Method drop-down box:

1.  Centroid Cylinder The neutral cylindrical surface is derived by the centroid location of the profile, based on the selected axis. The neutral radius and unrolled length are displayed.

2.  Custom Cylinder This allows you to select a sketched line to define the cylindrical neutral surface. The unrolled length is displayed.

3.  Developed Length This allows you to enter the developed length and displays the adjusted neutral radius.

4.  Neutral Radius This allows you to enter the neutral radius and displays the adjusted unrolled length.

These options all derive the developed length by multiplying the rolled angle by a neutral radius but differ from one another by the type of input specified.

6.  Set the unroll method to Custom Cylinder and select the sketch line denoted as Custom Neutral Axis for the Neutral Axis selection. Note the displayed unrolled length.

7.  Set the unroll method to Neutral Radius and enter 60 mm in the input box. You'll notice that the displayed unrolled length adjusts based on the change.

8.  Set the unroll method to Developed Length and enter 100 mm in the input box. You'll notice that the displayed neutral radius adjusts based on the change.

9.  Click the OK button to create the feature.

10.Click the Create Flat Pattern button on the Sheet Metal tab.

11.Right-click the Flat Pattern node in the browser and choose Extents. You'll see that the width of the flat pattern has been held to 100 mm, honoring your final input value.

12.Click the Close button in the Flat Pattern Extents dialog box and then deselect the Flat Pattern node in the browser (you can do so by clicking on-screen anywhere in the graphics area).

13.Click the Go To Folded Part button on the Sheet Metal tab to return to the folded model.

In the preceding steps you created a base feature using an open profile sketch and the Contour Roll tool. You can close this file without saving changes and continue looking at other tools used to create base features. Before continuing, though, you can open the filemi_6a_003.ipt to create a secondary contour roll feature based on the first.

Lofted Flange Tool

The Lofted Flange tool creates sheet-metal shapes typically seen in HVAC transitions and material-handling hoppers. Figure 6.4 shows a square-to-round transition. Basically, you create sketches of the beginning and end of the transition and then use the Lofted Flange tool to transition between the two. The Lofted Flange tool gives you the option of a die form or a press brake transition. For press brake transitions, you can define the bends by chord tolerance, facet angle, or facet distance. The chord tolerance is the distance between the angled face and the theoretical curved surface. As the chord tolerance is decreased, more facets are added.

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Figure 6.4 Square-to-round lofted flange

To create a lofted flange, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_004.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Click the Lofted Flange button in the Create panel.

4.  Select the square and the circle for the profile selections.

5.  In the output area of the dialog box, click the Die Formed button, and note that the preview changes to remove the press brake facets and that the facet controls in the dialog box are hidden.

6.  Click the Press Brake button and use the Facet Control drop-down to experiment with the Chord Tolerance, Facet Angle, and Facet Distance options to familiarize yourself with their behavior.

Chord Tolerance This value sets the maximum separation distance from the arc segment to the chord segment.

Facet Angle This value sets the maximum angle to the chord segment at the facet face vertex.

Facet Distance This value sets the maximum width of the length of the chord.

Converge This check box sets the bends of the flattened faceted sections to converge near a singular point.

Deciding which of these options to use depends largely on the design inputs you know and the equipment to be used to create the part on the shop floor.

7.  Ensure that the Converge check box is not selected, set the Facet Control drop-down to Facet Distance, and change the distance to 50 mm.

Note that there is a glyph icon at each of the transition corners on the model preview. If you hover your cursor over them, you can see them better. Clicking one of these Bend Zone Edit glyphs displays a dialog box to change the facet control and also displays individual glyphs for each bend. The Bend Zone Edit dialog box enables you to change the facet control for the corner corresponding to the glyph you clicked, as shown in Figure 6.5. Clicking one of the bend glyphs displays a Bend Zone Edit dialog box that enables you to override the bend radius and unfold rule for an individual bend.

Continuing with the previous steps, investigate the use of Bend Zone Edit glyphs for yourself with these steps:

8.  Click one of the Bend Zone Edit glyphs.

9.  Click the check box in the Bend Zone Edit dialog box and select Number Of Facets.

10.Enter 2 in the edit field and note that the preview updates.

11.Click one of the Bend Edit glyphs and then click the Bend Radius check box in the resulting Bend Edit dialog box.

12.Change the bend radius to BendRadius*10 and note the preview.

13.Click the OK button and note that the Bend Edit glyph has changed. A pencil is added to indicate that it has been overridden.

14.Click the OK button in the Bend Zone Edit dialog box. Hover your cursor over the glyph and note that a pencil has been added to it as well.

15.Click the OK button in the Lofted Flange dialog box to create the feature.

16.Click the Create Flat Pattern button on the Sheet Metal tab. Note that the part isn't flattened because it is a continuous piece.

17.Click the Go To Folded Part button on the Sheet Metal tab to return to the folded model.

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Figure 6.5 Bend Zone Edit dialog box

To get the lofted flange transition to flatten, you'll need to create a rip feature in one of the faces. The Rip tool will be discussed in the section “Adding, Removing, or Deforming Material” later in this chapter. For now, you can close the file without saving changes and continue to the next section to explore the creation of flanges.

Creating Secondary Flange Features

Once a base feature is created, you can add secondary features in the form of flanges. Flanges are planar faces connected by a bend and can be created using a number of tools. The Flange tool automatically creates bends between the flanges and the selected faces. You can also use the Contour Flange tool to create several flanges at once. The Hem tool allows you to create specialized flanges to hem sharp edges or to create rolled flange features. Another tool commonly used along with these tools is the Face tool. Depending on the selected tool, you can either control flange options or allow Inventor to apply predefined relationships and values.

Flange Tool

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The Flange tool creates a single planar face and bend for each edge selected, with controls for defining the flange height, bend position, and relief options at the edge intersections. For flanges referencing a single edge, width extent options are also available by clicking the button in the Flange dialog box. If multiple edges have been selected for flange locations, corner seams are automatically added, as shown in Figure 6.6. The bend and corner seam dimensions follow the sheet-metal rule unless a value is entered to override them per that particular feature. The preview displays glyphs at each bend and corner seam. If you click a glyph, a dialog box appears so you can override the values.

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Figure 6.6 A multi-edge flange feature preview with bend and corner edit glyphs

Creating Basic Flanges

To explore the Flange tool, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_005.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Flange tool from the Create panel of the Sheet Metal tab.

4.  Currently the Edge Select Mode button (on the left side of the Edges selection box) is selected, allowing you to select only one edge at a time. Click the Loop Select Mode button so you can select multiple edges at once.

5.  Place your cursor over the top face of the hexagonal-shaped base feature. Click the edge when you see all six edges highlight. Note that if you chose the bottom edge rather than the top, you can use the Flip Direction button to change the direction.

6.  Click the Edge Select Mode button and then hold the Ctrl key and click one of the currently selected edges to deselect it. The Edges selection box will indicate that you now have only five selected.

7.  Set the flange height to 100 mm.

8.  Set the flange angle to 60.

9.  Click the Corner tab, uncheck the Apply Auto-Mitering check box to observe the preview change, and then reselect the check box to allow the flanges to flare out into the mitered corners.

10.In the Miter Gap input box, enter 1 mm to reduce the gap size from the current default value (the GapSize parameter is currently set at 3 mm in the sheet-metal rule).

11.Click the Apply button to create the five flanges and leave the Flange dialog box open (recall that clicking the OK button creates the feature and closes the dialog box, and clicking Apply creates the feature but does not close the dialog box).

12.Click the Shape tab and ensure that the Edge Select Mode button is selected.

13.Click the edge that you removed from the previous selection set. Note that if you chose the bottom edge rather than the top, you can use the Flip Direction button to change the direction.

14.Set Flange Angle to 90.

15.Set the Height Extents drop-down box to To and then click the topmost corner vertex of any of the existing flanges. Figure 6.7 shows the To point being selected.

16.Click the OK button to create the flange.

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Figure 6.7 Setting a flange height using the To option

If you click the front plane on the ViewCube, you can see that all the flanges terminate in the same plane. Keep this in mind as you create flanges of varying angles. You will explore the tools used to close the remaining gaps in this flange combination later in this chapter, when looking at the Corner Seam tool, but for now you can close the file without saving changes and continue to explore the Flange tool.

Control Flange Widths

In this next set of steps, you'll create flanges of varying widths by adjusting the extents options.

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_006.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Flange tool from the Create panel of the Sheet Metal tab.

4.  Select the top edge of the yellow face to place a flange along the edge.

5.  Set the flange height to 50 mm and leave the angle at 90 degrees.

Note that currently the flange runs along the extents of the edge. If you imagine the flat pattern that would result from adding this flange, you'll understand that creating this flange would create a conflict at the inside corner. Although Inventor will not prevent you from creating the flange as is, it will issue an error to the flat pattern. To resolve this, you will set the flange width and an offset to hold it back from the corner. There are four possible Width Extents settings:

1.  Edge Runs the flange the length of the selected edge

2.  Width Allows you to specify the width of the flange and position it centered on the selected edge or offset from a selected reference point

3.  Offset Allows you to specify offsets from both ends of the selected edge

4.  From To Allows you to specify a start and end reference to establish the flange width

In the real world, the option you use will depend on the result you are trying to achieve and the available existing geometry. Here, you'll use the Width option.

6.  Click the button to expand the Flange dialog box.

7.  Change Width Extents Type to Width.

8.  Enter 96 mm in the Width input box.

9.  Switch the option from Centered to Offset.

10.Enter 0 mm for the offset value.

11.Click the end of the selected edge farthest from the green face to establish the offset point. Use the Offset Flip button to redirect the flange if needed.

12.Click the OK button to create the flange.

13.Click the Go To Flat Pattern button on the Sheet Metal tab to have a look at the resulting flat pattern.

Although the flange width options are easy to overlook because they are initially hidden in the More Options area of the dialog box, you should keep them in mind as you create flanges. For now, you can close this file without saving changes. Here are more options to be aware of when creating flanges:

1.  Flange Height Datum There are three Height Datum solutions available. These options control which faces are used to determine the height measurement. In Figure 6.8, each of the options is shown using a 40 mm flange.

1.  Bend From The Intersection Of The Two Outer Faces Measures the flange height from the intersection of the outer faces, as shown on the left in Figure 6.8

2.  Bend From The Intersection Of The Two Inner Faces Measures the flange height from the intersection of the inner faces, as shown in the center in Figure 6.8

3.  Parallel To The Flange Termination Detail Face Measures the flange height parallel to the flange face and tangent to the bend, as shown on the right in Figure 6.8

2.  Orthogonal and Aligned Flanges You can use the Aligned VS Orthogonal toggle button to determine whether the height measurement is aligned with the flange face or orthogonal to the base face. In Figure 6.9, the flange on the left is orthogonal, and the measurement on the right is aligned.

3.  Bend Position There are four options to select from to determine the bend position relative to the face of the selected edge. Figure 6.10 compares the four options, with the dashed line representing the selected edge of the base feature.

