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

Chapter 14. Exchanging Data with Other Systems

Many Autodesk® Inventor® users need to bring files created by other CAD applications into Inventor or need to export files from Inventor to other formats. For instance, if you design components that others use in their designs, you might need to output files to a standard format so that others can use them with a different software package. Or, if you are a manufacturing “job shop,” you may receive many different file formats from customers that you need to bring into Inventor.

In this chapter, you'll learn to

·     Import and export geometry

·     Use Inventor file translators

·     Work with imported data

·     Work with Design Review markups

Importing and Exporting Geometry

Essentially, three data types make up a 3D model: curves (or wires), surfaces, and solids. Wire-frame models are composed of only wires that define the size and shape but lack volume. A surface model, on the other hand, is composed of wires and faces that define the surfaces but still lacks a solid filled volume. A solid model is composed of wires and faces that define surfaces that in turn define the solid filled volume. Understanding the hierarchy of geometry data will help you understand the issues that can occur when translating from one of these data types to another.

There are different ways in which wires and curves are defined. If you are translating files that represent wires and curves as Non-Uniform Rational B-Splines (NURBS) to a format that represents wires and curves as simpler basis splines (B-splines), there might be something lost in translation. Likewise, when you translate a surface model, if the surface normal direction were to get reversed (think positive vs. negative), you will have translation issues. And so it is with translating solids; if a solid model is translated so that a gap is formed where two surfaces meet, then translation may not be complete.

Translation of curves, surfaces, and solids occurs between different software packages because these packages use different methods of geometric accuracy. Accuracy controls such things as how close two points in space are before being considered a single point or how close two edges can be before they are considered connected, and so on.

To help with translating from one software package that solves curves using method A to software that uses method B, you can create an intermediate, or neutral, file. Some common neutral file formats are Initial Graphic Exchange Specification (IGES), Standard for the Exchange of Product (STEP), and Standard ACIS Text (SAT), among others. Other common translations include importing files from Autodesk® AutoCAD® and Autodesk® Mechanical Desktop® software into Inventor. In these cases, you will be working with the DWG file type.

Working with Neutral File Formats

Although using neutral formats will help avoid problems, keep two things in mind when translating files:

·     Generally speaking, you should strive to keep the number of file formats between the source software and the destination software as low as possible.

·     Not all neutral file formats are created equal.

Translating DWG and DXF Files

When a DXF or DWG file is imported into Inventor, the file is translated into an Autodesk Inventor part, assembly, and/or drawing file, based on the import settings and the geometry present in the original file. When imported, the original DXF or DWG file is not changed; instead, the data is created in a new Inventor file or multiple Inventor files. When exported from Inventor to a DWG, a file is translated into AutoCAD objects and a new DWG file is created. The new translated DWG is not linked to the Inventor file from which it was created. Instead, the DWG data is fully editable within AutoCAD. You can use the file mi_14a_014.dwg in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for DWG files.

The process of translating DXF and DWG files follows similar steps. To import a DWG file, follow these steps:

1.  Click Open on the Get Started tab.

2.  Set the Files Of Type drop-down to AutoCAD DWG Files (*.dwg).

3.  Select the DWG file you are going to import.

4.  Click the Options button and choose Import. (If you are translating a number of DWG files, you can set Import to be the default by clicking the Tools tab, selecting the Application Options button, and choosing the Drawing tab.)

5.  Once you've selected Import, as shown in Figure 14.1, click the OK button.

6.  This returns you to the Open dialog box, where you will click the Open button to start the DWG/DXF File Wizard. Note the Configuration drop-down box.

7.  If you have an import configuration already saved, you can specify it now and click Finish. If you have not yet created a configuration template, click Next to go to the Import Destination Options dialog box.

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Figure 14.1 Importing a DWG file

You need to consider a number of options when importing DWG files, depending on the DWG data input and the intended translation output. The following sections discuss these considerations in relation to the import options.

Layers and Objects Import Options

Once you click Next in the DWG/DXF File Wizard screen, you will be presented with the Layers And Objects Import Options screen. On this screen you can select which layers or objects to include or exclude for importing. These two methods of selection are available:

1.  Select By Layer Use the check boxes to control which layers will be imported. Unchecking a layer will exclude all objects located on that layer.

