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

Chapter 7. Reusing Parts and Features

The ability to reuse parts and features in other designs is an important step in increasing productivity. Autodesk® Inventor® software provides this ability through different workflows. This chapter introduces you to several methods that will assist you in achieving your goal.

Developing the proper workflow for your company will depend on several criteria. Depending on your involvement with the functional-design aspect of Inventor, you may be converting some iParts to Content Center components. Additionally, you may decide to utilize iParts and iFeatures for design development if your design needs require them.

In this chapter, you'll learn to

·     Create and modify iParts

·     Create and use iFeatures and punches

·     Copy and clone features

·     Link parameters between two files

·     Configure, create, and access Content Center parts

Working with iParts

image
iParts differ from standard parts in that they are essentially table-driven part factories, allowing for many different variations to be generated from the same basic design. When an iPart is inserted into an assembly, a dialog box appears that allows you to specify a variation of the original part from the table. Figure 7.1 shows an example of three variations of the same base iPart.

image

Figure 7.1 Three variations of the same part

Within the iPart factory, you can configure feature sizes by specifying different values for the same parametric dimension, you can choose to include or suppress entire features, and you can configure the iProperties of a part. In addition to these general configuration controls, you can configure thread features and work features such as work planes, axes, and points. There are two basic forms of iParts: table-driven and custom. Both types can be combined to create a table-driven part that allows custom input.

Each original iPart, often called a factory part, generates individually derived, noneditable member parts. Member parts placed within an assembly can be replaced with a different member of the factory. When a member part is replaced, generally all existing Assembly constraints will be retained.

iParts bring several advantages within assemblies. They essentially function as completely different parts, allowing dimensional changes, feature suppression, and transfer of iProperties and other values.

Creating and Modifying iParts

iParts are created from an existing part. Existing parts already contain features and parameters. Although you can modify a standard part by changing the parameter values, this will affect the part wherever it is used. To create configurations of a standard part, you must first convert the part into an iPart.

You can publish iParts to a custom content folder for use as Content Center components or as additional content for functional design, such as Frame Generator and Bolted Connections. Published iParts can also be used in other aspects of functional design such as Frame Generator.

Modifying the Parameter List

Before converting a standard part into an iPart, you should modify the parameter list and rename the parameters to something more meaningful than the default names, such as renaming d1 to Length. To explore these tools, follow these steps:

1.  On the Get Started tab, click the Open button.

2.  Browse for the file mi_7a_001.ipt located in the Chapter 7 directory of your Mastering Inventor 2015 folder and click the Open button.

Where to Get the Files

If you have not already downloaded the Chapter 7 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.  Click the Parameters button on the Manage tab.

4.  The Parameters dialog box opens, and you'll note that many of the parameters have been named already. Change the names of the unnamed parameters d0, d1, and d2 to LengthWidth, and Height, as shown in Figure 7.2, and then click Done to exit the Parameters dialog box.

image

Figure 7.2 The Parameters dialog box

image
Tips for Working with Parameters

Recall that you cannot use spaces in parameter names; however, you can use an underscore or capital letters to help separate words in the parameter names, such as Base_length or BaseLength.

Be aware that modifying the parameter name after creating an iPart table will not automatically update the parameter name in the table; therefore, parameters should always be named before being included in the iPart table to maintain consistency.

Parameter names will be used as column header names in the iPart table. Parameters that have been renamed will automatically be pulled into the iPart table. You can manually add unnamed parameters to the iPart table; however, it is a best practice to give all parameters to be used in the iPart meaningful names.

Selecting the Export Parameter column permits creation of custom iProperties within the part file. By exporting parameters as iProperties, you can easily access them in parts lists and bills of materials (BOMs).

Creating the iPart

image
Continuing from the previous steps where you modified the parameter list, you'll next create the iPart table, configure it to include columns of features you want to modify, and add rows for each new configuration of the part you want to create.

1.  On the Author panel of the Manage tab, click the Create iPart button. All the named parameters will automatically show up in the iPart table.

2.  To remove columns that you do not want to include in the table, click the parameter in the right pane and use the  button. You can also select column headers in the table and then right-click and choose Delete Column. Remove all the columns except Length, Width, and Height. Note that the Member and Part Number columns are default columns and cannot be removed.

3.  Add a row to the table so that you can create a variation of this part. Right-click anywhere in row 1, and choose Insert Row.

4.  Set Height to 40 mm and leave the other values as they are.

5.  Create additional rows until you have eight rows with the Length, Width, and Height values, as shown in Table 7.1.

6.  Once your table is complete, click the OK button.

7.  Find the Table node in the browser and click the + sign to expand the node. You will see each member (variation) of the iPart table listed, as shown in Figure 7.3.

Table 7.1 iPart table information

Length

Width

Height

100 mm

50 mm

20 mm

100 mm

50 mm

40 mm

100 mm

75 mm

20 mm

100 mm

75 mm

40 mm

200 mm

50 mm

20 mm

200 mm

50 mm

40 mm

200 mm

75 mm

20 mm

200 mm

75 mm

40 mm

image

Figure 7.3 iPart browser list

You can switch between members of the iPart by double-clicking a member in the list or by right-clicking it and choosing Activate. Making changes to the features or sketches will change the active member but will not automatically update the table. If you make a change and then go to set another member as active, you will be prompted to save the changes to the table ordiscard them. This is because the default edit mode is set to edit the entire iPart factory rather than the members individually. Changes made in the table will be carried through to the members either way. You'll learn more about adjusting the edit scope in the sections “Working with Sheet-Metal iParts” and “Changing Color in iParts” later in this chapter.

You can close this file without saving changes and continue on to the next section to explore the tools used to edit iParts.

Editing the iPart Table

image
To edit an iPart, you can double-click the Table node in the Model browser, or you can right-click and choose Edit Table. You can also right-click and choose Edit Via Spreadsheet to edit the table with Microsoft Excel. Although some iPart table-editing tasks can be done in both Inventor and Excel, others should be done only in Inventor. Follow these steps to explore the process of editing an iPart table:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_003.ipt from the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  Right-click the table in the browser and choose Edit Table.

4.  In the iPart Author dialog box, right-click the Length column header and choose Key. Then click the arrow and select 1 to designate that this is the first parameter by which this part should be specified.

5.  Set the width to be key 2 and the height to be key 3; then click the OK button to close the iPart Author dialog box.

6.  Right-click the table in the browser and choose List By Keys. This sets the members to be listed by parameter keys in descending order, creating a drill-down tree so you can select the length, then the width, and then the height, as shown in Figure 7.4. Note that the active member is designated by a check mark next to the appropriate key.

Key Selection Is Important When Creating iParts

You should take time to consider how your users will utilize the parts. For example, consider a socket head cap screw iPart. In the iPart, you might have diameter (1/4”, 5/16”, 3/16”), pitch (UNC or UNF), length (2”, 3”, 4”, 5”), and material (stainless steel, alloy steel). Each of these columns could be key 1, but you should consider what makes it easiest to navigate to the correct part. In many cases, you might want to make the material the primary key, with the diameter, pitch, and length as the second, third, and fourth keys. This means that the user will first select the material and only then be presented with the remaining diameters, pitches, and lengths for that given material. It would be a poor choice (in most cases) to have the pitch as the primary key because this is usually not the first descriptive factor when choosing a fastener.

7.  Right-click the table in the browser and choose Edit Table again.

8.  Click the Properties tab to see the list of iProperties that are available for this part.

9.  Locate the Project category in the left pane and expand it to reveal the Description property.

10.Select Description and use the button to include it in the iPart table.

11.Confirm that the Description column shows as a column in the table and then click the OK button.

12.Right-click the table in the browser and choose Edit Table Via Spreadsheet to open the table in Excel.

13.Select cells F2 through F9 and then right-click and choose Format Cells.

14.Set the cells to General and click the OK button. This is necessary to allow Excel to evaluate the expression you will build in the next step.

15.In cell F2, enter = C2 & “X” & D2 & “X” & E2.

16.Right-click cell F2 and choose Copy.

17.Then select cells F3 through F9, right-click, and select Paste. Figure 7.5 shows the Excel table complete.

18.Save the spreadsheet and close Excel.

19.Because your table now contains data that is not in the part file, you will be prompted to update the file. Click Yes in the message dialog box.

20.Right-click the table in the browser and choose Edit Table.

21.In the iPart Author dialog box, notice that the cells in the Description column are highlighted to inform you that there is a formula in those cells.

22.Click the OK button (or Cancel if no changes were made) to exit the iPart Author dialog box.

image

Figure 7.4 iPart browser listed by keys

image

Figure 7.5 Excel table used to add descriptions

You can examine the iProperties of the part file by clicking the part name in the Model browser and choosing iProperties from the context menu. If you check the Description field on the Project tab, you'll see the value from the iPart table/Excel spreadsheet. When you switch members of the iPart, the description is now automatically updated. You can then close the file without saving changes and continue to the next section.

Converting an iPart to a Standard Part

You can convert an iPart to a standard part file by right-clicking the table in the Model browser and choosing Delete. The part will assume the active members' feature values and states.