1.  Inside Of Base Face Extents Positions the flange so that it honors the overall dimension of the selected base part, as shown on the far left of Figure 6.10

2.  Bend From Adjacent Face Holds the face of the selected edge as the start of the bend, as shown on the center left of Figure 6.10

3.  Outside Of Base Face Extents Positions the inside face of the flange so that it remains outside of the face of the selected edge, as shown on the center right of Figure 6.10

4.  Bend Tangent To Side Face Holds the bend tangent to the face of the selected edge, as shown on the far right of Figure 6.10

4.  Old Method When checked, this option disables the functionality introduced in the Autodesk® Inventor® 2008 program. If you open a file created in an older version, the features will likely have this option selected. You can uncheck the box to update the file to use all the available options. There is no reason to check this box on parts that you create with the current version of Inventor.

5.  Bend and Corner Edit Glyphs Although you will often create flanges along multiple edges as a single flange feature, you can still control the bend and corner options individually by using the edit glyphs displayed on the features in the graphics area. You can access the edit glyphs by expanding the Flange node in the browser and then right-clicking the bend or corner and choosing Edit Bend or Edit Corner. Once they are displayed, you can click the edit glyph for the bend or corner you want to edit and make changes on an individual basis. You can click the edit glyphs during the creation of flanges as well. Once bends or corners are edited, they can be reset to the defaults by expanding the Flange node in the browser, right-clicking the bend or corner, and choosing Reset All Bends/Corners.

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Figure 6.8 Flange height datum solutions

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Figure 6.9 Orthogonal and aligned flanges

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Figure 6.10 Bend positions compared

Contour Flange Tool

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In addition to creating base features as explored previously, the Contour Flange tool can be used to add flanges to an existing feature. Since the Contour Flange tool uses open profile sketches, it is ideal for quickly creating complex shapes and enclosure designs. As discussed earlier, the Contour Flange tool can either automatically bend line intersections or use sketched arcs for bends. A contour flange automatically creates a bend between itself and a selected edge on an existing face. The sketch profile for the Contour Flange tool does not need to be coincident with the edge; it simply needs to be sketched on a plane that is perpendicular to it. If the sketch profile is coincident with an edge, a bend will automatically be positioned to connect the sketch profile to the face. If the sketch is not coincident with a reference edge and the width extent option is changed to Distance, the result will be a contour flange that isn't attached to the part.

Just as with the Flange feature, automatic mitering of adjacent flanges and the placement of corner reliefs occur when multiple edges are selected, as shown in Figure 6.11.

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Figure 6.11 A multi-edge Contour Flange feature with automatic mitering and large radius bends

To explore the Contour Flange tool a bit more, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_007.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Contour Flange tool from the Create panel of the Sheet Metal tab.

4.  Select the visible sketch profile as the Profile selection.

5.  Select one of the edges (top or bottom) that have the two work planes running through it.

You'll note that you cannot add any more edges to the selection. This is because the sketch is disconnected from the base feature and therefore can be used only to create a flange along the one edge. Next, you'll use the work planes to define the width of the flange.

6.  Click the button to expand the dialog box and reveal the Width Extents options.

7.  Set the Type drop-down box to From To.

8.  Select the two visible work planes as the From and To selections.

9.  In the Bend Extensions area, click the left button (Extend Bend Aligned To Side Faces).

10.Click the OK button to create the contour flange.

You should notice that the flange width starts and stops at the work planes selected for the width extents. You'll also notice that the edge of the base feature extends to meet the flange. This is because of the Bend Extension option. The Bend Extension options are as follows:

Extend Bend Aligned To Side Faces Extends the base feature to meet the flange.

Extend Bend Perpendicular To Side Faces Extends the flange to meet the base feature. This is the default.

You'll explore these options a bit more in the upcoming pages, but for now you'll edit the flange and toggle this option to compare the results.

11.Right-click the Contour Flange feature in the browser and choose Edit Feature.

12.In the Bend Extensions area, click the right button (Extend Bend Perpendicular To Side Faces).

13.Click the OK button, and note that the flange has now extended to the base feature, as shown on the right of Figure 6.12.

14.Right-click Sketch3 in the browser and turn on the visibility.

15.Select the Contour Flange tool from the Create panel of the Sheet Metal tab.

16.Select the sketch profile in Sketch3 as the Profile selection.

17.Select the five edges of the hex-shaped face that were not used in the previous contour flange.

18.Notice the automatic mitering of the corners; if this was not the desired result, you could disable the Apply Auto-Mitering check box option on the Corner tab.

19.Click the OK button to create the flanges.

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Figure 6.12 Bend Extension options

As you can see, the Contour Flange tool can be used to quickly create multiple bend flanges from a basic open profile sketch. This is often the quickest way to create even simple flanges when they are the same on all edges of a base feature, particularly when the flanges require a miter fit. You can close this file without saving changes and continue to the next section to explore hems.

Hem Tool

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The Hem tool is like a contour flange because it has the ability to create multiple planar faces and bends for a selected edge, but it is restricted to predefined common hem profiles and geometric relationships.

To explore the different hem flange types and options, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_008.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

In this file, each of the four hem types has been created on one side of the part. You can use the cutouts on the other side to create a hem matching each of the ones on the left. Once you have experimented with the hem types using the cutouts, proceed to create a hem on the edge of the yellow face.

3.  Use the ViewCube to find a view of the yellow interior face.

4.  Select the Hem tool from the Create panel of the Sheet Metal tab.

5.  Set Type to Single.

6.  Select the edge along the outside of the yellow face.

7.  Set Gap to 2 mm.

8.  Set Length to 12 mm.

9.  Click the button to expand the dialog box.

10.Change Width Extents Type to Offset.

11.Use the appropriate offset input box to set the end that will interfere with the existing hem to 5 mm.

12.Set the other offset to 0 mm so that no offset is created.

13.Click the OK button to create the Hem flange.

Although the Hem tools are fairly straightforward, it is often the use of offsets that allows you to place hems as needed. You can close this file without saving changes and continue to the next section.

Face Tool

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The last feature capable of creating flanges is the Face tool. The Face tool uses a closed profile sketch, and it can automatically create an attaching bend on a selected edge. This automatic edge creation is powerful because it allows you to create a skeletal surface model of your design, project the planar surfaces into sketches, and create face features with attached bends. The manual controls can be utilized to connect face features to preexisting geometry, create double bends (joggles), or even deselect edges that have been automatically inferred because they share a common edge.

You can also use the Face tool to create models from 2D flat patterns that were created in another application, such as Autodesk® AutoCAD®. When the 2D flat pattern is imported, the Face tool can be used to thicken it to the desired value. A flat pattern can be produced for a planar face (no unfolding needs to actually occur), which enables a variety of uses.

In the following steps, you'll derive a frame into your sheet-metal part and use it as a reference to create a face. You'll then create another face and use the built-in Bend tools to connect them.

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_009.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Manage tab and click the Derive button on the Insert panel.

4.  Open the file mi_6a_888.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

5.  In the Derived Part dialog box, select the Body As Work Surface button at the top. This brings the frame in as a surface that can be turned off later.

6.  Click the OK button to create the frame surface.

7.  Expand the mi_6a_888 node in the browser and right-click the Frame:mi_6a_888.ipt node.

8.  From the context menu, deselect the Translucent option. This will make the frame edges easier to see.

9.  Right-click the face of the frame side with the triangular corner gussets and choose New Sketch to create a 2D sketch on the side of the frame.

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Click the Project Geometry drop-down menu and select Project Cut Edges. This will project the face of the frame into the sketch. Alternatively, you can use the Project Geometry tool and select the four outer edges and the eight holes.

11.Once the projected edges are created, click the Finish Sketch button to return to the Sheet Metal tab.

12.From the Sheet Metal tab, select the Face button.

13.Choose the sketch boundary (or boundaries) so that the entire side of the frame, minus the holes, is selected.

14.Ensure that the face is not going into the frame, use the Offset button if the direction needs to be adjusted, and then click the OK button to create the face feature with holes. Figure 6.13 shows the frame and face.

15.Locate the sketch called Flange Sketch in the browser and then right-click it and choose Visibility from the context menu. This sketch was prepared in the sheet-metal file ahead of time for this tutorial, but in the real world you would create it by referencing the frame as you did for the first face feature.

16.On the Sheet Metal tab, select the Face tool again and choose the rectangular profile minus the slots as the Profile selection.

17.Use the Offset button to ensure that the face is coming out away from the frame.

18.Click the Edges button in the Bend area of the dialog box and then select the left vertical edge of the first face feature. This will create a bend connecting to two faces.

19.Click the OK button to create the new face with the bend feature.

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Figure 6.13 Face from a derived frame

If you examine the slotted flange face, you might notice that it does not rest on the face of the frame. This is because the premade sketch that you made visible was created on a work plane at 302 mm from the center of the 600 mm–wide frame. Using the offset work plane, a 2 mm gap was created, allowing space for the bend radius, insert studs, and spacer hardware that might be required.

Be aware that when you have finished with a derived work surface (the frame in this case), you can right-click it in the browser and toggle off the visibility. This leaves only the sheet-metal part showing. To create the next sheet-metal part of the frame, such as the front or back covering, you would create a new sheet-metal part and derive the frame again. Once all of the parts are complete, you can place them into an assembly file knowing that they will all fit around the frame they were based on. For now, though, you can close this file without saving changes and continue to the next section.

Adding, Removing, or Deforming Material

Once the general shape of a sheet-metal component is roughed in, in most cases material will need to be removed, deformed, or added. Several sheet-metal-specific features have been created to optimize the process of adding, removing, and deforming sheet-metal parts because most sheet-metal-manufacturing operations (punch presses, for example) create features perpendicular to the surface. The current capabilities of Inventor assume that these manufacturing operations are done in the flat prior to folding and therefore should not interfere with unfolding (Inventor does not support post-folding manufacturing operations such as gussets, for example).

Cut Tool

The Cut tool is a special sheet-metal extrude. It creates a hole based on a sketched profile. The Cut tool helps simplify the options of the regular Extrude tool because the distance parameter defaults to Thickness, and therefore cut features automatically update if the sheet-metal part is changed to use a different material thickness. If a cut is not intended to be the full depth of the material thickness, you can enter an equation based on the thickness value, such as Thickness/2 to create half-thickness cuts.

Creating Cuts Across Sheet Metal Bends

The Cut tool can also wrap the sketch profile across planar faces and bends, as shown in Figure 6.14. This option is particularly helpful because it allows you to force a uniform cut across multiple planar faces and bends with a value greater than zero and equal to or less than Thickness.

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Figure 6.14 The cut feature using the Cut Across Bend option

Using Cuts

With sheet-metal parts, it is often best to create your base features and flanges and then apply the cuts as required. You will find that this provides a more stable model when creating a flat pattern and allows you to edit features individually. It's generally best practice to use the Cut tool whenever possible rather than creating voids in the base sketch.

To explore the options of the Cut tool, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_010.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  In the browser ensure that the view representation named Top Slot View is active. If it is not, simply expand the View browser node and double-click the Top Slot View node.

4.  Select the Cut tool from the Modify panel of the Sheet Metal tab.

5.  Click the OK button to create the cut feature. Note how the cut remains only in the top plane and is not accurate for a slot that would be cut in the flat pattern.

6.  Right-click the cut feature in the browser and choose Edit Feature.

7.  Select the Cut Across Bend check box, note the preview, and then click the OK button to create the cut feature. You'll notice that it cuts through the part and across the existing bends.