2.  Select By Object Uncheck the All check box and then select objects in the Import Preview window.

You can combine layer and object selections in order to create a specific selection set. Once the layers and objects are selected, you can click the Next button to continue to the Import Destination Options screen.

Importing 3D Solids

Once you've selected the layers and objects to be imported, you will be presented with the Import Destination Options screen. If the AutoCAD DWG has 3D solids, you can check the 3D Solids check box to translate them into Inventor part files. Use the Solids To Single Part File check box if you want multi-body solids to be translated into an Inventor part file. Leave this option unchecked if you want each solid body in the DWG to be created as an individual Inventor part file and automatically placed in an Inventor assembly.Figure 14.2 shows the import options for 3D solids.

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Figure 14.2 3D data options

Set the destination folder to a path in which you want to have the part files created and choose Use Default File Names to allow Inventor to name the resulting part files automatically. If you choose this option, the new Inventor parts will be given a name based on the DWG name and be incremented by a value of 1.

For instance, if the DWG is named Engine.dwg, then the solids in the DWG will be named Engine1.ipt, Engine2.ipt, Engine3.ipt, and so on. If Use Default File Names is left unchecked, each solid in the DWG will be named Part1.ipt, Part2.ipt, Part3.ipt, and so on.

Importing 2D Data

If the DWG contains a combination of 3D and 2D data that you want to import, you can set the options in the Destination For 2D Data area to handle the 2D data. If the DWG has only 2D data or has both but you want to import only the 2D data, then you can leave the 3D Solids check box deselected and set only the Destination For 2D Data area of the Import Destination Options dialog box, as shown in Figure 14.3. Selecting the New Drawing radio button translates the DWG data to a new Inventor DWG or IDW. If you check Promote Dimensions To Sketch, the 2D data is placed in a draft view that is created in the Inventor drawing.

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Figure 14.3 2D data options

Importing Title Blocks and Borders

You can use the Title Block and Border radio buttons to convert an AutoCAD title block DWG into an Inventor title block or border. When you do this, be sure to click the Mapping Options button (located in the lower-left corner of the dialog box) to set the layer and font mapping options shown in Figure 14.4. You can click the Symbol radio button to translate the 2D data into a sketched symbol for use in an Inventor DWG or IDW file.

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Figure 14.4 Mapping Options

Importing AutoCAD Blocks as Sketched Symbols

To import AutoCAD blocks as Inventor sketched symbol definitions, you can use the Symbol radio button. This can provide a quick way to convert common drawing symbols for use in your Inventor drawing templates.

Importing AutoCAD Part Drawings as New Inventor Parts

Click the New Part radio button to translate AutoCAD 2D data into a new IPT sketch to be used for the creation of a new part model. Choose to create either a 3D or 2D sketch within the file, depending on the type of geometry needed.

Inventor has both a decimal and a fractional unit style for dimensions. When dimensions are translated, if Inventor detects that the AutoCAD file employs a scientific, decimal, engineering, or Windows desktop style, those styles are converted to decimal style. AutoCAD fraction and architectural styles are mapped to Inventor fractional style.

Think Before Importing AutoCAD Geometry

Although you might be tempted to import 2D AutoCAD geometry and start extruding away, you do need to keep a few things in mind. If this is a part that will never change, or if it is a reference part, this approach is probably fine. However, if you are re-creating old AutoCAD data to be used in your Inventor models as part of a fully parametric design, you might consider modeling the parts from scratch. It will take longer, no doubt. However, modeling from scratch allows you to place the design intent into the parts, which you simply cannot do by importing. You can create the model in a proper order, and with the proper constraints, that will allow you or others to easily modify it in the future.

Units, Templates, Constraints, and Configurations

Whether importing to 2D or 3D, you will use the Templates area to specify which template to use for each of the file types to translate to. In the Import Files Units area, you can specify the units if they do not match the units that Inventor detects from the AutoCAD file. The detected unit is based on the INSUNITS system variable in the DWG file.

You can use the Constrain End Points and Apply Geometric Constraints check boxes to allow Inventor to place constraints on sketch entities when it can. Endpoints found to be coincident will be given Coincident constraints, lines found to be parallel will be given parallel constraints, and so on.