Including and Excluding Features

image
A common use of iParts is to create a configuration of a part family that might include features in some cases and not include them in others. You can add a column to the table to control feature suppression. To do this, follow these steps:

1.  On the Get Started tab, click the Open button.

2.  Open the file named mi_7a_005.ipt located in the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  Right-click the table in the browser and choose Edit Table.

4.  In the iPart Author dialog box, click the Suppression tab.

5.  Select the feature called Round_Boss1 and click the button to add it as a column in the table.

6.  Enter Suppress for the all the 100 mm length rows.

Suppressing vs. Computing

You can enter Suppress or ComputeS or C, and 0 or 1 for the suppress/compute cells. You can mix these options as well, meaning you can change only some values from Compute to S, for instance.

7.  Click the Verify button to ensure that you haven't entered a value that will not work, such as a spelling error. Errant cells will highlight in yellow, and you should fix them.

8.  Click the OK button to return to the model.

9.  Use the browser tree to activate different members, and notice that the boss features will be suppressed for all of the 100 mm members. Figure 7.6 shows the iPart Author dialog box.

image

Figure 7.6 Suppressing features

You'll notice that by suppressing the boss feature, we have suppressed both instances of the boss. This is because the boss was mirrored. To suppress just one boss, you could suppress the mirror feature; however, doing so would suppress one of the revolved features as well because it was included in the mirror. Keep this in mind when creating left and right configurations of the same part. Often, you will need to create separate features so that they can be controlled independently.

Creating Stacked, Toggled Features

Often when creating part configurations, you might need to create two features at the same location so you can toggle between the two features depending on the configuration. For instance, you might have an existing rectangular cut but then want to add an oblong cut in the same location so you can set the iPart to toggle between the two. When you attempt to place the oblong cut, Inventor warns that the feature did not change the number of unique faces and then results in an error. To correct this problem, simply accept the error, and then right-click the oblong cut and choose Suppress Features. Then you can set up the iPart table to toggle between the two features.

Including or Excluding Work Features in iParts

You can use the Work Features tab to indicate whether each work feature is included or excluded individually. A common use for this would be to create several work features in an iPart and then include only the one that is to be used for mating the specific iPart member in the assembly environment to control a specific offset value.

Working with Threaded iPart Features

You can change the thread parameters of a tapped hole or external thread feature for each member of the iPart table independently. Just use the Thread tab to include any thread parameters, which will vary. You should include all parameters that will vary between any of the table members; otherwise, the hole/thread feature may generate errors when you're switching between members. Often these errors may not become apparent until you attempt to publish your iPart to Content Center.

An example of this would be if you neglected to add the Class parameter to the table, even though not all of the members in the table have the same thread class. The thread class would then be set to the original thread class and would not be changed when the iPart is switched to a thread that does not include the original thread class. The same would be true, of course, if the Class column were included but not changed.

Working with Sheet-Metal iParts

You can configure a family of sheet-metal parts in the same way you would with a standard iPart—by adjusting lengths, widths, and so on—but sheet-metal parts have some additional controls that can be configured in an iPart. For instance, you can specify the sheet-metal rule, the sheet-metal unfold, and a named flat pattern orientation for individual members in an iPart. To edit the bend order, you must edit the member scope as opposed to making the edits per the iPart factory. Once the iPart is set to Member Scope, bend-order changes in the flat pattern are set to the active member. You can follow these general steps to set the scope of the edits:

1.  On the Manage tab, locate the Author panel.

2.  Click the Edit Factory/Member Scope drop-down and set it to Edit Member Scope. Figure 7.7 shows the drop-down.

image

Figure 7.7 Setting the iPart edits to Member Scope

Member Scope vs. Factory Scope

When you set the edit scope to Edit Member Scope, changes to the model such as suppressing a feature are automatically added to the iPart table.

Once the scope is set to edit just members, you follow these steps to adjust the bend order per iPart member:

1.  Activate the iPart member using the iPart table in the browser.

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

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

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

Directed Reorder 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.

Sequential Reorder You select each bend centerline glyph in the reorder sequence.

5.  Right-click and choose Finish Bend Order.

When you edit the iPart table, you will see that the FlatPatternBendOrder column is automatically added (because you are working under the member scope edit mode). The cell for the edited iPart member will show that it is using something other than the Default bend order.

Changing Color in iParts

To set iPart members to be different colors, you can create a custom iPart parameter on the Other tab and set it to the AppearanceColumn option. Then you can edit each member row of the iPart to be a different color/appearance. It is important that the name matches exactly, however, so be careful to match case. This means that entering red for Red will cause a mismatch. To avoid this, it is recommended that you use the member scope edit mode, as described in the previous section, to make color style edits to the part. This way, you can just set the member as active, change its appearance, and have the appearance change recorded in the iPart table automatically. To set up an Appearance column, follow these steps:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_012.ipt from the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  Right-click the table in the browser and choose Edit Table.

4.  In the iPart Author dialog box, click the Other tab.

5.  On the Other tab, click the Click Here To Add Value line.

6.  Type Color for the value name.

7.  Right-click the column header and choose Appearance Column, as shown in Figure 7.8.

8.  Type Default into the Appearance column for each of the three rows. Then click the OK button to exit the iPart Author dialog box.

Setting Colors

Note that if you do not enter Default or a valid Appearance style, you will receive a warning that states “Errors occurred while setting factory to specified member.” You can click Accept and then edit the table again.

9.  Ensure that Edit Member Scope is set (on the Manage tab, locate the Author panel and then set the drop-down to Edit Member Scope).

10.From the Quick Access bar (located at the top of the screen), select the Appearance Style drop-down and choose Cyan.

11.Expand the iPart table, use the keys to set the 25 mm × 50 mm member active, and then set its color to Red.

12.Change the edit scope to Edit Factory Scope using the iParts/iAssembly toolbar.

13.Use the keys to set the 50 mm × 50 mm member active and then set its color to Gold.

14.Right-click the table in the browser and choose Edit Table. You will receive a message asking whether you would like to set the table to match the document (that is, the part).

This demonstrates that when you are making edits to the model with the edit scope set to Factory, the changes to members do not get written back to the table automatically. Using the Edit Member Scope option is therefore recommended. You also get this message if you change the active member because the table is verified every time you switch members.

15.Click Yes; then take a look at the Appearance column to ensure that the colors match what you have set them to.

image

Figure 7.8 Creating an Appearance column

As mentioned earlier, you could also just edit the table and type in the color name. Experiment with this as you like, and then you can close the file without saving changes and continue to the next section.

Exploring the Authoring Options

The Options button, located in the lower-left corner of the authoring dialog box, allows you to create and edit part numbers and member names for iParts. You will typically want to set these naming options before you begin adding rows to the iPart table so that as rows are added, they are automatically named according to these options.

Notice the disk symbol located in the Member column header in Figure 7.9. This indicates that the Member column will be used as the filename for each iPart member. If you prefer to have the Part Number column used for the filenames, you can right-click that column header and select File Name Column.

image

Figure 7.9 Member column used for filename

A Member Name value is automatically created for each member as rows are added based on the settings for the part number and member name options. You can override these by editing the table in Excel, and you can even use a formula to create the names based on a concatenation of other column values in the table.

Generating Member Files

Once your iPart table is complete, you may want to generate the parts from the table. You can do this so the parts are established ahead of time, or you can allow the files to be generated automatically as they are used. If you have an iPart table with two dozen rows, it might make sense to generate them ahead of time. However, if you have an iPart table of 200 member rows, then it might make sense to allow parts to be generated only when, for example, a particular size is used. To generate member part files, right-click the table and choose Generate Members. Each member in the row will be created as a derived part based on the table values.

iPart Member File Save Locations

Because these parts are often used over and over in many assemblies, I recommend that you store them in a library folder. Recall that folders designated as libraries in your project file are handled as read-only by Inventor. The library directory where you want to save the iPart members is set up by you, and it is required that you use the same name as the factory library but preceded with an underscore. As an example, if you place the iPart factory file in a library folder named Fasteners, Inventor will automatically place all iPart members generated from that factory part in a second library folder named _Fasteners.

However, you are not required to store iParts in libraries. If you do not use libraries and you place an iPart member into an assembly or use the Generate Members option, Inventor will create a folder of the same name, and at the same level as the iPart factory, and store the iPart members there. For example, if you have an iPart factory file named ClipBracket.ipt saved at C:\Mastering Inventor\, then when ClipBracket.ipt is used in an assembly, a subdirectory called ClipBracket is created (C:\Mastering Inventor\ClipBracket), and the iPart member file is created there. Custom iPart members are always stored in a location specified by the user.

Creating Custom iParts

A custom iPart is an iPart factory that has one or more columns designated as a custom parameter column. A custom parameter column allows input of any value and, in turn, generates a custom iPart with infinite variations. Custom iParts are valuable for creating tube and pipe lengths, structural steel members, and other parts that require unique size input at the time of insertion. To designate a column as a custom parameter column, simply right-click the column and select Custom Parameter Column. Columns that are set as keys are not permitted to becustom columns.