8.  Click the Go To Flat Pattern button on the Sheet Metal tab to examine the slot cut in the flat pattern. You'll notice that the cut edges are normal to the flat sheet as expected.

9.  Click the Go To Folded Part button on the Sheet Metal tab to return to the folded model.

10.Edit the cut feature again, enter Thickness/2 in the Distance input box under Extents, and then click the OK button.

As you can see, the Cut tool allows you to create partial depth cutouts across bends as well. Using the Cut Across Bend option allows cut features to be created in the formed part model that are accurate to the way the cutout is created in the flat pattern, and then bent in the finished folded part, just as would be done in the real world.

You can leave this file open and continue to the next exercise to explore the creation of angled cuts held normal to the sheet-metal flat pattern.

Creating Angled Features Cut Normal to the Flat Pattern

To create angled cuts held normal to the sheet-metal flat pattern, follow these steps:

1.  If you do not already have file mi_6a_010.ipt open, then click the Get Started tab and choose Open; then select the file mi_6a_010.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

2.  In the browser, ensure that the view representation named Rod View is active. If it is not, simply expand the View browser node and double-click the Rod View node.

You'll see a yellow surface representing a keyed rod that runs through the sheet-metal bracket. Your goal is to create a cut feature in the bracket that allows the rod to fit through.

3.  Select the Cut tool from the Modify panel of the Sheet Metal tab. The Profile shape should be automatically selected for you since there is only one visible sketch available (the Rod CutOut sketch).

4.  Set the Extents drop-down box from Distance to All.

5.  Set the Direction button to go in both directions.

6.  Click the OK button to create the cut feature.

7.  Click the Go To Flat Pattern button on the Sheet Metal tab to examine the cuts in the flat pattern. You'll notice that the cut edges have bevels and are not normal to the flat sheet as you would want them to be if the cutouts were to be punched or laser cut.

8.  Click the Go To Folded Part button on the Sheet Metal tab to return to the folded model.

9.  Right-click the cut feature in the browser and choose Edit Feature.

10.Select the Cut Normal check box and then click the OK button.

11.Click the Go To Flat Pattern button on the Sheet Metal tab again and notice the cuts in the flat pattern no longer have the beveled edges.

These exercises demonstrate the use of the Cut Across Bend and Cut Normal options in the Cut tool. As a general rule, you should use the Cut tool to create cutouts in a sheet-metal part file, rather than the Extrude tool as you would in a standard part file. When you've finished exploring the Cut tool, you can close this file and continue to the next section.

Punch Tool

You can use the Punch tool to either remove material or deform it by placing predefined Punch tool geometry, as shown in Figure 6.15. Punches are special versions of iFeatures; they can be predefined with additional manufacturing information and can be built using a variety of standard and sheet-metal features.

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Figure 6.15 Multiple-instance punch feature placing a footing dimple

To explore the methods and options used to place punch features, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_011.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Click the Punch Tool button on the Modify panel of the Sheet Metal tab.

4.  In the Punch Tool dialog box, use the scroll bar in the left window to locate the Chapter 6 folder.

5.  Locate and select the file Knockout_73x.ide and then click the Open button.

Setting the Sheet-Metal Punch Tool Default Location

By default, Inventor is set to look for the punch library in the install directory on your local drive. If you're working on a network share drive, you will most likely want to point the Punch tool to automatically go to a path on the network. To do so, click the Application Options button on the Tools tab, select the iFeature tab, and set Sheet Metal Punches Root to the path of your choosing.

6.  Because this part has two visible sketches, no centers are automatically selected. Select any one of the center sketch points on the part.

7.  Continue selecting center points, and note that you can select only points that share the same sketch. Sketch2 contains three sketch points, toward one end of the part, and Sketch3 contains five sketch points grouped together at the other end.

Window-Select Multiple Punch Center Points

You can use a crossing window selection to select multiple punch center points at once. A window selection from left to right will select only items contained in the window. A window selection from right to left will select all items that touch the window or are contained in the window. If you window-select an item already selected, it will be removed from the selection set. Note, too, that you can hold the Ctrl key and select in empty space to clear the selection set.

8.  When you have added all of the center points you can (it will be either three or five, depending on which sketch the points are in), select the Size tab.

9.  Enter 35 mm for the diameter value and then click in the space below the Diameter row in the dialog box.

10.Click the Refresh button to see the diameter update on-screen. Note that if the diameter does not update, you probably did not click out of the Diameter row to set the edit. The Refresh option is a bit picky in this way. Keep in mind, however, that the punch preview does not need to be refreshed to build correctly.

11.Click the Finish button to create the punches.

12.Right-click and choose Repeat Punch Tool; then, in the Punch Tool dialog box, use the scroll bar in the left window to locate the Chapter 6 folder.

13.Once again, locate and select the file called Knockout_73x.ide; then click the Open button.

14.You'll notice that because you have only one visible sketch now, all of the center points in the sketch are automatically selected.

15.Click the Geometry tab and then click the Centers button.

16.Press and hold the Ctrl key on the keyboard and then deselect any one of the selected center points by clicking it in the sketch. Note that it is often easier to do this when viewing the sketch from straight on.

17.With all but one of the available center points selected, change Angle to 45 degrees. Note that all of the current punches are rotated.

18.Click Finish to create the punches.

19.Locate the sketch with the unused sketch point in the browser; then right-click it and choose Visibility to turn it back on.

20.Right-click and choose Repeat PunchTool; then in the Punch Tool dialog box, use the scroll bar in the left window to locate the Chapter 6 folder.

21.Locate and select the file Knockout_73x.ide and then click the Open button.

22.The final center point should be automatically selected. If not, select it and then click Finish to create it at the default size and orientation.

You can close this file without saving changes, but before moving on to the next topic, take a moment to understand how punch placement sketches and punch features work. In the preceding steps, you explored the options and methods used to place sheet-metal punches on an existing sketch. The process of applying a published Punch tool to your sheet-metal design is fairly straightforward. When you're authoring a Punch tool, the first sketch-based feature referenced to create the Punch tool must contain a single sketched center mark. To place a Punch tool, at least one sketched center mark is required in the placement sketch. Creating punch features (and regular iFeatures) is covered in Chapter 7, “Reusing Parts and Features.”

Corner Round and Corner Chamfer

Corner Round and Corner Chamfer are special sheet-metal tools that allow you to remove or break sharp edges, similar to filleting and chamfering. Edge selection has been optimized within the two tools, filtering out edges that are not normal to the sheet top and bottom faces for easy application. To explore the methods and options used to place round and chamfer features, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_012.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Corner Round tool on the Modify panel of the Sheet Metal tab.

4.  Set the radius to 8 mm and then click the Pencil icon in the Corner Round dialog box to change the focus from edit to select.

5.  Select the two sharp corner edges on the green flange and then click the OK button.

6.  Right-click and choose Repeat Corner Round and then set the Select Mode radio button to Feature.

7.  Select any of the yellow flanges, and you will see that all of the sharp corners for the feature called Flange1 are automatically selected.

8.  Change the radius to 15 mm and then click the OK button to create the rounds.

9.  Select the Corner Chamfer tool from the Modify panel of the Sheet Metal tab.

10.Select the remaining two sharp corners and set the distance to 18 mm. Click the OK button to create the corners.

As a final step you might want to right-click Flange1 in the browser, choose Properties, and set Feature Color Style to As Part. You can do the same to Flange2. When finished, you can close the file without saving the changes and continue to the next section.

Corner Seam Tool

The Corner Seam tool allows you to extend (as shown in Figure 6.16) or trim flange faces to manage the seam between them and select corner relief options. The Corner Seam dialog box contains numerous options for specifying the seam and contains two fundamentally different distance definition methods: Maximum Gap and Face/Edge. In older versions of Inventor, only the Face/Edge method was available for the Corner Seam tool. The Face/Edge method works for many situations but also tends to suffer from an inability to maintain a constant seam gap between planar faces that do not have an identical input angle. The Maximum Gap method was developed from the perspective of a physical inspection gauge, where the nominal value of the seam is exactly the value entered at every point, but you just might need to twist the tool as you draw it through the seam.

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Figure 6.16 The Corner Seam feature, applying the No Overlap seam type

Creating a Basic Corner Seam

To explore the Corner Seam tool and its options, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_013.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Corner Seam tool on the Modify panel of the Sheet Metal tab.

4.  Select the left edge of the yellow face and either edge of the blue face next to it. In the preview, the red edges represent the material to be removed and the green edges represent the material to be added.

5.  In the Seam area of the Corner Seam dialog box, select the Symmetric Gap option if it's not already selected.

6.  Set the gap to 1 mm and notice the change to the preview.

7.  Click the Apply button to create the seam feature.

8.  Select the right edge of the orange face and either edge of the blue face next to it and then click the OK button to create this seam and close the dialog box.

As you can see, corner seams are useful when you need to close up a corner between two seams. You can close this file without saving changes and continue with the next set of steps to explore more of the settings in the Corner Seam tool.

Understanding Corner Seam Gap and Overlap Settings

In these steps, you'll explore the gap and overlap settings found in the Corner Seam tool:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_014.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Corner Seam tool on the Modify panel of the Sheet Metal tab.

4.  Select the short edge of the orange flange nearest the yellow flange and the short edge of the yellow flange nearest the orange flange.

5.  You'll note that the preview shows that the two flanges come together in a 45-degree miter. Click the Overlap button to see the preview change to extend one of the flanges so it overlaps the other.

6.  Click the Reverse Overlap button to see the opposite overlap in the preview.

7.  Click the Apply button to create the seam.

8.  Click a short edge of the yellow flange nearest the blue flange and a short edge of the blue flange nearest the yellow flange.

9.  Set the Seam option to Maximum Gap Distance (if it is not already) and click the Symmetric Gap button.

10.Click the OK button to create the corner seam and then click the top face on the ViewCube to observe the corner of the yellow and blue flanges. Note that it may be helpful to zoom up on the corner.

If you measure the gap distance at the inside vertices between the two flanges, it will be 3 mm, which is what the Gap parameter is set to, as shown on the left of Figure 6.17.

11.Edit the corner feature you just created, switch the radio button to Face/Edge Distance, and then click the OK button.

Now the Gap parameter holds the distance between the face and edge of the two flanges, as shown on the right of Figure 6.17.

12.Edit the corner feature again, and this time click the Overlap button.

13.Enter 0.5 in the Percent Overlap input box and then click the OK button.

You will see that the yellow flange overlaps the edge of the blue flange exactly halfway, or 50 percent. You can specify the overlap as a percentage of the flange thickness using a decimal value ranging from 0.0 to 1.0. For instance, 1.0 equals 100 percent, 0.5 equals 50 percent, and so on.

14.Edit the corner feature once again and click the Reverse Overlap button.

15.Enter 1.0 in the Percent Overlap input box and then click the OK button.

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Figure 6.17 Maximum Gap Distance compared to Face/Edge Distance

You will see that the blue flange now overlaps the yellow flange completely, or the full 100 percent. Figure 6.18 shows a comparison of overlap values with the same gap setting of 3 mm. On the left the overlap is set to 1.0, or 100 percent of the 3 mm gap. In the middle the overlap is set to 0.5, or 50 percent of the 3 mm gap. And on the right the overlap is set to 0.0, or 0 percent of the 3 mm gap.