Once all these options are configured, you can click the Save Configurations button, shown in Figure 14.5, to write out a file to use the next time you convert a DWG file. Doing this allows you to convert files more accurately and more quickly.

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Figure 14.5 More import destination options

When all the configuration settings have been made and saved, click Finish to start the import process. Inventor will create the new files based on your configurations and leave the files open in the current Inventor session.

Mechanical Desktop DWG

Autodesk Mechanical Desktop (MDT) was a 3D parametric modeler similar to Inventor that was developed on top of the existing AutoCAD platform. Once Inventor was created, Autodesk stopped developing MDT and has since discontinued support for it. If you have files that were created using MDT, they can be translated to Inventor part and assembly files. If the source files contain geometry or features that are not recognized in Inventor, they are omitted, and the missing data is noted in the browser or the translation log file. No links are maintained to the existing MDT files. You must have MDT on your computer to import files into Inventor. Note that the AutoCAD Inventor suite does not ship with MDT. If you have a need to use MDT for translation, you can download the last version that Autodesk released, MDT 2009, from the Autodesk website, or you can purchase or request installation media.

MDT's native file format was the DWG file, and you can import MDT DWG files using the Options button in the Open dialog box just as you would a regular DWG. However, if Inventor detects that it is an MDT file, you are given the option to read the data as an MDT file or as an AutoCAD or AutoCAD Mechanical file, as shown in Figure 14.6.

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Figure 14.6 Reading MDT file contents

Although many of the options for templates, units, and configuration settings are the same as previously described for regular DWG files, the assembly and part options are specific to MDT files, as shown in Figure 14.7.

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Figure 14.7 MDT assembly and part options

Consider the following items when migrating MDT files to Inventor:

·     Broken views, base section views, and breakout section views from MDT will be turned into base views.

·     Exploded views will become unexploded views (no tweaks applied).

·     Importing discards (AMPARDIMS) from MDT automatically creates associative model dimensions in Inventor.

·     If Move With Parent is selected in an MDT file, Inventor aligns all views according to the view type.

·     If a parent view is missing in an MDT file, a child view is not created in Inventor.

·     Inventor centerlines and center marks are automatically generated during translation; therefore, they might not be the same as in the MDT file.

·     Radial section views have broken alignment in Inventor.

In addition to importing MDT files one at a time, you can use the Inventor Task Scheduler to batch the translation from MDT to Inventor. It is important to ensure that the MDT files are migrated to the latest version of MDT before attempting to translate them into Inventor files.

STEP and IGES

Standard for the Exchange of Product (STEP) and Initial Graphic Exchange Specification (IGES) are nonproprietary file formats you can write data to in order to exchange data among proprietary software. When a STEP or IGES file is opened in Inventor, one part file will be created if the file contains only one part body; otherwise, you can create multiple Inventor part files placed within an assembly file.

Although no links are maintained between the original STEP or IGES file and the Inventor files created from them, when importing an updated STEP or IGES file, Inventor updates the geometry and maintains all modeling constraints and features applied to that STEP or IGES file. You can use the files called mi_14a_014.stp and mi_14a_014.igs located in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for STEP and IGES files.

To import a STEP or IGES file, follow these steps:

1.  Click Open on the Get Started tab and set the Files Of Type drop-down to STEP Files (*.stp, *.ste, *.step) or IGES Files (*.igs, *.ige, *.iges).

2.  Select the file you intend to import.

3.  Click the Options button, and you will be presented with the Import Options dialog.

In the Import Options dialog, you can choose from three save options:

1.  Save In Workspace Writes the files to the Workspace folder defined in your current project file. The files are saved as Inventor files during the import process.

2.  Select Save Location Allows you to specify where the resulting Inventor files will be saved. If the translated file contains separate solid bodies, you can configure the import to save those files to one location and the top-level assembly file to another location.

3.  Save At Import File Location Writes the resulting Inventor file(s) to the same location as the original file. Figure 14.8 shows the import save options.

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Figure 14.8 STEP or IGES save options

In the Translation Report area, choose to embed the report in the imported 3D model file (it will be placed as a node in the browser), or choose to save the report to disk. Note that you can choose both of these options or deselect them both in order to skip saving the translation report altogether.