Rather than setting an entire column to be custom, you may want to set only the column entry for a single member to be custom. To do this, you can right-click any cell in a nonkey column and choose Custom Parameter Cell. Once cells or columns are designated as custom, you can right-click and set both columns and cells to restrict input to a specified range and increment.

Here is a common example of setting a range for a custom part:

1.  Right-click the column to set the Length column to be custom (it cannot be a key column).

2.  Right-click the column to set the range so the part can be placed only in lengths from 25 mm to 150 mm.

3.  Right-click the column to set the increment to 5 mm so the lengths are limited to standard sizes within that range.

4.  When the custom iPart is placed into an assembly, the size is then specified.

5.  Unlike standard iParts, custom iParts are saved to a location of your choice at the time of placement.

Figure 7.10 shows the options for creating a custom column.

image

Figure 7.10 Custom column settings

Testing the iPart

Before placing a completed iPart into production for others to use, test the accuracy and interface of your part by inserting the iPart using Place Component within a blank assembly file. Using Place Component, insert every member in the table and inspect and/or measure the placed component.

Moving the test forward, create an IDW file with a base view of your assembly. You will also need to generate a parts list with the desired columns and verify the accuracy of each cell. Once you are assured of having accurate member components, you can place this iPart into a project library folder or other location to be used in production. If using this iPart in conjunction with the functional-design features of Inventor, you will need to publish the factory iPart to a custom Content Center library. Publishing to Content Center is covered in more depth later in this chapter.

No Zero-Value Dimensions

You should not attempt to create a zero-value dimension as a method of suppressing features. Zero-value dimensions can create unpredictable results when the zero value is set back to some value greater than zero. Often the dimension will solve in the wrong direction, causing feature profiles to become invalid and create errors within your iPart. It is better to create a column to suppress individual features, rather than attempt to do so through dimensions.

Editing the iPart Factory

Editing an original iPart factory follows the same workflow as creating an iPart. If you've placed the original iPart factory into a project library folder, you will not be able to edit it within that same project. Instead, you should create a new project file for the purpose of editing library parts. When creating a new project file, you can either define the workspace for the project file by placing the project file in the library subfolder or just duplicate your original project file and remove the library paths using the Project Editor dialog box. Any files within the library path will now be editable with this specific project file.

With the new Library Edit project file active, open the iPart you want to edit. Locate the table in the Model browser and either double-click or right-click to activate the iPart Author dialog box. At this point, you can edit any part of the table. When you have completed your editing, you can save the part to its original location.

Can't Generate iPart Members?

When changes are made to an iPart factory and they impact existing iPart members, you should be able to use the Generate Files option to replace the iPart members (provided the folder or files are not set as read-only by Windows). However, sometimes you'll find that Inventor won't generate new versions of existing iPart members once edits are made, even when you right-click them in the table and choose Generate Files and have checked the read-only status. Although the reason for this behavior is often unclear, you can generally get around it by browsing to the location of the iPart members and deleting them. Then you can return to the iPart Factory and choose Generate Files.

You can convert an iPart factory component into a standard parametric part by deleting the table attached to the iPart. Simply right-click the table in the Model browser and select Delete. The part will revert to a parametric part with no history of the iPart functionality.

Using iParts in Designs

Using an iPart in an assembly design is a bit different from creating parts within an assembly. To place an iPart member of a particular size into an assembly, you will use the Place Component tool to browse and place the iPart factory. Upon placing the iPart factory into the assembly, you'll be presented with the Place iPart dialog box, from which you can specify the member or choose from the keys you set previously. Keep in mind that if you didn't set any keys in the iPart table, all of the columns will be listed in the Keys tab of the Place Standard iPart dialog box. Figure 7.11 shows the placement of an iPart that has three keys set.

image

Figure 7.11 Placing an iPart into an assembly

In Figure 7.11 Length is Key 1, Width is Key 2, and Height is Key 3. Keep in mind that for the best results keys should be set from top to bottom in the Place iPart dialog box because the values are filtered in that order. However, Inventor does not prevent you from setting Key 3 first and then Key 1. But working out of order with keys can create some confusion and unexpected results in the values you see listed in the drop-downs.

Once an iPart is placed, you might find that you need to change to another size, color, or configuration. To change between iPart members, follow these steps:

1.  Locate and expand the iPart in the assembly browser tree.

2.  Right-click the table.

3.  Choose Change Component.

This opens the iPart placement dialog box, which allows you to specify a new member to be used in place of the existing one. Figure 7.12 shows the specific selection path for changing the component. This replacement procedure will replace only the selected component instance.

image

Figure 7.12 Changing the component

If you want to replace all exact duplicate members of the iPart within this assembly, follow these steps:

1.  Right-click the part within the graphics window or the Model browser.

2.  Select Component.

3.  Choose Replace All. A dialog box appears, allowing you to select the original iPart factory.

4.  Once the original iPart factory is selected, you will be prompted with the iPart placement dialog box to allow you to select the specific member to be used as the replacement.

When a component is replaced with a different member of the same family, as with iParts, normally all Assembly constraints will be retained. If the replaced component is of a different family, the Assembly constraints might be broken. The same is true of parts in the same family if the original part used a certain feature to constrain to and the replacement part has that feature suppressed.

image
iPart Factories in Assemblies

You should be aware that Inventor does not allow an iPart factory file to be placed into an assembly. If you attempt to do so, only a member of the factory will be placed instead. However, keep in mind that if you create a regular part file, place it into an assembly, and then turn it into an iPart factory, changing the factory table does not place a member file but simply updates the factory. Using factory files in assemblies in this manner is not the intended workflow for iParts.

iFeatures are features that have been extracted from an existing part file and configured for reuse in other parts. If you are familiar with Autodesk® AutoCAD® software, you might relate iFeatures to blocks, in that you can write out blocks for reuse in other drawings. Any feature based on a sketch can be used as an iFeature, but there are some best practices to follow when creating sketches and features to be extracted for iFeatures. Once extracted, the iFeature is stored in an external location and can be placed into any other part file. Inventor is supplied with a number of standard iFeature files as well. iFeatures cannot currently be published to Content Center.

Working with iFeatures

Using iFeatures in your designs can greatly simplify your workflow and accelerate productivity, especially if your designs contain repetitive features. Figure 7.13 shows an example of a sheet-metal part that could be created quickly using iFeatures.

image

Figure 7.13 Sheet-metal part with iFeatures

iFeatures used in sheet-metal parts are authored with center points that allow them to be placed as sheet-metal punches. iFeatures are stored in a Catalog folder defined in the Inventor application options. By default, the catalog is located in the Inventor install directory, but you can customize the location by selecting the Tools tab, clicking Application Options, and then choosing the iFeatures tab. On the iFeatures tab, you can set the catalog path to a directory of your choosing, most often located on a network server. You can create additional subfolders in the Catalog folder as required to better organize your iFeatures. Extracted iFeatures are saved with .ide filename extensions. iFeatures are also available online from such locations as http://cbliss.com. Often these online files contain the extracted iFeature and the original file it was created from. These can serve as good examples of how to set up complex geometry for iFeature extraction.

The following are some tips for working with iFeatures:

·     Keep your iFeatures clean, and do not include projected geometry or reference geometry unless required.

·     If dependent geometry is required, have it dependent only on geometry within the iFeature.

·     You should avoid the use of origin work planes, axes, and the origin center point for work features.

·     Use parallel and perpendicular constraints to other geometry in the iFeature rather than horizontal and vertical constraints.

·     Know that updating table-driven iFeatures does not update existing instances of the iFeature.

·     Save iFeatures before placing them in other parts.

Creating iFeatures

Once you have a part that consists of a feature or features that you want to reuse in the design of other parts, you can easily extract those features and place them into the catalog. The chief advantage of using iFeatures is that the original part does not need to be open in order to copy the feature. In addition, you can alter any of the parameters at will when inserting the feature into a new part.

To extract a part feature or features, go to the Manage tab and click the Extract iFeature button on the Author panel. Select the feature to be extracted, from either the Model browser or the graphics window. If additional features exist that are dependent on the selected feature, they will be included in the feature selection as well but can then be removed during the iFeature creation process if not needed.

Recall that a feature is dependent on another feature if it uses the other feature as a reference in the sketch or feature creation. For instance, if you created a sketch on the face of an Extrude feature, that sketch (and any feature created from that sketch) is inherently dependent on the base Extrude feature because it uses the face as a reference plane. Therefore, if you extracted the base Extrude feature, the dependent feature is automatically included, but it can be removed if not needed. Figure 7.14 illustrates how to remove a dependent feature (Fillet1) while creating an iFeature.

image

Figure 7.14 Removing a dependent feature

A standard iFeature will typically require a profile plane in order to position the geometry onto a new part. Named parameters and values involved in the selected feature are transferred from the existing part into the new iFeature. In Figure 7.15, notice that prompts will be added for each of the named parameters. You can edit the prompts as needed. You'll also notice that range and list limits have been set for some of the parameters. This allows you to control the input for iFeatures by limiting them to a predefined list of sizes or a specified range between sizes. When inserting this iFeature into a different part in the future, you will be prompted to enter new values for these parameters.

image

Figure 7.15 Parameters and prompts

Placing an iFeature

To place an iFeature in a standard part (not a sheet-metal part), browse to the stored iFeature and select the face you want to use for placement. During the placement, you can adjust the rotation angle and size parameters. To see a simple example of how iFeatures are extracted and placed, follow these steps:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_017.ipt from the Chapter 7 directory of the Mastering Inventor 2015 folder.