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Figure 6.18 Overlap comparisons

In the previous steps you explored the gap and overlap settings of the Corner Seam tool. You can close this file without saving changes and continue with the next set of steps to explore one more set of options in the Corner Seam tool.

Understanding Corner Seam Extend Options

In the following steps, you will look at the options for controlling the way flanges are extended when their edges are not perpendicular:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_015.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Corner Seam tool on the Modify panel of the Sheet Metal tab.

4.  Select the shorter edge of the blue flange and the closest edge of the yellow flange.

5.  Click the button in the Corner Seam dialog box and set the Extend Corner option to Perpendicular; then click the Apply button.

6.  Select the taller edge of the blue flange and the closest edge of the orange flange.

7.  Click the button in the Corner Seam dialog box again (if needed) and toggle the Extend Corner option between Perpendicular and Aligned to see the difference.

8.  Set the Extend Corner option to Perpendicular and click the OK button.

Figure 6.19 shows a comparison of the Perpendicular and Aligned extend options. In the image on the right, the frontmost flange uses the Aligned solution and the other uses the Perpendicular solution.

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Figure 6.19 Perpendicular and Aligned extend corner options

As you can see, becoming familiar with all the settings in the Corner Seam tool can make you aware of a great number of combinations and in the end provide the exact corner you are trying to achieve. You can close this file without saving changes and continue on to explore the Fold tool.

Fold Tool

The Fold tool enables you to design a flange with a unique profile by allowing you to sketch the position of the bend centerline on a planar face and then fold the part using the sketch line, as shown in Figure 6.20.

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Figure 6.20 The Fold tool being applied to a face with a spline contour

This tool is a sketch consumption feature and contains numerous controls for specifying exactly how a planar face should be manipulated into two planar faces connected by a bend. The sketch bend centerline must be coincident with the face extents, requiring you to project edges and constrain the sketch. When utilizing the Fold tool, remember that the feature works from the opposite design perspective of other sheet-metal features, where bend allowance is actually consumed, not added to the resulting folded feature. The Fold tool can be combined with the Face tool to help import preexisting 2D flat patterns and then deform them into their final shape.

To explore the Fold tool, follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_016.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Fold tool on the Create panel of the Sheet Metal tab. (Be aware that there is an Unfold button and a Refold button as well. You will explore those in the coming pages, but for now ensure that you select the Fold tool.)

4.  Select the visible sketch line on the circular feature for the Bend Line selection.

5.  Use the Flip Side and Flip Direction buttons to set the preview arrows so that they are going up and out from the center of the part.

6.  Set Fold Angle to 45 (degrees) and Bend Radius to 16 mm.

7.  Use the Fold Location buttons to set the fold so that it does not include the cutout.

8.  Click the OK button to create the folded feature.

9.  To reuse the sketch containing the bend lines, you'll need to make it visible again. To do so, expand the Fold feature in the browser, right-click the sketch, and choose Visibility from the context menu.

10.Create a fold for each of the remaining lines, setting Fold Angle to 90, Bend Radius to 2 mm, and Fold Location to Centerline Ff Bend. Use the flip controls to set the folds so they are all going up and out from the center of the part.

Although not the most commonly used of the sheet-metal tools, the Fold tool can be useful in some circumstances. If you happen to have a lot of flat pattern drawings done in AutoCAD, for instance, you can use the Fold tool to convert them to folded models. You can close this file without saving changes and continue on to explore the Bend tool in the next section.

Bend Tool

The Bend tool allows you to connect two planar faces by selecting a pair of parallel edges. Since Inventor allows the modeling of multiple disconnected faces, the Bend tool can add either a single bend or a double bend, depending on the number of selections you make. For design situations in which multiple disconnected faces have been produced, the Bend tool is often used to combine the faces into a single body.

There are four possible double-bend results, depending on the orientation of the edges and selected option. If the sheet-metal edges face the same direction, the tool creates either a full round bend or two bends connected with a face. If the sheet-metal edges face in opposite directions, a joggle is created with either two 45-degree bends and one edge fixed or both edges fixed and the angle calculated. In both cases, the faces will be extended or trimmed as necessary to create the bends.

Exploring Bend Options

The following example demonstrates the various ways in which double bends can be created:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_017.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Select the Bend tool from the Create panel of the Sheet Metal tab.

4.  Select an edge along each of the yellow faces for the Edges selection. Note that the Full Radius and 90 Degree Double Bend controls are enabled.

5.  Set the Double Bend option to Full Radius.

6.  Toggle the Flip Fixed Edge button and note how the preview updates. Then set it so that the upper face is the fixed edge (the preview will display partially into the lower face).

7.  Click the Apply button to create the Bend feature.

8.  Select an edge along each of the orange faces for the Edges selection.

9.  Set the Double Bend option to 90 Degree.

10.Set the Flip Fixed Edge button so that the lower face is the fixed edge and the bend previews on the outermost edge.

11.Click the OK button to create the Bend feature, and note how the lower face width is carried through to the upper face.

12.Right-click the Bend feature you just created in the browser and choose Edit Feature.

13.Click the Extend Bend Aligned To Side Faces button in the Bend Extension area and then click the OK button. Notice how the upper face width is now carried through to the bend.

14.Select the Bend tool again, choose the edge of the blue face on the small feature with two holes, and then select the edge of the blue face on the large base feature (indicated with the arrow). Keep in mind that the selection order is important for this step. When you have the correct order, the preview should show the upper feature being extended down into the lower base feature.

15.Set the bend radius to 18 mm and then click the OK button.

16.Right-click the Bend feature you just created in the browser and choose Edit Feature.

17.Change the Double Bend option to Fix Edges and then click the OK button.

Although this file showcases the available options of the Bend tool, you would not typically create faces that just float in space above or below one another. Instead, these tools are often used to create bends on faces that are modeled to fit around other existing parts, most often by projecting edges in from an assembly file. You can close this file without saving changes and take a look at the next steps to see the Bend tool used in a more realistic manner.

Using the Bend Tool to Create an Enclosure

In the following steps, you will mirror an existing side of an enclosure around the centerline of a derived frame and then use the Bend tool to join the two halves:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_018.ipt from the Chapter 6 directory of the Mastering Inventor 2015 folder.

3.  Click the Mirror button on the Pattern panel of the Sheet Metal tab.

4.  Select the features called Right_Side_Face, Front_Flange, and Back_Flange from the browser for the Features selection.

5.  Click the Mirror Plane button in the Mirror dialog box and then choose the visible YZ plane. Recall that you must select work planes by clicking their edges in the graphics area or by selecting them from the browser.

6.  Click the OK button to create the mirror feature.

7.  Select the Bend tool on the Create panel of the Sheet Metal tab.

8.  Select the top edges of the original and the mirrored faces, leave the Double Bend option set to 90 Degree, and note the preview of the bend connecting the two faces.

9.  Click the OK button to create the bend feature. Figure 6.21 shows the two sides being connected with the Bend tool.

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Figure 6.21 Creating a bend to connect the sides of an enclosure

In the previous steps, not only have you created bends, but you have essentially defined the entire top face of the enclosure with the Bend tool. Using the Bend tool to connect faces in this manner can be a quick way to use geometry projected in from an assembly or a derived work surface. You can close this file without saving changes and continue on to the next section to explore the Rip tool.

Rip Tool

The Rip tool creates a gap in a sheet-metal part. A common workflow is to create a transition with the Lofted Flange tool and then add a Rip feature so it can be flattened. The Rip tool creates a gap that is cut normal to the selected face. The Rip tool interface is optimized to create a simple gap with minimal inputs.

Inventor has three options for creating a rip, as follows:

1.  Single Point If the corner of a face is selected as the single point, the rip will follow the edge. If a sketch point located on an edge is selected, the rip will be perpendicular to the edge.

2.  Point To Point For Point To Point, a linear rip is created between the two points.

3.  Face Extents For face selection, all edges of the face are ripped.

Follow these steps to create a simple Rip feature on a square-to-round transition:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_019.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Click the Rip button in the Modify panel on the Sheet Metal tab.

4.  Set the Rip Type drop-down box to Point To Point.

5.  Select the yellow face for the Rip Face selection.

6.  Select the midpoint of the arc along the top of the yellow face and the midpoint of the arc along the bottom of the yellow face for the Start Point and End Point selections.

7.  Click the OK button to create the Rip feature. Figure 6.22 shows the Rip tool selections.

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Figure 6.22 Ripping a crease on a square-to-round transition

Creating Rip features allows you to open up a part for unfolding in a quick and easy manner. Keep in mind that you can use an extruded cut to do this as well. In most cases, though, the Rip tool will be the best tool to use. You can close this file without saving changes and continue on to the next section to explore the Unfold and Refold tools.

Unfold and Refold Tool

The Unfold and Refold tools are a powerful tool combination that allows you to unfold and then refold the model. There are several reasons to do this:

·     To add features in the unfolded state

·     To refold the model in bend order to see the manufacturing stages of the part

·     To change the orientation of the folded model in space

One of the limitations in early versions of Inventor was that you couldn't fold a deformation. Using Unfold or Refold, you can add a deformation that crosses the bend zone and then refold it. Since the deformation is simply calculated around the bend, there can be distortion issues when the deformation is large with respect to the bend radius. For best results, limit the deformation to the material thickness. For larger deformations, make sure the final results match what would be created in the shop.

Another aspect of the Unfold and Refold tools involves bend order. Many sheet-metal parts are complex, with several bend-order possibilities. Using Unfold or Refold allows you to experiment with bend order so you can determine the best way to manufacture the part.

Changing the orientation of the folded model allows for some interesting workflows. When you unfold a model, you select a face that remains stationary. When you refold the model, you also have to select the stationary face. If you select a different stationary face for the refold than you did for the unfold, the model will have a different orientation when you have finished.

Unfolded vs. Flat Pattern

The flat pattern is a separate model object that shows the completely flattened part for documentation. The flat pattern also contains manufacturing information such as bend direction. Unfold and Refold features can't be directly accessed in the drawing, so you can't have views showing different states of the same model. To show intermediate fold states in a drawing, use derived parts or an iPart to create models with refold features suppressed and then create views of those models.

Unfolding and Refolding Sheet-Metal Parts

The Unfold/Refold process is straightforward. The selections have filters for the correct geometry, so you are not required to focus on a small target. Follow these steps:

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_020.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  Click the Unfold button in the Modify panel.

4.  Select the blue face on the part for the Stationary Reference selection.

5.  Select each of the bends on the folded model. Each bend will highlight when you hover your mouse pointer over it, so you know when you have a valid selection. The unfolded preview updates as you select each bend. Alternatively, you can use the Add All Bends button.

6.  Click the Sketches button and select the visible sketch in the graphics window so that it is unfolded to match the face it resides on.

7.  Click the OK button. The model should look like Figure 6.23. Note that a copy of the sketch was placed on the unfolded model and that the original (Sketch12) is still displayed as a reference.

8.  Right-click Sketch12 in the browser and choose Visibility to toggle off its visibility so that the copied sketch can be more easily viewed.