In the Entity Types To Import area, use the selection buttons to specify the inclusion of solids, surfaces, wires, and points in the import action. Click the Import Assembly As Single Part check box to turn a multi-body STEP or IGES into a single-part file. Then choose from one of two options:

1.  Single Composite Feature This option allows you to import the assembly as a single composite feature into a single-part file.

2.  Multiple Solid Part With this option, you can import the assembly as individual solid bodies into a single-part file.

The Import Into Repair Environment option checks the model for errors and creates a repair node in the browser. You can edit, diagnose, and repair imported base bodies in the repair environment.

Click the Import Multiple Solid Parts As Assembly check box to turn a multi-body STEP or IGES into individual part files. When imported, the new Inventor parts will be given a name based on the filename and incremented by a value of 1. For instance, if an IGES were named 4278_T.igs, then the Inventor parts will be named 4278_T 1.ipt, 4278_T 2.ipt, 4278_T 3.ipt, and so on.

If you leave both of those check boxes deselected, you can specify how surface objects will be translated:

1.  Individual Surface Bodies Imports surfaces as individual surfaces in a single-part file.

2.  Single Composite Feature Imports surfaces as a single composite in a single-part file.

3.  Multiple Composite Features Imports surfaces as multiple composites all contained in a single-part file. Composites are created for each level, layer, or group, according to the Create From information specified.

composite is a collection of surfaces, as opposed to a single quilt of surfaces. A composite can consist of any combination of single- or multiple-faced surfaces or closed volume surfaces. Often these surfaces will not be connected, even if they appear to be. Composites can be used when many surfaces are imported as an expedient way of getting surface data into Inventor for reference or inspection.

You can also specify which units the imported geometry will be converted to and the postprocess options, as listed here:

1.  Check Parts During Load This option performs a quality check on the imported data. Bad data is marked with a symbol in the browser and any remaining data is not checked. If the parts are determined not to have any errors, they are marked with a green check mark in the browser. Checking parts can significantly increase the time required to translate a file.

2.  Auto Stitch This option stitches surfaces into a quilt or solid, when possible. If the stitch results in a single body, it is promoted out of the construction environment; otherwise, it remains in the construction environment.

3.  Enable Advanced Healing This option allows small alterations in the surface geometry in order to stitch the surfaces.

Figure 14.9 shows the STEP and IGES options.

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Figure 14.9 STEP or IGES import options

Many Inventor users prefer to send and receive STEP files to and from vendors or clients because they find that STEP files import better than other file formats such as IGES. Here is a list of attributes that make STEP a popular choice:

·     STEP files can retain the original part names when importing to an assembly.

·     STEP creates instances for duplicated parts. If you are sent a STEP of an assembly created in another software package and that assembly has 12 instances of a certain screw size, Inventor will typically create just one file for the screw and instance it 12 times instead of creating 12 different files.

·     STEP files can maintain assembly hierarchy, meaning that subassembly structure can be translated. In other formats, assemblies may be translated with all parts at the top-level assembly.

·     STEP translates part colors, whereas other formats generally do not contain the information needed to carry part colors across different platforms.

·     STEP format is governed independently and is not tied to a particular modeling kernel; as a result, it is often considered a more standard format.

To export a file as a STEP, click the Inventor button and then select Save Copy As. In the resulting dialog box, set Save As Type to STEP Files (*.stp, *.ste, *.step). Click the Options button to set the STEP version. You can also choose to include sketches. Included sketches are translated to the STEP file in named groups.

To export a file as an IGES, click the Inventor button, select Save Copy As, and set Save As Type to IGES Files (*.igs, *.ige, *.iges). Click the Options button to set the IGES output to either surfaces or solids. You can choose to include sketches. Included sketches are translated to the IGES file in named layers.

SAT

Standard ACIS Text (SAT) files are written in the standard file exchange format for the ACIS solid modeling kernel. You can use the file mi_14a_014.sat located in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for SAT files. To import a SAT file, follow these steps:

1.  Click Open on the Get Started tab.

2.  Set the Files Of Type drop-down to SAT Files (*.sat).

3.  Select the file you want to import.

4.  Click the Options button, and you will be presented with the Import Options dialog box.

In the Import Options dialog box, you can choose from three save options:

1.  Save In Workspace Writes the files to the Workspace folder defined in your current project file (see Chapter 1, “Getting Started,” for more on projects and workspaces). The files are saved as Inventor files during the import process.