3.  On the Manage tab, click the Extract iFeature button.

4.  In the Model browser, click Extrusion2 as the selected feature. The dialog box will be populated with the parameter information found in that feature.

5.  Click the parameter named E2_Ext_Ang and use the  button to remove it from the parameter list. This parameter is the taper angle of the extrusion, and by removing it from the list you are ensuring that users of iFeatures in the future cannot specify a taper.

Adjusting Extracted Features

In this case, the parameters have been renamed previously using the Parameters dialog box. However, you can adjust parameter names and the corresponding prompts at this point if needed.

You can also adjust the default values for the parameters without adjusting the current model, as well as add lists and ranges to each parameter using the Limits column.

6.  For this example, accept the default for the rest of the parameters and click Save.

7.  Notice that Inventor takes you straight to the Catalog folder. This location is specified in the Application Options dialog box on the iFeature tab and can be changed if needed. Use the list of Frequently Used Subfolders on the left of the Save As dialog box to go to the Chapter 7 folder and name this iFeature SquareSocket.ide. Click the Save button to save the file.

8.  Next, you'll place the iFeature back into the model as a test. On the Manage tab, select the Insert iFeature tool.

9.  Click the Browse button to go to the Chapter 7 folder.

10.Locate and select the SquareSocket feature you just created (or use the file called mi_7a_025.ide) and click the Open button.

11.Select the top face of Extrusion1 to use as the profile plane.

12.Once the plane is selected, set the angle to 45 degrees, use the flip arrow to ensure that the feature is placed in the correct direction, and then click Next.

13.Enter 20 mm for the E2_Circ_Dia parameter and then click the edit icon (it looks like a pencil), or click in the space below the Diameter row or on another row in the dialog box to set the row out of edit mode.

14.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 as active. The refresh option is a bit picky in this way. Keep in mind, however, that the preview does not need to be refreshed to build to the specified value correctly.

15.Once the size parameter has been adjusted, as shown in Figure 7.16, click Next.

16.You will be presented with two options for placing the iFeature; choose Activate Sketch Edit Immediately, and then click Finish.

17.You will see that the iFeature sketch is set and ready to be edited and constrained into place so that it can't be moved accidentally.

image

Figure 7.16 Inserting a simple iFeature

You'll notice that there is some extra geometry included in the sketch. This geometry came from the original feature from which you extracted the iFeature.

It would have been the best practice to prep the sketch and remove this geometry from the sketch before extracting. However, in this case you were not instructed to do so in order to illustrate the presence of relic geometry at this point. It's often a good idea to save a copy of your original part file and use it to clean up unwanted geometry before extracting iFeatures.

You can click the Finish Sketch button and close the file without saving changes.

Taking the Time to Constrain the Sketch

You should also notice that the sketch is currently underconstrained. In particular, it has no dimensions or constraints holding it in position. You can place general dimensions into the sketch to anchor it in place. Also present is some relic geometry that originated from the sketch from which the iFeature was extracted. It is poor practice to extract iFeatures without cleaning them up first, so eliminate this stray geometry beforehand.

It is also good practice to create a separate part file from which to generate an iFeature rather than attempting to use a part file designed for production. You can copy the part features from a production part into your iFeature test part using one of the copy or cloning methods discussed in the upcoming pages.

Editing an iFeature File

Once iFeature (IDE) files have been extracted and tested, you can open them in Inventor and edit them much as you do iParts. Follow these steps to explore the options involved in editing an iFeature:

1.  Select the Get Started tab, click the Open button, and then browse for the Chapter 7 directory in your Mastering Inventor 2015 folder.

2.  Locate and open the file SquareSocket.ide you created in the previous exercise. If you did not complete that exercise, you can use the file mi_7a_025.ide in the Chapter 7 directory.

Continue exploring the iFeature edit tools by following these general instructions:

·     Use the Edit iFeature icon to refine parameter names, sizes, and instructional prompts for the placement of iFeatures.

·     If the iFeature has dependent features, you can edit them as well.

·     You can rename the iFeature if you want to configure it in a more in-depth manner by using the iFeature Author Table dialog box.

·     The iFeature Author Table dialog box allows a table to be added to the iFeature so that rows and columns can be added to configure the iFeature in the same way you configured a part file using the iPart Author dialog box.

·     Once you've added the table to the iFeature, you can further edit it by clicking the Edit Using Spread Sheet icon to open the table in Microsoft Excel.

When creating iFeatures, you'll find it a good idea to keep the original IPT file that you used to create the IDE file. This file is often useful in case you want to totally redesign the iFeature or make a similar iFeature.

Creating Punch Features

Punch features are really just iFeatures with extended functions that are slightly different in behavior from standard iFeatures. Punch features must have a single sketch center point in the base sketch to be extracted. The sketch center point will be used to locate the punch feature upon insertion into sheet-metal parts. The destination parts will require an active sketch containing sketch center points for the location of the punch feature. It is the center point in the iFeature punch and the center point in the placement sketch that allow punch features to be precisely placed and constrained beyond the capabilities of the standard iFeature.

Including Placement Instructions

You can embed an instructional document detailing the placement selection requirements for more complex shapes that require faces to be selected in a certain order or need more information about size and settings. Here are the steps for including placement instructions:

1.  On the Tools tab, click Insert Object.

2.  Select Create From File, browse for the precreated instruction file, and then click the OK button.

3.  The file will show in the 3rd Party browser node, as shown here:image

4.  Right-click the embedded object and select Placement Help to allow this file to be accessed from the feature's dialog box during placement.

Punch Features in Standard Non-Sheet-Metal Parts?

Although the Punch tool is not available for use in the standard part-modeling environment, you may have a need to quickly and precisely place a feature multiple times in a way that lends itself to the Punch tool.

To do this, you can use the Convert To Sheet Metal Part button (on the Model tab) to temporarily convert the part to a sheet-metal part. Once this is done, you can use the Punch tool as required.

After you've placed the punches, you can use the Convert To Standard Part button (found in the Setup drop-down of the Sheet Metal tab) to convert the part back. This will leave some relic sheet-metal parameters in your part file, but that shouldn't cause an issue.

Creating Punch Features

When creating a punch feature, consider that in normal use most features extend through the thickness of the sheet metal. Therefore, it is important to use the Thickness parameter when creating the iFeature. Constructed properly, the punch feature will adjust to the thickness of any sheet-metal part to which it is applied.

The part used in the following steps is a simple sheet-metal part with one cut feature. Figure 7.17 shows the sketch underlying the cut feature. The sketch was created utilizing a single center point, which will be used for placement when inserting the punch feature. There was no need to anchor the sketch since it was created for the sole purpose of extracting a punch iFeature.

image

Figure 7.17 A sheet-metal sketch

Follow these steps:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_027.ipt from the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  On the Manage tab, select the Extract iFeature tool (you'll find it on the Author panel).

4.  Select Cut1 in the Model browser.

5.  Click the radio button at the top of the dialog box to toggle the iFeature type from Standard iFeature to Sheet-Metal Punch iFeature.

Punches and Center Points

If you have created multiple center-point locations within your sketch, you will receive an error message when trying to create the punch feature. Recall that by using the Center Point icon next to the Construction icon, you can switch extra center points in your sketch to standard points so that they will not interfere. In this example, you have only one center point within the sketch, even though there are other points locating two of the circles on the ellipse. The others have been made standard points as described ahead of time.

6.  Under the Manufacturing area, specify the punch ID as K775. Although not required, if it's included, this punch ID can be retrieved and placed onto a drawing in the form of a punch note or punch table so the shop floor will know which punch to use.

7.  Click the Select Sketch button for Simplified Representation and then click Sketch3 in the Model browser. Simplified sketches are optional but may help represent complex sketches more cleanly in the detail drawing.

8.  When your dialog box resembles Figure 7.18, click Save, and select the Punches folder in the Chapter 7 folder of your Mastering Inventor 2015 directory.

9.  Name the punch feature K775.ide and then save the file.

image

Figure 7.18 Extracting a sheet-metal iFeature

iFeatures Are Powerful Tools

These tools allow you to quickly create standard features in your models. Examples include o-ring grooves, louvers, bosses, ribs, electrical connector punches, patterns of holes, and an infinite number of other features. Another major advantage of iFeatures is that they enforce standards. Since the iFeature can be designed to allow the user to select predefined sizes only, the possibility of error is greatly reduced. Take a few moments to examine your designs, and you'll likely see many opportunities for iFeatures.