You may have noticed that there was an option to turn off the visibility of the parent sketch in the Unfold tool as well. Most likely that is the way you would handle copied sketches, but in this case you've been instructed to do this manually to observe the way the sketches are copied. In the next steps you will create formed slots using the copied sketch.

9.  Click the Cut button in the Modify panel.

10.Select the two oblong profiles in the copied sketch and click the OK button.

11.Select the 3DModel tab and click Extrude.

12.Select the two oblong profiles in the copied sketch.

13.Click the flyout arrow in the Distance input box and choose List Parameters; then select Thickness from the list (or just type Thickness in the input box).

14.Click the Symmetric button so that the extrusion will extend equally in both directions from the sketch plane and then click the OK button.

15.Expand the Unfold1 feature in the browser, right-click Sketch12 and choose Visibility to turn off the sketch.

16.Select the Sheet Metal tab and click Refold in the Modify panel.

17.Select the yellow face on the part to use as the new stationary reference.

18.Click the Add All Bends button to automatically select all the bends. Then click the OK button.

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Figure 6.23 Unfolded model with sketch

Note that the model is in a different position than it was before the unfold action since the yellow face was kept stationary during the refold. If you drag the End-of-Folded marker above the Unfold feature, the model will be in its original position. As you can see, using the Unfold and Refold tools offers a lot of possibilities for placing features in a flattened version of the model. You can close this file without saving changes.

Unfolding and Refolding Contour Rolls Features

You can also unfold or refold a contour roll. If the tools detect that the part is a contour roll, work planes are displayed on each end face. Since a flat reference face is required, you can select one of the work planes and then unfold the contour roll, as shown in Figure 6.24.

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Figure 6.24 Unfolding a contour roll

You can open the file mi_6a_030.ipt located in the Chapter 6 directory of your Mastering Inventor 2015 folder and experiment with unfolding and refolding the part.

Project Flat Pattern Tool

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A well-hidden segment of sheet-metal-specific functionality is a special version of sketch projection called Project Flat Pattern (nested at the end of the sketch projection flyout). Project Flat Pattern is available from the folded model environment and is utilized to include the projected edges of the flattened sheet-metal component, oriented to the sketch plane that is active.

This option is powerful when combined with the Cut Across Bend option because it allows you to create parametric dimensions and constrained relationships from the perspective of the flattened sheet. When utilizing the Project Flat Pattern option, it isn't necessary to select every face; just pick the ones at the extremities (ensuring that they're on the same flattened side of the part as your sketch), and all the connecting planar faces and bends will automatically be included.

In the following steps, you'll use the Project Flat Pattern tool to place sketch entities as they would be on the flat pattern. You'll then use the Cut Across Bends option of the Cut tool to create the features in place on this rather extreme example of a bent sheet-metal part.

1.  Click the Get Started tab and choose Open.

2.  Open the file mi_6a_021.ipt from the Chapter 6 directory of the Mastering Inventor 2015 folder.

3.  Select the orange face and create a new 2D sketch on it.

4.  Click the drop-down arrow next to the Project Geometry button and select Project Flat Pattern from the drop-down menu.

5.  Select one of the yellow faces to project the chain of faces between it and the orange face into the sketch; then select the other yellow face to complete both sides.

6.  Try to select the blue faces to project into the sketch, and you'll note that nothing happens.

Nothing happens because the blue faces are actually opposite the original orange face when this part is flattened out. You could select the underside of the blue faces to include them in the sketch, but in this case you can just use the green faces.

7.  Select the green faces to project the remainder of the flat pattern into the sketch. Keep in mind that you really only need to project the faces you plan to use in the sketch, but for this example you've been instructed to select them all.

8.  Next, add three circles to the sketch. Two of the circles are to be placed at the center points of the projected yellow faces and will be 50 mm in diameter, and the third circle will be 25 mm in diameter and is to be placed in line with the center of the part and 375 mm off the tip of the orange face. Figure 6.25 shows the completed sketch.

9.  Click the Finish Sketch button when the sketch is complete and then select the Cut tool from the Modify panel.

10.Select all three of the circles for the Profile selection.

11.Select the Cut Across Bend check box and then click the OK button.

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Figure 6.25 Adding geometry to a projected flat pattern sketch

The result is that the circular cuts are placed on the folded model in accordance with their position in the flat pattern. This ability to lay out features in the flat pattern and then cut them across existing bends is a subtle but powerful tool. Keep in mind, too, that the projected flat pattern is fully associative and will update along with changes made to the features from which it was created. You can close this file without saving changes and continue on to the next section.

Using Sheet-Metal Templates and Rules

Inventor offers the ability to create sheet-metal rules that can be stored in the Inventor style library. The style library makes sheet-metal definition information more manageable, more reusable, and ultimately more powerful than simply using a template file to manage sheet-metal styles; however, using sheet-metal styles and templates to manage material and unfolding setups is supported.

What Are Sheet-Metal Rules?

Sheet-metal parts of a certain material and thickness often share bend, corner, and gap parameters. The unfold, bend, and corner settings as well as representation of punch features in the flat pattern and the bending angle or open angle option when the part is shown in the flat pattern all make up a sheet-metal rule. For instance, you might have a sheet-metal rule called 3 mm Galvanized Steel. In this rule, the material would be set to galvanized steel, the thickness to 3 mm, and the bend, corner, punch representation, and flat pattern bend angle settings would be configured to output those features consistently.

When a new part is created, you can select the predefined sheet-metal rule, and the part will follow the settings outlined within it. When a new feature such as a flange is added, the bend and corner options defined in the rule are automatically used to define it. If a setting such as a corner relief needs to deviate from the rule, it can be modified in the feature as needed. If the part is changed to use a different sheet-metal rule, the overridden settings honor the overrides, and all others update to match the rule settings.

Creating a Sheet-Metal Rule

Sheet-metal rules are created and accessed in one of two ways. You can click the Styles Editor button on the Manage tab, or you can click the Sheet Metal Defaults button found on the Sheet Metal tab. The Sheet Metal Defaults dialog, shown in Figure 6.26, allows you to specify the sheet-metal rule and whether to use the thickness, material style, and unfold rules defined in the sheet-metal rule or to override them.

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Figure 6.26 The Sheet Metal Defaults dialog box

To create or edit a sheet-metal rule, click the Edit Sheet Metal Rule button (it looks like a pencil), and the Style And Standard Editor appears. Figure 6.27 shows the sheet-metal rule options in the Style And Standard Editor.

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Figure 6.27 The Sheet Metal Rule page in the Style And Standard Editor dialog box displaying an active rule

Follow these general steps to create a new rule:

1.  Select an existing rule and click the New button at the top of the screen.

2.  Enter a name for the new rule.

3.  Set the sheet material and thickness.

4.  Set an unfold rule to use.

5.  Set the gap thickness to use. You can set this to Thickness so that it will update to match the sheet thickness, or you can set it to a fixed value.

6.  Set the bend angle to either Bending Angle or Opening Angle.

7.  Set the Flat Pattern Punch Representation style.

8.  Click the Bend tab and set the bend options.

9.  Click the Corner tab and set the corner options.

10.Click the Save button along the top of the Style And Standard Editor dialog box. The rule is now saved in the current part file.

11.Optionally, right-click the new unfold rule name in the left list and choose Save To Style Library to write the new unfold rule to the external style library XML file.

12.Click Done to exit the Style And Standard Editor dialog box.

Bend and Corner Quick References in the Help Files

Autodesk has done a good job of hiding the help references for many of the sheet-metal features. However, once you find them, they are helpful in determining what these options adjust. When you find them, you can create a Favorites link so they are more accessible. Here are a couple you might want to add to your favorites:

1.  Sheet Metal Bend Options Press F1 to bring up the help pages. On the Contents tab, expand the tree to find Autodesk Inventor Parts Sheet Metal Parts Sheet Metal Features Faces and then click the Quick Reference tab in the right pane. Select Sheet Metal Bend Options.

2.  Sheet Metal Corner Options Press F1 to bring up the help pages. On the Contents tab, expand the tree to find Autodesk Inventor Parts Sheet Metal Parts Sheet Metal Features Corner Seams and then click the Quick Reference tab in the right pane. Select Sheet Metal Corner Options.

To add them to your favorites, click the Favorites tab and click Add in the left pane while viewing the page. Once they are added, you can rename them via the context menu.

Sheet-Metal Rules vs. Sheet-Metal Styles

Sheet-metal rules are set up using the Style And Standard Editor. Initially, the rules are created in a part file as a local style, meaning they exist in that part file only. If you save the part file as a template file, all of your new parts will contain the sheet-metal rule. In addition to using templates to manage sheet-metal rules, you can add the rules to the style library. Style libraries are XML files that are stored externally to the part files and therefore can be used by newly created parts or existing parts. You save a rule to a library by right-clicking the rule in the Style And Standard Editor and selecting Save To Style Library, assuming your project (.ipj) file is set up to use a style library.

Unfold Rules

Whenever you fold a sheet-metal part on the shop floor, some material deformation occurs at the bend location. To the outside of the bend the material stretches, and to the inside of the bend the material is compressed. To calculate this deformation for each bend, Inventor uses sheet-metal unfold rules. Sheet-metal unfold rules control the method of unfolding used to calculate the flat pattern for a folded sheet-metal part. You can create unfold rules using a K-factor or a bend table.

K-Factors

K-factors define the theoretical percentage of the material thickness where a folded part is neutral and neither expands nor contracts. The reason this surface is referred to as the neutral surface is that it defines a measurable position within the bend that has the same value in the folded and unfolded states. For instance, if your material is 10 mm thick and you use a K-factor of 0.44, bends and folds are calculated so that deformation of the bend takes place at 4.4 mm (or 44 percent of the material thickness). Unfolding with a K-factor is accomplished by determining the bend allowance (the amount of material required to produce a bend) for a given bend using the sheet thickness, the bend angle, the inner bend radius, and a K-factor value. The K-factor you use will depend on numerous factors, including material, thickness, and tooling. Most likely, you will need to perform a number of test bends on a specific press brake to determine the ideal K-factor for you.

The following equation is used to determine the developed flat pattern length using a K-factor:

equation

The bend allowance is calculated using this equation:

equation

In this equation, the abbreviations have the following meanings:

·     BA = bend allowance

·     A = bend angle in degrees

·     R = inside bend radius

·     K = K-factor

·     T = material thickness

Figure 6.28 shows a basic bend.

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Figure 6.28 Basic bend references

To create an unfold rule to use a K-factor, follow these general steps:

Custom Unfold Equations

In addition to K-factors and bend tables, you can create custom unfold equations to use as an unfold method. You can find more information concerning custom unfold equations by selecting the Index tab of the help file and searching the keywordUnfolding and then selecting Sheet Metal Equations from the list.

1.  Select the Manage tab and click the Styles Editor button to open the Style And Standard Editor dialog box.

2.  Click the plus sign to the left of the Sheet Metal Unfold Rule node in the left pane of the Style And Standard Editor dialog box to display the existing unfold rules.