2.  Select Save Location Allows you to specify where the resulting Inventor files will be saved. If the translated file contains separate solid bodies, you can configure the import to save those files to one location and the top-level assembly file to another location.

3.  Save At Import File Location Writes the resulting Inventor file(s) to the same location as the original file.

In the Entity Types To Import area, use the selection buttons to specify the inclusion of solids, surfaces, and wires in the import action.

The Import Into Repair Environment option checks the model for errors and creates a repair node in the browser. You can edit, diagnose, and repair imported base bodies in the repair environment.

Use the Import As Single Part check box option to turn a multi-body SAT into a single-part file. Then choose from one of two options:

1.  Single Composite Feature Imports the assembly as a single composite feature into a single-part file

2.  Multiple Solid Part Imports the assembly as individual solid bodies into a single-part file If you leave this check box deselected, you can specify how surface objects will be translated:

3.  Individual Surface Bodies Imports surfaces as individual surfaces in a single-part file

4.  Single Composite Feature Imports surfaces as a single composite in a single-part file

Some CAD software outputs SAT files in a default unit without regard for the units used to create the original file. You can specify the units to which the imported geometry will be converted as well as the postprocess options listed here.

1.  Check Parts During Load This option performs a quality check on the imported data. Bad data is marked with a symbol in the browser, and any remaining data is not checked. If the parts are determined not to have any errors, they are marked with a green check mark in the browser. Checking parts can significantly increase the time required to translate files.

2.  Auto Stitch This option stitches surfaces into a quilt or solid, when possible. If the stitch results in a single body, it is promoted out of the construction environment; otherwise, it remains in the construction environment.

3.  Enable Advanced Healing This option allows small alterations in the surface geometry in order to stitch the surfaces.

To export a file as SAT, click the Inventor button, choose Save Copy As, and set Save As Type to SAT Files (*.sat). Click the Options button to set the SAT version. The default is version 7.0. You can also choose to include sketches. Included sketches are translated to the SAT ungrouped.

Watch for SAT File Versions

As of Inventor release 5.3, Autodesk broke away from the ACIS SAT standard when it created its ShapeManager kernel. This means that Inventor cannot read in any SAT file that is newer than version 6.0. Keep this in mind when requesting models from third parties or when downloading them from a vendor's website.

Using Inventor File Translators

With Inventor, you can access files from other CAD systems without downloading an add-in or translating the files to an intermediate format such as STEP, IGES, or SAT. Instead, you simply open the file, and Inventor will translate the file into an Inventor file on the fly. You can translate all of the file types in the following list by clicking Open on the Get Started tab and then setting the Files Of Type drop-down to the appropriate type. Once the file type is selected, click the Option button to configure the import options.

·     CATIA V4

·     CATIA V5

·     Pro/ENGINEER

·     Unigraphics

·     Parasolids

·     SolidWorks

·     Rhino

In the Import Options dialog box, you can choose from three save options:

1.  Save In Workspace Writes the files to the Workspace folder defined in your current project file (see Chapter 1 for more on projects and workspaces). The files are saved as Inventor files during the import process.

2.  Select Save Location Allows you to specify where the resulting Inventor files will be saved. If the translated file contains separate solid bodies, you can configure the import to save those files to one location and the top-level assembly file to another location.

3.  Save At Import File Location Writes the resulting Inventor files to the same location as the original file.

The Import Into Repair Environment option checks the model for errors and creates a repair node in the browser. You can edit, diagnose, and repair imported base bodies in the repair environment.

For each of these file types, you can specify the units to which the imported geometry will be converted as well as the postprocess options listed here:

1.  Check Parts During Load This option performs a quality check on the imported data. Bad data is marked with a symbol in the browser, and any remaining data is not checked. If the parts are determined not to have any errors, they are marked with a green check mark in the browser. Checking parts can significantly increase the time required to translate files.

2.  Auto Stitch This option stitches surfaces into a quilt or solid, when possible. If the stitch results in a single body, it is promoted out of the construction environment; otherwise, it remains in the construction environment.

3.  Enable Advanced Healing This option allows small alterations in the surface geometry in order to stitch the surfaces.