Placing a Sheet-Metal Punch Feature

When working on a sheet-metal part, you can access iFeatures through the Punch tool or the Insert iFeature button on the Manage tab. The Punch tool is optimized for sheet-metal parts, so unless you are placing a regular iFeature, you should always use the Punch tool. Prior to placing a feature, you must have an unconsumed, visible sketch containing one or more center points from which the punch will position itself. Follow these steps to place a sheet-metal punch:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_029.ipt from the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  Inspect the Model browser to see that Sketch2 is visible. This sketch has been prepared for you to use in placing your new punch feature on the three center points.

4.  Next, locate and select the Punch Tool button on the Sheet Metal tab.

5.  Select the K775.ide file you created in the previous exercise from the Punches folder and click the Open button. (If you did not complete the previous exercise, you can browse to the Punches folder of the Chapter 7 directory and choose the file called K777.ide.) You will notice that every unconsumed center point within the sketch will be populated with the selected punch.

Center Points

If you want to reserve a sketch center point for some other feature, click the Geometry tab in the Punch Tool dialog box and hold down the Ctrl key while selecting the center point to be removed. If you want to place only one center point, hold down the Ctrl key, click the sketch away from a center point, and then click the center point where you want the punch. If you have more than one visible, unconsumed sketch, the center points will not be automatically selected because you will need to tell Inventor which sketch to use.

6.  Click the Geometry tab and set the angle to 90.

7.  Click the Size tab and set InsertDia to 20 mm, Major to 50 mm, and Minor to 25 mm.

8.  Click the Edit icon (it looks like a pencil) or click in the space below the Diameter row or on another row in the dialog box to set the row out of edit mode.

9.  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 as active. The refresh option is a bit picky in this way. Keep in mind, however, that the preview does not need to be refreshed to build to the specified value correctly. Figure 7.19 shows the punch parameters.

10.Click the Finish button to complete the punch action.

11.Click the Go To Flat Pattern button to view the flat pattern.

12.Right-click the Flat Pattern node in the Model browser and choose Edit Flat Pattern Definition.

13.Click the Punch Representation tab, set the drop-down to 2D Sketch Rep And Center Mark, and then click the OK button. Note the simplified version of the punches. This can be useful for placing grouped punches or helping to simplify drawings that have many punches on them.

image

Figure 7.19 Placing a punch

Note that you could use the Insert iFeature option to place the punches, but you would not be offered the same placement options. Instead, its behavior would be similar to that of a standard iFeature, requiring constraint of the placed punch by anchoring it to the base feature. In general, it is best to use the Punch tool for sheet-metal parts rather than placing punches as a standard iFeature.

Note that whereas the iFeature tool is available in the standard and sheet-metal environments, the Punch tool is available only in the sheet-metal environment. You can close this file without saving changes when you have finished.

Reusing Existing Geometry

Geometry reuse is a productive technique in Inventor. You can reuse existing features and sketch geometry to create additional features within the same part or even on other open parts. You don't need to create additional new sketches to utilize this technique. The following sections show how to copy sketches and features and develop dependent and independent relationships between the features.

Copying Features

image
Copying features in Inventor is a relatively simple procedure using the Model browser. In an existing model, simply right-click a feature within the browser and select Copy. Next, select a different face within the model, right-click, and select Paste. Figure 7.20 shows a preview of the placement and the Paste Features dialog box.

image

Figure 7.20 Copied features

Beware of Projected Loops

When you select a face with the Project Geometry tool rather than selecting individual edges, a projected loop is created. If you select an edge, a projected edge is created. It is important to understand that when you right-click a feature that is based on projected loops, you will not get an option to copy it.

To resolve this, you can locate the projected loop by expanding the Sketch node in the browser and then right-clicking it and choosing Break Link. Once you break the link of the projected loop, you can copy the sketch. When you select just an edge to project, rather than a face, the result is a projected edge. Projected edges can be copied without breaking the link. But if you have the need to break the link of a projected edge, you can do so by right-clicking it in the graphics area and choosing Break Link.

There are two questions to consider when copying a feature:

·     What should Inventor do with features that are built based on the feature you are copying?

·     What should Inventor do with the dimensions for your new feature?

You'll explore the features first.

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_031.ipt from the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  Right-click Extrusion2 in the Model browser, and notice that there is no Copy option. This is because there is a projected loop present in the sketch.

4.  Choose Edit Sketch from the context menu.

5.  Expand the Sketch2 node in the browser and notice the projected loop. This was created when the face the sketch is on was projected into the sketch.

6.  Right-click the Projected Loop node and choose Break Link.

Now that the link from the loop to the face is broken, the sketch is underconstrained. In real life, you'd take the time to reconstrain the sketch so that future changes to the base feature would not upset Sketch2 or Feature2. Most likely you'd do this by deleting the projected outer lines and reapplying the 20 mm dimensions to the projected edges of the base feature. For this exercise, though, you can leave the sketch underconstrained.

7.  Click the Finish Sketch button to exit the sketch.

8.  Right-click Extrusion2 in the Model browser and choose Copy.

9.  Right-click anywhere in the blank space of the graphics area and choose Paste.

10.Drag your cursor over any face of the part, and you will see a preview of the copied feature.

11.In the Paste Features dialog box, set the Paste Features drop-down to Dependent, and you will notice that the fillets are now in the preview as well because they are dependents of Extrusion2.

12.Click the front face of the part to position the new feature, as shown in Figure 7.20.

13.Use the plus sign–shaped arrows in the center of the copied feature to move the feature around the selected face.

14.Use the C-shaped arrow to rotate the new feature, and notice that the rotation angle is reflected in the dialog box and can be adjusted there as well.

By default, the dimensions of the new feature will be independent, meaning that because the original feature has a width of 25 mm, the new feature will have the same value, but the two will not be linked. However, if you set the Parameter drop-down to Dependent, the dimensions of the new feature will reference the original feature so that if the original width changes from 25 mm to 35 mm, the new feature follows.

15.Set the Parameter drop-down to Dependent also and then click Finish.

16.Locate and edit Sketch2 in Extrusion2 and set the diameter dimension to 6 mm.

17.Finish the sketch, and notice that the new feature follows the edits of the original.

Once you've copied the feature, you should edit the copied feature sketch to properly anchor the sketch on the destination face. When editing a dependent sketch, notice that the dimensions indicate that they are being driven by a parameter from the original feature. If you change the dimensions from a parameter value to a numeric value, you will break the dependency with the original sketch. You can close this file without saving changes, or you can leave it open to experiment with cloning a feature from one part to another part in the next section.

Cloning

Cloning is the process of copying feature geometry from one open part to another. The cloning process creates independent features, meaning that the new feature in the new part will have no relationship to the original feature in the original part unless set up manually.

To clone a feature from one part to another, you must first have both parts open in Inventor. Here are the general steps:

1.  From the source part, right-click the feature to be copied in the Model browser and choose Copy.

2.  Switch to the destination part, right-click anywhere and choose Paste.

3.  Drag your cursor over the face of the part you want to paste onto, and you will see a preview of the copied feature.

4.  Click the face and then click Finish when the part is positioned to your liking.

The primary difference between copying features within the same part and cloning features between two parts is that parameters can be set to be independent only during the cloning process.

It will be necessary to fully constrain and anchor the feature sketch to the new part once the feature has been copied. To accomplish this, simply edit the new feature sketch and project construction geometry from the new part base feature to serve as anchor points.

Linking Parameters Between Two Files

image
You can establish a relationship between two parts, between two assemblies, or between a part and an assembly by linking the files' parameters. This can allow you to place all the design information in one file and link other files to it so the intent of the design is maintained. Here are the steps to do this:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_033.iam from the Chapter 7 directory of your Mastering Inventor 2015 folder.

This is a simple pin and plate assembly. Your goal is to link the shaft diameter of the pin to the hole diameter in the plate. To do this, you will first edit the pin part called mi_7a_034.ipt.

3.  Select mi_7a_034.ipt from the browser, right-click, and choose Edit (or just double-click the pin in the graphics area).

4.  Once the part is active for edits, click the Parameters button on the Manage tab.

5.  At the bottom of the Parameters dialog box, click the Link button, as shown on the left of Figure 7.21.

6.  Adjust the Files Of Type drop-down to show Inventor Files; then open the file mi_7a_035.ipt from the Chapter 7 directory of your Mastering Inventor 2015 folder and click the Open button.

7.  This opens the Link Parameter dialog box, allowing you to choose which parameters to link to this part. Click the button next to the parameter named Diameter and then click the OK button.

This will add the selected parameter to the user parameters in the pin part, making it available for you to reference in another parameter.

8.  Locate Shaft_Diameter in the list, activate the cell in the Equation column, and clear the existing value.

9.  Click the flyout arrow, as shown in Figure 7.22, and choose List Parameters from the flyout menu.

10.Select Diameter from the Parameters lists and then add - 1 mm so that your final shaft diameter equation is Diameter - 1 mm. Subtracting 1 mm from the shaft diameter creates a loose hole.

11.Click Done at the bottom of the dialog box to return to the model.