3.  Click an existing default rule to serve as the template for the new rule.

4.  Click the New button along the top of the Style And Standard Editor dialog box.

5.  Enter the name of the new sheet-metal unfold rule and click the OK button.

6.  Ensure that the unfold method is set to Linear.

7.  Enter a new K-factor value.

8.  Click the Save button at the top of the Style And Standard Editor dialog box. The rule is now saved in the current part file.

9.  Optionally, right-click the new unfold rule name in the left list and choose Save To Style Library to write the new unfold rule to the external style library XML file.

10.Click Done to exit the Style And Standard Editor dialog box.

Bend Tables

An alternative to using K-factors is to create a bend table. Using bend tables is the most accurate method of unfolding because bend tables are created by taking measurements of actual bent test parts of the exact material and thickness made on the shop floor. To create a bend table in Inventor, you must first gather accurate bend information by creating bend tests. The granularity of the experimental values is up to you. It could be based on 15-degree increments or perhaps 0.5-degree increments; it depends on how much experimental data you have.

Typically, a number of test blanks are cut from a given material and thickness and then bent to the most common angles and radii used. If you measure the folded sample using virtual sharp locations, the values obtained will inherently be too large. The overmeasurement of the test fold sample needs to be compensated for by deducting an amount of length. By subtracting your combined measurements from the initial measurement of the sample taken prior to folding, you will be able to determine the value of excessive length (overmeasurement); this is what gets entered into the bend table and is where the method name bend deduction comes from. Bends are then calculated as follows:

equation

You can set up a test bend table as described in the following steps:

1.  Click the Get Started tab, and choose Open.

2.  Open the file mi_6a_022.ipt from the Chapter 6 directory of your Mastering Inventor 2015 folder.

3.  On the Sheet Metal tab, select Sheet Metal Defaults.

4.  Click the Edit button for Unfold Rule (it looks like a pencil).

5.  In the Style And Standard Editor, expand the Sheet Metal Unfold node from the list on the left (if it's not already expanded), select Default_KFactor, and then click the New button at the top. This creates a new unfold rule based on the existing one.

6.  Enter Mastering Bend Table for the name and click the OK button.

7.  Change the Unfold Method drop-down box to Bend Table.

8.  Set Linear Unit to millimeter (mm) to match the units of this part file.

9.  Click the Click Here To Add row in the Thickness box, and enter 2.00 for 2 millimeters.

10.Enter 30 into the leftmost cell of the table to define the angle at 30 degrees.

11.Enter 1.0 in the topmost cell to define the bend radius at 1 mm.

12.Enter 0.5 in the cell to the right of the angle cell and just under the bend radius cell. This is the bend deduction (in this case, 0.5 is a hypothetical value).

13.Add another bend angle row by right-clicking the cell containing 30 and choosing Insert Row.

14.Enter 45 for the angle and 0.6 for the bend deduction.

15.Add another bend radius column by right-clicking the cell containing 1.000000 and choosing Insert Column.

16.Enter 2.0 in the column header for the bend radius and then enter 0.55 for the 30-degree row and 0.65 for the 45-degree row.

17.Add a third row of 60 degrees with 0.70 and 0.75 bend deductions in the 1.000000-degree and 2.000000-degree columns, respectively.

18.Add a third column of 3.0 mm with 0.600.70, and 0.80 for the 30-, 45-, and 60-degree rows, respectively.

19.Bends greater than 90 degrees and bends less than 90 degrees are handled differently, so in this case you want to set the Angle Reference radio button to use the Bending Angle Reference (A) option. This allows the table to match the existing part. If you wanted to use the Open Angle Reference (B) option, your table angles would need to be 150, 135, and 120. You can check your table against the one in Figure 6.29.

20.Click Save and then Done to finish the bend table.

21.In the Sheet Metal Defaults dialog box, choose Mastering Bend Table from the Unfold Rule drop-down box to make it the active unfold rule for this part and then click the OK button.

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Figure 6.29 The sample bend table

Bending Angle and Open Angle References

Originally, the Inventor Bend Table was designed to reference an open angle datum structure (which is still the default) for measuring bends. However, the sheet-metal features all use a bending angle datum structure to create bent features. As a means to bridge this disparity in measurement convention, the Bend Angle option at the top of the bend table interface allows you to declare the structure in which your values were measured; Inventor will use this option to convert the values internally if necessary. Keep in mind that the angular values are not altered within the table when this option is changed.

As you can see, the process of creating a bend table in Inventor is a straightforward endeavor. Typically, the real work is in creating the test blanks and bends to gather the information to put into the table.

Here are a few more things to know about creating bend tables:

·     Note that you can reorder rows and columns by clicking the header cell and dragging them into place.

·     You can also right-click the top, leftmost cell and choose Paste Table to paste in a table copied from an Excel spreadsheet. Likewise, you can choose Copy Table to copy the table into Excel.

·     You can add a bend table for each thickness required by clicking the Click To Add row in the Thickness box.

·     If the bend deduction is outside of the values defined in the table, Inventor uses the Backup K-factor. You can think of this as an insurance plan that allows you to obtain a flat pattern even if your bend table doesn't define what deduction to use for smaller or larger combinations of bend angle and radius.

·     For combinations that fall within the table boundaries but not exactly at angle/radius coordinate values, Inventor uses linear approximation to derive a value; depending on the change in bend compensation between steps in the table, you can achieve better results with smaller angle increments.

·     You can specify a table tolerance to allow Inventor to include thicknesses, radii, and angles that are within the specified tolerance. For example, if the angle tolerance is 0.004 and a bend angle measures 30.002, Inventor would use the 45-degree row in your table to calculate the deduction.

To test the bend table, you can examine the flat pattern in mi_6a_022.ipt, where a sketch has already been placed to display the flat pattern length. Because the part file has a current thickness of 2 mm, a bend angle of 60 degrees, and a bend radius of 2 mm, the bend deduction indexed from the bend table will be 0.75 mm, as shown in Figure 6.29.

In this case, then, the bend deduction is calculated as follows:

equation

If you were to change the angle to 45 degrees (and click the Update button) and check the flat pattern again, you would expect to see this:

equation

What would happen if you were to set the angle to 37.5 degrees, which is halfway between 30 and 45 degrees? Because the bend table has no entry for 37.5 degrees, Inventor uses a linear extrapolation of the bend deductions of 0.55 mm for 30 degrees and 0.65 mm for 45 degrees and arrives at the halfway point of 0.60 mm for 37.5 degrees. If you check the flat pattern, you will expect to see this:

equation

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K-Factors and Bend Tables: Which Should I Use?

The most common question asked about flat patterns concerns the use of K-factors and bend tables. Which to use depends on your manufacturing processes and the capabilities of your machines. These are the main questions to ask when determining which is right for you:

·     Do you outsource your sheet-metal manufacturing?

·     How accurate do your parts need to be?

Whether you build the parts in-house or you outsource them, you should be able to get the data from the shop. If your sheet-metal shop is unsophisticated, they may use rules of thumb to determine the bend allowance. In that case, you need to work with them to determine whether a K-factor or a bend table is the best solution. One of the advantages of using sheet-metal rules is that you can create rules for each shop. For example, if you generally use your shop but you outsource when you are busy, you can select the rule for the other shop, and the flat pattern will automatically update.

In general, K-factors are used for parts with large tolerances. Since the K-factor is an approximation, the actual value will vary depending on the machine. For parts with very tight tolerances, you need to know specific compensation values for the bend radius and angle for the machine, material type, and thickness. Depending on the material, you might need different values based on the grain direction. For extremely tight tolerances with certain material types, you might even need different values for each shipment of material.

Bend Compensation

In addition to using K-factors and bend tables, you have the ability to enter an expression for a bend compensation. Instead of entering values for specific bend angles and using linear interpolation between the values, you can enter ranges of bend angles that use an expression to determine the proper compensation within that range. To access the Bend Compensation settings, click the Style Editor button on the Manage tab and then expand the Sheet Metal Unfold node in the left pane. Finally, select BendCompensation. Figure 6.30 shows the BendCompensation settings.

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Figure 6.30 BendCompensation settings

Working with Styles and Templates

If your project location is set to use the style library, it is important to understand what has been defined within your template and what has been stored within the style library. For example, suppose you have a sheet-metal rule named MyRule1 with the Thickness value equal to 2 mm stored only locally in your template file, and another sheet-metal rule also named MyRule1 but with the Thickness value equal to 5 mm, also stored in your style library. Each time you start a new design from the template referencing MyRule1, you will see a Thickness value of 5 mm being applied. The reason for this is that the style library is the “published” source of your standards; its definition will always win. After saving your design, if you want to make changes to the Thickness value of MyRule1, you can apply the changes without fear that they might be automatically overwritten because this occurs only when creating a new document using the template. (As a side note, if you did want to overwrite the local/document definition with the style library's definition, right-clicking an existing rule will present a context menu from which you can select Update Style, which will manually refresh the rule's definition in the document.)

It is a good practice when using the style library to have only a single generic sheet-metal rule embedded in your template file (at least one is required). Once you know what sheet-metal rule you want to apply to your model, selecting it either in the Style And Standard Editor dialog box or in the Sheet Metal Defaults dialog box will automatically draw the information into the active document. This process keeps extraneous information out of your document, providing a smaller footprint, and helps reduce the chance of style information mismatch. If you have a template file that has numerous sheet-metal rules stored within it, after publishing them to the style library, you can use the purge functionality with the Style Management Wizard to remove them.

Working with the Flat Pattern

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The flat pattern derived from the folded model ties the design to the manufacturing environment. Within Inventor, the flat pattern model is an actual flattened version of the folded model vs. a sheet that has been pieced together and thickened. Numerous tools, utilities, and data sources have been provided to enable the flat pattern to suit your individual manufacturing and documentation needs.

The flat pattern contains a wealth of manufacturing information that is stored progressively during the design process. Punch and bend information is stored within the flat pattern model specifically so that customers working with drawings, customers working with the application programming interface (API), or those who want to translate the flat pattern to a different file version can control all their options in a common location; the flat pattern is commonly referred to as the jumping-off point for all downstream consumers.

The following sections detail these capabilities and tools.

Exploring the Flat Pattern Edit Features

The flat pattern environment has its own panel bar containing a customized set of modeling tools drawn from the Part Features panel bar and the Sheet Metal Features panel bar. The flat pattern tools are referred to as flat pattern edit features because they are intended to apply small alterations to the flat pattern model instead of doing large-scale modeling. Flat pattern edit features are applied only to the flat pattern, whereas folded model features are first applied to the folded model and then carried over to the flat pattern. The flat pattern can be imagined as a derivative of the folded model, establishing a parent–child relationship (flat pattern edit features are not reflected in the folded model). There are many situations in which the generated flat pattern is not exactly what you need for manufacturing; flat pattern edit features are ideal for making small associative tweaks that previously required exporting the flat pattern to an external (disassociated) file.

Adding Manufacturing Information to the Flat Pattern

There are two features specifically designed to allow you to add manufacturing information to the flat pattern. The Bend Order Annotation tool enables you to specify the order in which bends are created. The Cosmetic Centerlines tool marks bend locations, such as cross brakes, where there is mild deformation.

1.  Bend Order Annotation

When you click the Bend Order Annotation icon in the Manage panel, the bends are automatically numbered. You can renumber individual bends by double-clicking the number glyph or right-clicking and choosing one of two options for overriding the numbering: Directed Reorder and Sequential Reorder. Figure 6.31 shows the bend order being edited.