CATIA Import Options

When importing CATIA (Computer-Aided Three-Dimensional Interactive Application) V4 or V5 files, you can choose between solids, surfaces, meshes, wires, and points. You can use the file mi_14a_014.CATProduct in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for these files. To open CATIA files, follow these steps:

1.  Click Open on the Get Started tab.

2.  Set the Files Of Type drop-down to CATIA V5 Files (*.CATPart; *.CATProduct).

3.  Select the CATIA file you want to open and click the Options button.

In the Entity Types To Import area, use the selection buttons to specify the inclusion of solids, surfaces, wires, and points in the import action. Use the Import Assembly As Single Part check box to turn a multi-body CATIA file into a single-part file. Then choose from one of two options:

1.  Single Composite Feature Imports the assembly as a single composite feature into a single-part file

2.  Multiple Solid Part Imports the assembly as individual solid bodies into a single-part file

If you leave the Import Assembly As Single and Import Into Repair Environment check boxes deselected, you can specify how surface objects will be translated:

1.  Individual Surface Bodies Imports surfaces as individual surfaces in a single-part file

2.  Single Composite Feature Imports surfaces as a single composite in a single-part file

Pro/ENGINEER Import Options

You can use the file mi_14a_014.asm located in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for Pro/ENGINEER files. To open models created in Pro/ENGINEER, follow these steps:

1.  Select Open from the Get Started tab.

2.  Set the Files Of Type drop-down to Pro/ENGINEER and Creo Parametric Files (*.prt*; *.asm*), or Pro/ENGINEER Granite Files (*.g), or Pro/ENGINEER Neutral Files (*.neu*).

3.  Select the Pro/ENGINEER file you want to open and click the Options button.

In the Entity Types To Import area, use the selection buttons to specify the inclusion of solids, surfaces, wires, work planes, work axes, and work points in the import action. Use the Import Assembly As Single Part check box to turn a multi-body Pro/ENGINEER file into a single-part file. Then choose from one of two options:

1.  Single Composite Feature Imports the assembly as a single composite feature into a single-part file

2.  Multiple Solid Part Imports the assembly as individual solid bodies into a single-part file

If you leave the Import Assembly As Single and Import Into Repair Environment check boxes deselected, you can specify how surface objects will be translated:

1.  Individual Surface Bodies Imports surfaces as individual surfaces contained in a single-part file

2.  Single Composite Feature Imports surfaces as a single composite in a single-part file

To import Pro/ENGINEER parts or assemblies that contain instances of family tables, the accelerator files (*.xpr or *.xas) must be saved independently of the Pro/ENGINEER part and assembly files.

When the files are opened in Inventor, they will consist of a base solid, work features, and a translation report. You can then add features to the base solid using standard Inventor part-modeling tools.

Unigraphics and Parasolids Import Options

You can access Unigraphics and Parasolids files in the same way you would Pro/ENGINEER files. You can use the file mi_14a_014.prt located in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for Pro/ENGINEER files. To do so, follow these steps:

1.  Click Open on the Get Started tab.

2.  Set the Files Of Type drop-down to Parasolid Text Files (*.x_t), Parasolid Binary Files (*.x_b), or NX Files (*.prt).

3.  Browse for the file you want to open and click the Options button.

In the Entity Types To Import area, use the selection buttons to specify the inclusion of wires, solids, surfaces, and points in the import action. Use the Import Assembly As Single Part check box to turn a multi-body Parasolid file into a single-part file. Then choose from one of two options:

1.  Single Composite Feature Imports the assembly as a single composite feature into a single-part file

2.  Multiple Solid Part Imports the assembly as individual solid bodies into a single-part file

If you leave the Import Into Repair Environment and Import Assembly As Single Part check boxes deselected, you can specify how surface objects will be translated. Here are the options:

1.  Individual Surface Bodies Imports surfaces as individual surfaces contained in a single-part file

2.  Single Composite Feature Imports surfaces as a single composite in a single-part file

SolidWorks Import Options

You can use the file mi_14a_014.SLDASM located in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for SolidWorks files. To open models created in SolidWorks, follow these steps:

1.  Click Open on the Get Started tab and set the Files Of Type drop-down to SolidWorks Files (*.prt, *.sldpart, *.asm, and *.sldasm).