12.Click the Update button from the Quick Access bar (at the top of the graphics area) to see the model update if needed. If you have the Immediate Update check box selected in the Parameters dialog box, the part updates right away, but the updates may need to be pushed up to the assembly.

13.Finally, right-click and choose Finish Edit to return to the assembly level.

image

Figure 7.21 Linking parameters

image

Figure 7.22 Setting a parameter to reference a linked parameter

Now the shaft diameter is linked to the hole diameter in the part called mi_7a_035.ipt. You can open or edit mi_7a_035.ipt and change the hole diameter value to see the change carry through to the shaft of the pin. Linking parameters in this way allows you to place design information in one location and pull it into many other parts for automatic updates.

Copying Sketches

Quite often it is desirable to copy existing part sketches to another location within the same part or a different part. A good example of this would be creating a loft feature where each profile sketch may simply change size.

In the example shown in Figure 7.23, the part contains one unconsumed sketch and multiple work planes parallel to the XY origin plane. To copy an existing sketch, simply right-click the target sketch and select Copy. Then select the destination work plane, right-click, and select Paste. Pasted sketches are always independent of the original sketch and will create additional parameters for each copy.

image

Figure 7.23 Copying a sketch

The following exercise will explore copying sketches:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_039.ipt from the Chapter 7 directory of the Mastering Inventor 2015 folder.

3.  Right-click Sketch1 in the Model browser and choose Copy.

4.  Click any edge of the work plane closest to the sketch and then right-click and choose Paste.

5.  Repeat this for each of the remaining work planes.

6.  Select the 20 mm dimension in each of the copied sketches and adjust the minor axis on each of the sketches, decreasing the dimension value by 4 mm on each subsequent sketch, as shown in Figure 7.23.

7.  Edit Rectangular Pattern1 and change the pattern count to 6.

8.  Right-click any edge of the new work plane and choose New Sketch.

9.  If it's not done automatically, project the origin center point to the sketch. You can use the Project Geometry tool on the Sketch tab and select the center point of the ellipse in any of the other sketches.

As you can see, copying sketches can be a quick way to duplicate repetitive geometry. To carry this thought through, you can create a loft utilizing all the sketches, including the sketch consisting of just the projected origin point. Apply a tangent condition to the projected point to achieve a result that holds the work plane as the extent of the loft.

In this example, you copied a sketch within the same part. The procedure to copy an existing sketch to another part requires that both parts be open at the same time. Right-click the original sketch and then select Copy. Then, after selecting the destination part work plane or part face in the second file, right-click and select Paste.

Once the sketches are pasted, they can be edited at any time by adding additional geometry, changing dimensions, or simply using the pasted geometry for reference.

Using Flip Normal

At times you may find that your sketch “flips” when you're pasting it onto a work plane. In many cases, you can easily fix this by right-clicking the work plane and selecting Flip Normal. This flips the positive axis of the work plane. Then when you paste the sketch onto the work plane, it will no longer be flipped.

Introducing Content Center

In Inventor 2015, Content Center is available in two forms: Desktop Content and the traditional Autodesk Data Management Server (ADMS)–based Content Center. The ADMS-based Content Center is a set of database libraries contained in Microsoft SQL and is generally used when sharing a central customized Content Center over a network. The other is a stand-alone install of Content Center that typically resides on your local machine. The stand-alone install is the default form of Content Center. No matter how you choose to install Content Center, you can select which libraries to use. These libraries provide standard content in several common international standards, such as ANSI, ISO, and DIN, just to name a few. Figure 7.24 shows the complete list. Once properly configured and populated, Content Center provides an organized method for part and feature reuse.

image

Figure 7.24 Content Center libraries

You can think of these libraries simply as recipes for creating parts because no actual part files exist in the Content Center file store. Instead, Content Center is a table of part parameters stored in the Content Center database. Once these library databases are installed, you can access them from Inventor and place common parts into your designs.

Understand that it is at this point the Content Center part file is created. Up until this point, the part existed only as a definition in the database table. If you work in a shared environment, the Content Center part files might typically be stored on a network server so that as users collaborate on designs, they have access to the same part files used within the assemblies. Because the Content Center library database files are just definitions of the files, they can be installed on the users' local machines or on a network server, or both.

Content Center provides support for functional design using the design accelerator, Frame Generator, and other features within Inventor. When you're using these tools, the parts generated are pulled from the Content Center libraries. You can use Content Center in conjunction with standard iParts and iFeatures organized within libraries in the project.

Configuring Content Center

Content Center, loaded with all the standard libraries, provides in excess of 800,000 variations in parts. To optimize loading, you will want to configure only the appropriate standards for your use. Installing all libraries will cause Inventor to take more time to search and index the data. There are two installation strategies for Content Center. Depending on how you work, you may want to install the desktop Content Center or the ADMS version.

Installing Content Center for a Stand-Alone User

If you work as a stand-alone user, I recommend you use the Desktop Content method. No server setup or login is required because the Content Center libraries are installed in the Libraries folder, at a path similar to C:\ProgramData\Autodesk\Inventor 2015\Content Center\Libraries\. You can insert the install media and install or reinstall the Content Center libraries at any point by following the installation steps. Once the libraries are installed, you use the Place From Content Center tool or the Open From Content Center tool to access the Content Center libraries.

Installing Content Center for a Collaborative Environment

If working in a shared group, you will likely want to install Content Center on a server location instead of, or in addition to, the Desktop Content libraries. When installing on a server, you will install the libraries on the Autodesk Data Management Server. The ADMS is essentially just the interface with which you interact with the SQL database program. Once the ADMS is installed and the required Content Center libraries are loaded, users log into the ADMS through Inventor.

When deciding whether to install Content Center libraries on a network server or install them locally, consider whether you plan to create and use a custom library. If not, you may not need to install Content Center on a server, and you can choose to install the libraries on all the local machines only. Because the standard Content Center libraries are all read-only databases, they cannot become out of sync; therefore, two users can access two different instances of the standard libraries and work without issue. If you plan to create custom Content Center libraries, however, I recommend you install on a network server so that as the library is updated over time, all users are pulling from the same source. You can consult the installation media for more information on installing the ADMS and the Content Center libraries.

Desktop Content vs. ADMS Content Center Libraries

If both the Desktop Content and the ADMS Content Center libraries are installed, then the current radio button selection under the Access options found by going to the Tools tab, clicking the Application Options button, and selecting the Content Center tab will control which is used. By default this is set to Inventor Desktop Content and will need to be changed to Autodesk Vault Server if the ADMS Content Center libraries are installed and are intended to be used.

Managing Your Memory Footprint

Installing all libraries into the ADMS will increase your overall memory usage substantially. As mentioned earlier, installing only the libraries you use will keep Content Center efficient. As you will see in the coming pages, you can create a custom Content Center library based on the standard libraries and include only what you require. Once the custom library is created, standard libraries can be removed from the ADMS. You can add them back at any time by reinstalling them from the Inventor installation disks.

Configuring Content Center Libraries in the Project Files

Once you've installed the ADMS and the required libraries, you will need to configure the project file to ensure that all required libraries are included in the project. To do this, you will want to close all files in Inventor so that the project file can be edited. Then follow these steps:

1.  In Inventor, select the Get Started tab and click the Projects button.

2.  In the Project Editor dialog box, ensure that your project is set as active and click the Configure Content Center Libraries button at the lower right of the Projects dialog box to open the Configure Libraries dialog box, as shown in Figure 7.25.

3.  Use the buttons at the bottom of the dialog box to update, import, add, or remove libraries for the project. Removing libraries from a project will speed up the interaction between Inventor and Content Center when placing a part because fewer library tables are required to be read, searched, and indexed. Once a library is removed, you can add it to the project again at any time.

image

Figure 7.25 Configuring Content Center libraries

If you only occasionally access a certain library because you typically do not work with that standard, you might install it but remove it from your Inventor project. When you do need to access this library, use the Configure Libraries dialog box to load it for use and then unload it once you have finished. Although the suggestion to add and remove libraries may seem like a hassle, it will pay off in time savings because you will not find yourself waiting for the libraries to load every time you access Content Center.

Using Content Center

Content Center is used in many areas of Inventor. Components from Content Center are used in functional-design tools, such as the Shaft Generator or Frame Generator, as well as in individual, reusable components in general assembly design. Content Center is also available for use within the part environment using the Place Feature tool.

Placing Components into an Assembly

Let's take a closer look at placing components into an assembly from Content Center.

1.  Make sure you have either Desktop Content or the ADMS installed and the ANSI content library loaded to continue with this example.

2.  If you are running Content Center through the ADMS, ensure that you are logged in to the ADMS by clicking the Inventor icon and selecting Vault Server  Content CenterLog In.

If you are already logged in or logged into Vault, Log In will be grayed out and will not be an option in your menu.

3.  Enter your login information, if known. By default, the ADMS installs with a user account called Administrator with no password set. You can also select the Content Center library's Read-Only check box to access content without logging in.

4.  Specify the name of the server on which you installed the ADMS. If you have installed the ADMS on your local machine, enter localhost. In the Database text box, enter the name of the ADMS database; the default is Vault.