1.  Directed Reorder With this option you are prompted for the selection of a start glyph and an end glyph. An algorithm is used to renumber bend centerlines that lie between the selected start and end glyphs.

2.  Sequential Reorder With this option you select each bend centerline glyph in the reorder sequence.

You can follow these general steps to adjust bend order:

1.  Click the Go To Flat Pattern button on the Sheet Metal tab.

2.  Click the Bend Order Annotation button on the Sheet Metal tab.

3.  You can select a specific bend centerline glyph (or glyphs) and enter the new order number or right-click and choose one of the reorder methods.

4.  Right-click and choose Finish Bend Order.

Cross Breaks, Creases, and Cosmetic Centerlines When working with large parts made with thin sheet materials (such as in HVAC designs), you may have a need to show cross-break information. Adding these features in the folded model is a challenge and is generally not required. Instead, you can add cross-break information to the flat pattern in the form of cosmetic centerlines. Cosmetic centerlines capture bend information in the flat pattern without changing the model. Figure 6.32 shows the Cosmetic Centerlines tool in use.

To create cross-break lines, follow these general steps:

1.  Click the Create Flat Pattern button (or the Go To Flat Pattern button if it's already created) on the Sheet Metal tab.

2.  Create a new 2D sketch on the appropriate face of the flat pattern (click the OK button if warned about the sketches on the flat pattern not carrying over to the folded model).

3.  Use the Line tool to create the cross-break lines as needed.

4.  Click the Finish Sketch button on the Sketch tab.

5.  Click the Cosmetic Centerline button (on the Create panel in the Flat Pattern tab) and select any previously sketched lines.

6.  Adjust the manufacturing information using the controls in the Cosmetic Centerline dialog box and then click the OK button.

A Cosmetic Centerline feature will be created in the browser, and it will consume the sketch you created. You can edit it as you would any other feature if needed.

image

Figure 6.31 Editing the bend order annotation

image

Figure 6.32 Creating cross breaks with the Cosmetic Centerlines tool

Using the Flat Pattern Definition Dialog Box

You can manipulate the flat pattern model by using a tool called Edit Flat Pattern Definition, which is available by right-clicking anywhere in the graphics area and selecting Edit Flat Pattern Definition. The Flat Pattern Definition dialog box allows you to control a number of aspects pertaining to the flat pattern's orientation and the information stored within it, as shown in Figure 6.33.

image

Figure 6.33 Assigning flat pattern orientation to run on different machinery

The first tab of the Flat Pattern Definition dialog box relates to the flat pattern orientation. The selection control allows you to select either an edge or two points to define the horizontal or vertical orientation. The orientation of the flat pattern is important because the implied x-axis is used to calculate the rotational angle of Punch tools that have been applied to the model. When you orient the flat pattern to your specific punch equipment, the required tool rotation angle should be directly available from your flat pattern.

Since the flat pattern base face is going to be either the face already selected or the backside, the control of the base face has been simplified to a “flip” option. Base face definition is critical because it establishes a directional reference for bends and punch tooling as well as an association with the front navigation tool view and the default Drawing Manager view.

The second tab is the Punch Representation tab, which allows you to override the representation setting in the sheet-metal document without having to edit the active sheet-metal rule.

The third tab is the Bend Angle tab, which allows you to declare how bend angles should be reported to the API and Drawing Manager. For example, this means that by changing the Bend Angle option to an open angle, Drawing Manager annotations of your flattened bends will recover the complementary angle of the bending angle.

Controlling the Finished Face of the Flat Pattern

If you work with prefinished surface materials, having the finish side up when laser cutting, punching, or breaking is often an important consideration. To control the upward-facing surface, or base face, when creating the flat pattern, you can select any face of the folded part on the finished side and then click the Create Flat Pattern button. Inventor will hold the selected face as the base face.

If you need to change the base face, you can use the Flip button found in the Pattern Definition dialog box. Do this by clicking the Go To Flat Pattern button, right-clicking the Flat Pattern node in the browser, and selecting Edit Flat Pattern Definition.

Manufacturing Your Flat Pattern

There is a close association between sheet-metal design and manufacturing, and the flat pattern solution within Inventor embraces this relationship. Inventor generically supports the ability to translate models to a variety of file formats, but Inventor sheet metal actually has its own utility to support the translation to SAT (.sat), DWG (.dwg), and DXF (.dxf) formats.

Saving Flat Patterns

After selecting the Flat Pattern browser node, you can right-click and select Save Copy As; this launches the Flat Pattern Translation dialog box. For SAT files, a simple option defining the file version will be presented. For DWG and DXF file formats, an extensive list of options and file-processing capabilities is made available to you.

Within the Flat Pattern Translation dialog box, you will find standard options for file type, but there is also a Layer tab that supports layer naming and visibility control. The last tab is the Geometry tab, which allows you to decide whether you want to apply a variety of manufacturing-specific options to the translation. The first of these options is for spline simplification because many Computer Numerical Control (CNC)–profile manufacturing centers cannot leverage splines and are restricted to arcs and lines.

Translating Splines

The translation utility allows you to apply faceting rules to break the outer contour of flat patterns into linear segments. The second options group relates to the post-processing of the translated file, allowing you to force the 2D result into positive coordinate space and to merge interior and exterior contours into polylines, which may be critical for a path-based tool. Figure 6.34 shows these settings.

image

Figure 6.34 Geometry translation when saving a DXF file

Sketching on Flat Patterns

Sometimes you'll need additional tool path manufacturing information such as etch lines in your DXF/DWG output. For this, the flat pattern has the ability to export unconsumed sketches created on the flat pattern. With these you can create a sketch containing the lines you need on the flat pattern. Once you save the DXF or DWG file, any visible sketches located on the flat pattern are exported, and a layer called IV_UNCONSUMED_SKETCHES is added to contain these sketches. Note that sketch text will not export using this method. If you need to add single-line text paths to your flat pattern for laser engraving, the best method is to do so in the DWG or DXF after it has been exported from Inventor.

Using Sheet-Metal iPart Factories

iParts are part configurations or part families that allow you to create a base part and then add a table to it. Once the table is added, the part features can be suppressed or configured to create a family of parts based on the original. The configured part is referred to as an iPart factory, and the individual configurations are called members. Sheet-metal iParts have a number of uses, from creating variations of basic parts to creating progressive die parts.

More iPart Information

You can find more information, including step-by-step instructions for creating iParts and sheet-metal iParts, in Chapter 7.

iParts for Configurations

Using iParts for sheet-metal configurations is common for parts that are basically the same but vary in the size, material, or inclusion of certain features. For example, a bracket could be designed and configured in basic mild steel, or optionally in an upgraded stainless steel version. Or you could create an iPart to handle variable hole locations on a standard-shaped bracket. Another common use would be a series of brackets that are identical in material and fold information but vary in length. Sheet-metal configurations via iParts could be beneficial and profitable to a company that deals in varieties of components that need to fit into the same space but utilize different materials or manufacturing processes or contain different features. Once different members of the iPart factory are configured, you can use the Generate Files option shown in Figure 6.35.

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Figure 6.35 Sheet-metal iPart factory example, displaying Generate Files for selected member files

This tool is intended to support the batch creation of member files on disk; it can also be used to force updates, such as the flat pattern, out to the member files already in existence. In addition, you can use a pull method vs. a push method. If you open the iPart factory, execute the Rebuild All operation, and then save the rebuilt and migrated data, the member files when individually opened will “see” that they are out-of-date with the factory. Selecting the now-enabled Update button within the individual member file will then draw in the flat pattern information automatically.

iParts for Fold Progression

If you have the need to show the order in which a part is created, such as detailing progressive dies, you might want to explore the use of iParts and the Unfold tool. Once a folded part is complete, you can convert it to an iPart and use the Unfold tool to detail each step of the progression. In the iPart, the unfold features can then be suppressed to show the part folding back up. Because each iPart member (in this case representing the same part in different stages) can be detailed on a drawing, you can quickly illustrate the progression of the blank, flat piece to the finished part.

Modeling with Non-Sheet-Metal Features

Although the sheet-metal feature set is extensive, sometimes using non-sheet-metal features can be helpful or possibly even required to accomplish your design. The challenge when using non-sheet-metal features is to honor the guiding principles of sheet-metal design so that the resulting component can be unfolded; in addition, you want to incorporate sheet-metal conditions so that the features are manufacturable and therefore cost-effective.

Selecting Problematic Features

Although it's possible to design sheet-metal components using lofts, solid sweeps, and shells, these features can produce unpredictable and hard-to-control results. The Loft tool, unless highly restricted, produces doubly curved surfaces that cannot be unfolded properly. It's possible to utilize rails to control loft curvature, but it's time-consuming and invariably frustrating. Solid sweeps are a measure better than lofts, but these too can create unintended doubly curved surfaces. The Shell tool can be used nine times out of ten to successfully create a legitimate sheet-metal feature, but the tenth time, if it doesn't work and it's not clear why, will be confounding. If you use the parameter Thickness to shell your component, you'll probably be in fairly good shape, but there are certain situations in which the Shell tool cannot assure uniform thickness after the shell. These situations are not always simple to predict.

Using Surface-Based Workflows

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In addition to the sheet-metal-specific tools, you might sometimes need to use standard non-sheet-metal tools to create complex parts or features. The most successful non-sheet-metal feature workflows typically use a surface that is later thickened. The reason these workflows are so successful is that it's often easier to ensure that the resulting model embodies sheet-metal conditions (the side faces are perpendicular to the top and bottom faces and the part maintains a constant thickness) since the part can be thickened normal to the surface using the Thicken/Offset tool. When you're constructing surfaces that will be thickened, the Extrude and Revolve tools are excellent choices because they have restricted directions in which features are created, which can help ensure that only cones, cylinders, and planes are created (these can be unfolded).

The Sweep tool is possibly another good choice, but care needs to be taken to ensure that the profile and the sweep path do not contain any splines or ellipses that might prevent unfolding. For thickened, extruded, revolved, or swept features, the sketch profile geometry should ideally be limited to arcs and lines to help ensure the creation of unfoldable geometry. When you're using the Sweep tool, the Guide Surface option (see Chapter 5, “Advanced Modeling Techniques”) is ideal because the swept profile is rotated along the path to ensure that it remains normal to the guide surface. Sometimes a thickened sheet-metal component needs to be trimmed with a complicated profile. For these situations, a swept surface combined with the sculpt feature can result in a model that still has sheet-metal conditions.

Another common surface-generating workflow is to use a derived component, where you select the Body As Work Surface option when placing the derived component into the sheet-metal file. This workflow can be combined well with either a thicken feature or a sheet-metal face feature after creating projected sketches for each planar surface. This was the method used earlier in this chapter when you used the Bend tool to create an enclosure from the derived frame.

One of the biggest benefits of working with surfaces is that you can apply complicated alterations to the surface prior to thickening. Some of the most common features utilized to create cutting surfaces are Extrude, Revolve, and Sweep. Additionally, the Split tool (and perhaps Delete Face) can be utilized to remove faces from the thickened surface selection.