Placing Parts from Content Center

Once logged in to the ADMS or if you have installed Desktop Content (there is no login required), you are ready to place parts from Content Center. To do so, follow these steps:

1.  From the Get Started tab, click the Open button.

2.  Open the file mi_7a_044.iam from the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  On the Assemble tab, click the Place From Content Center icon. Check to see that the three buttons indicated in Figure 7.26 are selected. From left to right these buttons are Filters, AutoDrop, and Tree View:

Filters Button Select ANSI to filter out all other standards. To turn the filter off after this exercise, click the Filters button again and deselect ANSI. If you do not have the ANSI library installed, you can select another library, but the size and bolt names will differ from the following steps.

AutoDrop Button This button turns on the ability to automatically size components based on geometry in the model.

Tree View Button This button splits the screen so that the Category View pane is accessible on the left of the dialog box.

4.  Select the Fasteners category in the left pane, browse to Bolts and then Round Head, select Cross Recessed Binding Head Machine Screw – Type I, and click the OK button.

5.  In the model, zoom in to one of the caster wheel assemblies and take note of the empty holes.

6.  Pause your mouse pointer over one of the holes on the castor plate.

You will see the AutoDrop icon activate and flicker as Inventor indexes the database for an appropriate size. If no matching size can be found in the database, a cursor note will appear saying so. If an appropriate size is found, a cursor note will display it, and a preview of the part will be shown.

7.  Once the size appears, click the edge of the hole to set the screw in place. The AutoDrop toolbar will appear along with the red grip arrow.

8.  Drag the grip arrow up or down to specify the length of the screw. Note that only lengths found in the database are available.

9.  Click the Apply button and continue placing screws as you see fit. Experiment with placing the mouse pointer over one of the large diameters in the caster assembly to watch AutoDrop attempt to find an appropriate size. Figure 7.27 shows the AutoDrop toolbar.

Once you've experimented with placing bolts from Content Center, you can close this file without saving changes or continue exploring the other options discussed. Here is a brief description of each of the tool icons shown in the AutoDrop toolbar in Figure 7.27:

1.  Insert Multiple The first icon is available when Inventor identifies multiple targets that are like the selected target. In this case, the other holes in the plate are picked up and previewed. If you apply the screw now, four screws will be placed at once. If you do not want the multiples to be placed, you can click the Insert Multiple icon to turn it off.

2.  Change Size The second icon is grayed out while Insert Multiple is on. It inserts the part and opens the Part Family dialog box, which allows you to edit the component.

3.  Bolted Connection The next icon opens the Bolted Connection Component Generator and allows you to place bolt, nut, and washer sets as a group.

4.  Apply The fourth icon sets the previewed components and allows you to continue placing more components of the same family.

5.  Place The last icon sets the components and exits the AutoDrop mode.

image

Figure 7.26 Place From Content Center settings

image

Figure 7.27 Placing a screw with AutoDrop

The AutoDrop toolbar is context-sensitive, so the icons may vary depending on the component to be placed and the selected geometry. If you press F1 on the keyboard while the AutoDrop toolbar is displayed, Inventor will open the help file and list all the icons and their descriptions.

Now that you've placed Content Center components, let's examine where Inventor is storing the newly generated Content Center files. Select the Tools tab, click Application Options, and then click the File tab. Look for the file path indicating the default Content Center files, as shown at the top of Figure 7.28.

image

Figure 7.28 Content Center files storage path

This is where Inventor will place all standard parts placed from Content Center by default. Typically you should change this path to a path that is on the network server, particularly if you're working in a multiuser environment. If you work only on your local hard drive, you will still likely want to change the path to be similar to the path where you save your Inventor designs.

If this path is left at the default, Content Center part files will be saved on your local machine. This causes a problem when a co-worker opens an assembly you created. There is one more place where you can set this path, and that is in the project file under Folder Options, as shown at the bottom of Figure 7.28. It is important to note that a path set in the project file takes precedence over a path set in application options. If the project file is set as Content Center Files = [Default], then the files are stored at the application options path.

Only standard Content Center files are stored at this location. Custom-sized Content Center part files, such as standard steel shapes, pipes, and so on, are stored at a path chosen by you at the time of their creation.

Customizing Content Center Libraries

You should be aware of a few options customizing Content Center Libraries. You can find these settings on the Content Center tab of the Application Options dialog box.

Refresh Out-Of-Date Standard Parts During Placement

When this option is selected, existing standard part files are automatically replaced with newer versions. For instance, if you update a standard part with your part number in the Content Center library tables but that part has already been placed in other assemblies and therefore already exists in the Content Center parts file folder, having this option selected will update the Content Center file folder and place the new version in the assemblies.

Custom Family Default

Set this option to place a custom Content Center part as a standard part. When you place a custom part as standard, the part file is saved in the Content Center files folder and is considered a standard part.

Access Options

This sets the source of the Content Center libraries. You can choose between Desktop Content and the ADMS/Vault server.

Standard Content Center libraries supplied with Inventor are designated as read-only and cannot be modified. If you need to create custom part libraries or modify standard content such as adding part numbers or material types, you can do so by creating a custom Content Center library. Custom libraries are initially set as read/write libraries so that you can add and modify content.

Do You Need to Use Content Center?

Many people find the file structure of Content Center–generated files to be at odds with the way they store purchased and standard parts. If you find this is the case with your setup, you might want to use Content Center to generate parts but then save copies of them under your own file structure as needed. Often, commonly used components are generated from Content Center in this manner and then placed in a company's purchase part directory after the Part Number and Description iProperties are adjusted.

Creating Custom Libraries for ADMS Installs

You add libraries from the Autodesk Data Management Server console when using Content Center with the ADMS. You can access the ADMS by selecting Start  All Programs  Autodesk  Autodesk Data Management  Autodesk Data Management Server Console. Typically this would be done on the server machine. Figure 7.29 shows how to create a custom library.

image

Figure 7.29 Creating a custom library in the ADMS

Once you're logged into the ADMS console, expand the folder in the top of the left pane, right-click the Libraries subfolder, and select Create Library. Create a new library called Mastering Inventor.

Once the library is created, follow these steps:

1.  Select the Get Started tab.

2.  Click the Projects button.

3.  Click the Configure Content Center Libraries button at the bottom-right corner of the Project Editor dialog box.

4.  Ensure that the In Use check box for this new library is selected so that the project is configured to include it.

Creating Custom Libraries for Desktop Content

You can create a custom Content Center library for Desktop Content through the Content Center configuration of the Project Editor. To do so, follow these steps:

1.  Select the Get Started tab.

2.  Click the Projects button.

3.  Click the Configure Content Center Libraries button at the bottom-right corner of the Project Editor dialog box.

4.  Click the Create Library button and enter Mastering Inventor into the input box, as shown in Figure 7.30.

5.  Click the OK button.

6.  Ensure that the In Use check box for this new library is selected so that the project is configured to include it.

image

Figure 7.30 Creating a custom library with Desktop Content

Copying Existing Libraries into Custom Libraries

After creating a custom library, you can copy entire or partial contents of existing standard libraries into your custom library. You might use this process when you want to simplify one of the standard libraries, remove portions of the library that are not needed in your work environment, or edit component properties such as part numbers. Here are the steps to copy families to a custom library:

1.  Access the Content Center Editor from within Inventor by selecting the Manage tab and clicking the Editor button on the Content Center panel. This editor looks similar to the Content Center dialog box.

2.  Locate the library or the part family within a library that you want to copy, right-click, and choose Copy To  Mastering Inventor, as shown in Figure 7.31.

image

Figure 7.31 Copying a Content Center family

The library must be included in the project file configuration list in order to be visible within the editor. If you copy an entire library to your custom library, then the entire folder structure and contents will be replicated in your custom library. If you copy an individual part to your custom library, then only the affected category structure will be replicated in the custom library along with the copied part.

To copy only a portion of the category structure, browse to the last hierarchical portion of the structure that you want to replicate. Otherwise, starting from the top and copying the structure will replicate the entire structure.

Setting Category Properties

Each category within Content Center contains category properties. Within the category properties is general information regarding the category itself. The General tab contains the category name, category image, and source library.

Creating Multiple Material Types for Content Center Families

It's pretty easy for your design department to have the Content Center parts reflect their own internal part numbers so that bills of materials and parts lists will extract this information automatically. Doing this is as simple as copying the appropriate standard Content Center categories to a custom read/write library and editing the tables to include the new part numbers.

However, if multiple material types are used for the same component type, then multiple copies of the family can be made to accommodate this. For instance, if you use stainless steel fasteners of a given type for certain design instances and also use galvanized fasteners of the same type in other design instances, you would most likely need these to have separate part numbers.

You can use the Material Guide to add materials in one of three ways.

·     You can edit a family table and select the members to add new materials to. Then click the Material Guide button or right-click and choose Material Guide to copy the selected members, add them to the family table, and assign the new materials to them.