Working with Imported Parts

The Inventor sheet-metal environment has been designed to work with imported geometry because its solid unfold engine is concerned with topology, not with features. This means that files imported directly from other 3D modelers such as SolidWorks, CATIA, and Pro/ENGINEER, as well as neutral file types such as STEP, SAT, and IGES files (.step, .sat, and .iges) can be brought into Inventor. Once imported, they can be modified with additional features and unfolded, provided they maintain a constant thickness that matches the thickness set in the part.

More on Importing Part Files

You can find more information about importing part files and exchanging data with other CAD systems in Chapter 14, “Exchanging Data with Other Systems.”

Setting Yourself Up for Success

There are two main methods for importing parts into Inventor: the Open dialog box and the Import tool that's on the Insert panel of the Manage tab. If you are able to use Open (which is preferred), a standard part template is going to be utilized by default to embed initial styles and document options, so the first step will be to use the Convert To Sheet Metal tool to draw the sheet-metal subtype options and rules into the document. If you use the Import tool from within an empty sheet-metal document, the imported geometry will be in the form of a surface. To work with this geometry, you will need to thicken each surface, which can be a time-consuming process. I recommend, when possible, that you “open” imported parts so that a solid body can be recovered.

The next step you need to accomplish is the measurement of the sheet thickness of your imported model; once you have this value, you can match it with an appropriate sheet-metal rule (or create a new one). Matching the thickness can be as simple as taking a measurement from the sheet and overriding the Thickness value within the Sheet Metal Defaults dialog box with a simple copy and paste. Since the solid unfolder works with evaluated topology to facilitate the unfolding, the thickness of the actual part must match the thickness of the active sheet-metal rule exactly.

If the imported part contains portions that are not of uniform thickness, proper unfolding may not be possible; spend some time evaluating your imported model to ensure that it conforms to sheet-metal conditions. If your imported model contains faces defined by splines or ellipses, you are not going to be able to unfold your part. In these cases, removing these faces and replacing them with faces defined by tangent arcs may be an acceptable modification.

Converting Components

On the Environments tab is the Convert To Sheet Metal tool. The purpose of this tool is to take a component that has been designed with a regular part template and convert that document to a sheet-metal subtyped document. This means all the sheet-metal reference parameters and the default sheet-metal rule and unfold rule are automatically added to the document.

You can also convert a sheet-metal part back to a part document. Basically, this deletes the flat pattern and disables the sheet-metal functionality, but the sheet-metal parameters are not deleted.

Be Careful When Converting Back to a Standard Part

You should convert a sheet-metal part back to a standard part file only if the manufacturing process for a part has changed. Some people have gotten into the habit of using the convert tools to access the part-modeling tools. Using the convert tools to navigate back and forth can have undesirable effects. Most notably, it can delete your flat pattern and break associations with downstream documentation; therefore, use the convert tools sparingly.

Annotating Your Sheet-Metal Design

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The Drawing Manager environment contains several tools and functions specifically focused on helping you document your sheet-metal design. A quick overview of sheet-metal annotation tools might help you understand them a bit better.

Creating a View of Your Sheet-Metal Design

The first step in creating your documentation will be to choose which model file to reference, but with sheet metal comes the added requirement of deciding between a folded model and a flat pattern view, as shown in Figure 6.36. Once a sheet-metal model file is selected on the Component tab, a Sheet Metal View options group will appear immediately below the file's path information. The displayed options allow you to choose between creating a folded or flat pattern view and, in the case of a flat pattern, choose whether you want center marks to be recovered for any embedded Punch tools. The default view options will change based on your selection, because the flat pattern has a clear distinction between its top (default) face and its bottom (backside) face. The actual orientation of the 3D flat pattern defines what is a top face and what is a bottom face. This also impacts bend orientation with respect to what is reported as up and what is reported as down. All punch angular information is based on the virtual x-axis previewed during flat pattern orientation.

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Figure 6.36 The Drawing Manager: the Drawing View dialog box's Component tab with options displayed for sheet-metal view creation

The Model State tab may also be of interest because sheet-metal iPart members can be individually selected when a factory file is referenced, as shown in Figure 6.37. Choosing between a folded model and a flat pattern is also necessary when creating a drawing view of the sheet-metal iPart member. If the member has not already been placed, selecting the member from the Drawing View dialog box will automatically create the file.

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Figure 6.37 The Drawing Manager: the Drawing View dialog box's Model State tab with options displayed for sheet-metal iPart member view creation

The last tab is the Display Options tab, which is important because it controls whether sheet-metal bend extents should be drawn in the view, and it controls other annotations such as work features and tangent edges, as shown in Figure 6.38.

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Figure 6.38 The Drawing Manager: the Drawing View dialog box's Display Options tab with options displayed for sheet-metal bend extents

Adding Bend, Punch, and Flat Pattern Annotations

Once you've created the view of your sheet-metal component, you can switch to the Drawing Annotate tab to complete the documentation of your design. The sheet-metal annotation tools within the Drawing Manager are specific to flat pattern views. You can add bend notes and punch notes, as shown in Figure 6.39.

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Figure 6.39 The Drawing Annotate tab with Punch and Bend tools displayed

Bend Annotation Tables

Bend notes allow you to recover bend angle, bend direction, bend radius, and K-factor (which is not on by default) for any bend centerline. You can utilize the General Table tool to create a Drawing Manager bend table (not to be confused with bend tables utilized for unfolding) that documents all the bends in a selected view. To create a Drawing Manager bend table, follow these steps:

1.  Select General from the Table panel of the Drawing Annotation tab.

2.  Select an existing flat pattern view.

3.  Decide whether the chosen columns are acceptable (bend direction, angle, and so on); if not, alter the selected columns.

4.  Choose the Bend ID format and enter a prefix if desired.

5.  Click the OK button to create the bend table.

Punch Annotation Tables

The punch note allows you to select a formed punch, center mark, or 2D alternate punch representation in order to recover the punch angle, punch direction, punch ID, and punch depth (punch ID and depth need to be added to the Punch tool description when the punch feature is authored). When editing the punch note, you will also see a Quantity option that allows you to recover the number of instances of the same Punch tool in the view.

Punch table creation is a little different from bend table creation because it has been incorporated within the preexisting hole table annotation tools. The reason punch support was combined with hole tables is that you most likely used the Hole tool out of convenience, not necessarily to convey a manufacturing process. To make sure all of this tool-based information is consolidated, an enhancement to hole tables was made. After invoking the Hole Table – View tool and selecting a flat pattern view, you will see that the standards in the toolbar have changed to reflect predefined hole table standards. Within this list (as shown in Figure 6.40) is an example standard for punch tables, which prevents you from having to first create a standard hole table and then edit it to add all the punch information columns.

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Figure 6.40 Drawing Manager active style toolbar showing punch table style preset

From within the Text tool, you can reference the sheet-metal flat pattern extent values by selecting a new Sheet Metal Properties option from the Type list, as shown in Figure 6.41. Once you've selected the Sheet Metal Properties type, the Property list will provide options for entering the flat pattern extents area, length, or width in the text box.

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Figure 6.41 The Drawing Manager: the Format Text dialog box displaying the Sheet Metal Properties option for flat pattern extents

Use Sheet-Metal Manufacturing Annotation Effectively

You may have noticed that different toolmakers and machinists like to see different annotations. Although there are some definite right and wrong ways to annotate a part, a lot of gray area exists concerning this as well, because there is no specific way to annotate the part “correctly.” It is in these areas where you must talk to your fabricators and outside vendors to determine what information they'd like to see on the prints and to explain what type of annotation you plan to provide. Don't be afraid to ask the fabricators what information would make their job easier. As long as it does not impact your workflow dramatically, it might just save you some time and money on your parts.

The last annotation tool that can interact with sheet-metal properties is the Parts List tool. To recover flat pattern length and width extents within the parts list, follow these steps:

1.  From within your sheet-metal model, right-click the filename node in the Model browser and choose iProperties.

2.  Select the Custom tab and create a new custom iProperty named Length.

3.  Ensure that the type is set to Text.

4.  Enter a value of = <FLAT PATTERN LENGTH> cm.

5.  Repeat steps 2 through 4 for a custom iProperty named Width, entering a value of = <FLAT PATTERN WIDTH> cm.

6.  Save the sheet-metal model file.

7.  From within the Drawing Manager, launch the Parts List tool.

8.  Using the Select View tool, select a flat pattern view of the sheet-metal model containing the custom iProperties, click the OK button, and place the parts list on your drawing.

9.  Right-click your parts list, and select the Edit Parts List tool.

10.Right-click the table, and select Column Chooser.

11.Select the New Property tool and enter Length.

12.Repeat step 11, creating an additional property named Width.

13.Click the OK button.

14.Select the new column named Length, right-click, and select the Format Column tool.

15.Change the formatting and precision of the length to match your needs.

16.Repeat step 15 for the Width column, clicking the OK button when complete.

Saving Time with Custom iProperties

If custom property information is something you might routinely want to access, create the custom iProperty values in your sheet-metal template file so that they are always available.

The Bottom Line

1.  Take advantage of the specific sheet-metal features available in Inventor. Knowing what features are available to help realize your design can make more efficient and productive use of your time.

1.  Master It Of the sheet-metal features discussed, how many require a sketch to produce their result?

2.  Understand sheet-metal templates and rules. Templates can help get your design started on the right path, and sheet-metal rules and associated styles allow you to drive powerful and intelligent manufacturing variations into your design; combining the two can be productive as long as you understand some basic principles.

1.  Master It Name two methods that can be used to publish a sheet-metal rule from a sheet-metal part file to the style library.

3.  Author and insert punch tooling. Creating and managing Punch tools can streamline your design process and standardize tooling in your manufacturing environment.

1.  Master It Name two methods that can be utilized to produce irregular (nonsymmetric) patterns of punch features.

4.  Utilize the flat pattern information and options. The sheet-metal folded model captures your manufacturing intent during the design process; understanding how to leverage this information and customize it for your needs can make you extremely productive.

1.  Master It How can you change the reported angle of all your Punch features by 90 degrees?

5.  Understand the nuances of sheet-metal iPart factories. Sheet-metal iPart factories enable you to create true manufacturing configurations with the inclusion of folded and flat pattern models in each member file.

1.  Master It If you created sheet-metal iPart factories prior to Inventor 2009, any instantiated files contain only a folded model. Name two methods that you could use to drive the flat pattern model into the instantiated file.

6.  Model sheet-metal components with non-sheet-metal features. Inventor doesn't always allow you to restrict yourself to sheet metal–specific design tools; understanding how to utilize non-sheet-metal features will ensure that your creativity is limitless.

1.  Master It Name two non-sheet-metal features that can lead to unfolding problems if used to create your design.

7.  Work with imported sheet-metal parts. Understanding the way in which Inventor accomplishes unfolding as well as how to associate an appropriate sheet-metal rule are keys to successfully working with imported parts.

1.  Master It Name the one measured value that is critical if you want to unfold an imported part.

8.  Understand the tools available to annotate your sheet-metal design. Designing your component is essential, but it's equally important to understand the tools that are available to efficiently document your design and extract your embedded manufacturing intent.

1.  Master It What process is required to recover flat pattern width and height extents within your Drawing Manager parts list?