·     You can use the Material Guide for an entire family, copying all members with a new material and adding them to the existing family. Select the family in the Content Center Editor and click the Material Guide button, or right-click and choose Material Guide. Then choose the option called Add Materials As New Family Members, thereby copying all members into the same family table and setting a new material at the same time.

·     You can create new families of a different material as well. Select the family in the Content Center Editor and click the Material Guide button, or right-click and choose Material Guide. Then choose the option Create New Family For Each Material, thereby copying the entire existing family and setting a new material for this new family at the same time.

The Parameters tab contains parameters used within the category to assist in the description of parts located within that category. Figure 7.32 illustrates the parameter list in the ANSI Socket Head category.

image

Figure 7.32 Socket head parameters

Within these parameters, some are optional and some are required. If you are placing a part within this category, you must map your part properties to all required fields for proper operation. Optional fields do not require mapping.

What this means is that if you are planning on publishing a large number of your own parts to Content Center, your part parameters must match the category parameters. If you are unable to match the parameters, consider creating a new category.

Expect Some Inconsistency

The mapping required for Content Center is not consistent for all types of parts because of the evolution of these tools over time. Some of the categories require authoring before you can publish a part. Other categories are open for publishing without authoring. The requirements for restricted categories are driven by tools such as the design accelerator, Bolted Connection, and AutoDrop, which require certain parameters so they can intelligently place components. One inconsistency is Frame Generator. Since Content Center steel shapes predate Frame Generator, which originally had its own shape library, there weren't any authoring requirements. Just be aware of the inconsistencies.

Right-clicking an individual Content Center part will allow you to view the family properties and mapping of that part. Compare the category parameters of the part with the parameters of the intended category. Matching the two parameter lists ensures that the part will map easily into that category.

Editing a Custom Content Center Family

A Content Center family is an individual part, similar to an iPart. The part consists of a standard factory part with a family table attached that generates any of the optional table values.

You can edit any individual part by first switching the library view to your custom library designation, as shown in Figure 7.33.

image

Figure 7.33 Editing a Content Center part

In the previous example, you switched the library view to the Mastering Inventor custom library. Right-click a part located within the custom library and select Family Table. This launches a dialog box that allows the user to modify values, copy/paste, add/delete rows, or suppress existing rows within the table. The dialog box also allows the addition, deletion, and modification of columns and properties.

Publishing Parts to Content Center

Developing a process for reusing parts within your company's design environment is essential for standardization and improved productivity. Part of this process may include publishing existing Inventor parts stored in project libraries. Both normal parts and iParts can be published to a custom Content Center library.

The act of publishing a standard part into the custom library adds a family table to the published part. Exported part parameters will be converted to table parameters when published to the custom Content Center. iPart tables are converted to family tables when published.

Preparing the Part for Publishing

If the part you intend to publish will be included in an existing Content Center family category (that is, fasteners, shaft parts, and so on), you can use the Component Authoring tool to prepare components with the necessary properties for use as “smart” content in the Content Center library. You can do this by following these steps:

1.  On the Get Started tab, click the Open button.

2.  Open the file mi_7a_064.ipt from the Chapter 7 directory of your Mastering Inventor 2015 folder.

3.  Select the Manage tab and click the Component Authoring button on the Author panel (you may need to use the drop-down to find it).

4.  From the drop-down list, select Fasteners  Bolts and select Other. Note that the graphics and selection prompts change depending on the category of component selected.

5.  Select the geometry for each row in the dialog box that corresponds to the dialog box graphic to map iMate placement to this part (iMates are preprogrammed Assembly constraints).

6.  Click the Parameter Mapping tab. Note that the parameters listed in the light yellow/orange rows are required, whereas the others are optional. Click the … button for the Grip Length row.

7.  In the Part Template Parameters dialog box, expand the browser to find Parameters  User and select GripLength. This maps the part parameter to the corresponding family table parameter. Click the OK button.

8.  Map the Nominal Diameter and the Nominal Length parameters to the NomDiameter and NomLength model parameters, respectively (you can find these at Parameters  Model rather than Parameters  User).

9.  Click the OK button to write the mapped parameters and iMates to the part file. You could also click the Publish Now button to start the publishing process.

You can author parts ahead of time and use the Batch Publish tool to publish one or more unopened parts at once. Or you can publish one part at a time, as covered in the next section. Figure 7.34 shows the Component Authoring dialog box tabs. You can close this part without saving changes and move on to the next section, which is about publishing parts.

image

Figure 7.34 Component Authoring tabs

Publishing the Part

To publish a part to Content Center, you must have a custom library with read/write capability created, and your current project file must be configured to include this custom library. In this example, you will publish a simple part that has already been authored to the custom read/write Content Center library called Mastering Inventor. If you haven't already created this library, review the steps in the section “Creating Custom Libraries for Desktop Content” or “Creating Custom Libraries for ADMS Installs,” depending on which method applies to your setup. Follow these steps to publish a part:

1.  On the Get Started tab, click the Open button.

2.  Browse for the file mi_7a_068.ipt located in the Chapter 7 directory of the Mastering Inventor 2015 folder and click the Open button.

3.  Select the Manage tab and click the Publish Part button on the Content Center panel.

4.  Select the Mastering Inventor library, and set the language as required; then click Next.

5.  Ensure that Category To Publish To is set to Fasteners  Bolts  Other; then click Next.

6.  Notice that most of the parameters are already mapped; this is because this part has previously been authored following the steps in the section “Preparing the Part for Publishing.” Recall that all parameters in the light yellow/orange rows are required. Click the … button for the Thread Type row.

7.  In the Part Template Parameters dialog box, expand the browser to find Threads  Thread1, select Type, and then click the OK button.

8.  Click Next in the Publish Guide dialog box.

9.  Select Nominal Diameter, Nominal Length, and Part Number in the left pane and use the arrow button to include them in the right pane. This defines keys that are available for selection upon placement of the Content Center part once published. At least one Key column must be defined. Click Next to continue.

10.Enter EyeBolt for the family name and set the Standard Organization option to ANSI. Only the family name is required; however, designating the Standard Organization option allows the part to be listed when filtering per standard. You can also type a custom standard into the field, such as your company name. This allows you to create a filter for the parts you published.

11.Click Next, and notice the preview thumbnail. You can use the Browse icon to select a different graphic file for use as a thumbnail, if one exists.

12.Click Publish to complete the task and add this part to your custom Content Center library. Click the OK button in the successful publish confirmation box.

This creates the part family table in the Content Center library, but at this point there is only one row in the table. Typically you will want to add a row for each size or different type of the component. You can do this by using the Content Center Editor (on the Manage tab). Figure 7.35 shows the family key and properties steps of the Publish Guide. You can close this part without saving changes.

image

Figure 7.35 Publishing a part to Content Center

You can also convert a part to a table-driven iPart before publishing and include the rows for each size and type of the part configuration in the iPart table. Once you have a workable iPart that behaves correctly, you can open the original factory iPart and publish the part. The iPart may be a custom iPart or a fully table-driven factory. iParts containing multiple row definitions in the table will convert to a fully table-driven Content Center part. You can find more information on iParts in the section “Working with iParts” at the beginning of this chapter.

Before using a newly published Content Center component in production, test the part in a blank assembly for proper function.

Adding a New Category to Content Center

If you need a unique category for your own specific parts, you can simply add a new family of parts instead of using an existing category. You can do this from the Content Center Editor (accessed from the Manage tab). Make sure the library view is set to view only the read/write library in which you intend to create the new category and that the tree view is enabled. Then right-click in the blank space in the Category View pane and choose Create Category. You can also create a subcategory by right-clicking an existing category and selecting Create Category.

image

The Bottom Line

1.  Create and modify iParts. iParts are the solution to creating parts that allow for an infinite number of variations without affecting other members of the same part family already used within your designs.

1.  Master It You use a purchased specialty part in your designs and would like to create the many size configurations that this part comes in ahead of time for use within assembly design. How would this be done?

2.  Create and use iFeatures and punches. Creating a library of often-used features is essential to standardization and improved productivity within your design workflow.

1.  Master It You want to be able to place common punches, slots, and milled features quickly rather than having to generate the feature every time. What is the best way to approach this?

3.  Copy and clone features. You do not have to create iFeatures to reuse various part features in your designs. If a part feature will have limited use in other designs, it is often better to simply copy it from part to part or from face to face on the same part.

1.  Master It You need to reuse features within a part or among parts. You consider iFeatures but realize that this feature is not used often enough to justify setting up an iFeature. How would you proceed?

4.  Link parameters between two files. Linking design parameters between two or more files allows you to control design changes from a single source, making it easy to update an entire design from one file.

1.  Master It You want to specify the overall length and width of a layout design in a base part and then have other components update as changes are made to this part. What are the methods to do this?

5.  Configure, create, and access Content Center parts. Content Center provides a great opportunity to reuse database-created geometry within assemblies and within functional-design modules. The Content Center Editor provides the means to add custom content into Content Center. You can create and add custom libraries to your current project file.

1.  Master It You would like to change the part numbers in some Content Center components to match the part numbers your company uses. You would also like to add proprietary components to Content Center. How do you customize Content Center?