2.  Select the SolidWorks file you want to open and click the Options button.

In the Entity Types To Import area, use the selection buttons to specify the inclusion of wires, solids, and surfaces in the import action. Use the Import Assembly As Single Part check box to turn a multi-body SolidWorks file into a single-part file. Then choose from one of two options:

1.  Single Composite Feature Imports the assembly as a single composite feature into a single-part file

2.  Multiple Solid Part Imports the assembly as individual solid bodies into a single-part file

You can use the Import Multiple Solid Parts As Assembly check box to turn a multi-body SolidWorks file into individual part files. When imported, the new Inventor parts will be given a name based on the name of the original files.

If you leave the Import Into Repair Environment and Import Assembly As Single Part check boxes deselected, you can specify how surface objects will be translated. Here are the options:

1.  Individual Surface Bodies Imports surfaces as individual surfaces in a single-part file

2.  Single Composite Feature Imports surfaces as a single composite in a single-part file

Rhino Import Options

You can use the file mi_14a_014.3dm located in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for Rhino files. To open models created in Rhino, follow these steps:

1.  Click Open on the Get Started tab and set the Files Of Type drop-down to Rhino (*.3dm).

2.  Select the Rhino file you want to open and click the Options button.

In the Entity Types To Import area, use the selection buttons to specify the inclusion of solids, surfaces, wires, and/or points in the import action. Use the Data Organization options to select how the file will import:

1.  Create Surfaces As Select the surface types to create during the import. You can choose from the following options:

1.  Individual Surface Bodies Imports each surface as a single surface body in the part environment

2.  Single Composite Feature Imports the surfaces as a single composite in the part environment

3.  Multiple Composite Features Imports the surfaces as multiple composites in the part

IDF Board Files

Intermediate Data Format (IDF) is the standard data exchange format for transferring printed circuit assembly (PCA) files between printed circuit board (PCB) layouts and mechanical design programs. You can access IDF board files by clicking Open on the Get Started tab and setting the Files Of Type drop-down to IDF Board Files (*.brd, *.emn, *.bdf, and *.idb).

IDF board files can be imported into Inventor as assembly or part files. When brought in as an assembly, board components are translated into individual parts contained in the new assembly. When imported as a part, the board components are translated into sketches and features. Inventor will translate IDF outlines, keepouts, group areas, drilled holes, and components.

Part files are automatically named based on the information in the existing board file. Once imported, the files can be placed into Inventor assemblies and detailed in Inventor drawings just as you would any other Inventor model. Figure 14.10 shows the IDF import options. You are presented with this dialog box automatically when you open an IDF board file.

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Figure 14.10 Importing an IDF board file

You can use the file mi_14a_014.brd located in the Chapter 14 directory of your Mastering Inventor 2015 folder to explore the import options for IDF files.

Placing Components from Other CAD Systems

So far, you have learned about importing and translating files into Inventor using the Open dialog box to convert them into Inventor files. You can also access most of these file types in the assembly environment and place them straight into your Inventor assembly file just as you would any other model.

To place a non-Inventor component into an Inventor assembly, click the Place Components icon in the Assembly panel. In the Open dialog box, select the file type of the component you intend to place or set the file type to All Files. Select the file and then click the Options button. Configure the options as required and click the OK button. Click Open to translate and place the component into the assembly.

Configuring Your System to Translate Automatically

Depending on how you work with translated files, you might want to configure your system to automatically translate other CAD formats to Inventor files when they are accessed. For instance, if you use a lot of supplier content from a website that downloads in the form of STEP files, you could set up Inventor to be the default application to open STEP files. To do so, right-click a STEP file in Windows Explorer and choose Open With and then choose Default Program. In the resulting dialog, choose Inventor or click the Browse button and browse for Inventor. Now when you double-click a STEP file, it will automatically be translated and opened as an Inventor file with the last set of options you used.

Working with Imported Data

In a perfect world, you would not need to import or export data at all. Instead, all files would exist in one perfect, universal file format. Of course, this perfect world does not exist, and you are probably required to import files created in another program from time to time. In a near-perfect world, imported data would always come in healthy and without any problems. But that is rarely the case.

Repair Tools

When importing data becomes a struggle, you can often (but not always) use tools in Inventor to fix the imported geometry. Typically, the biggest struggles come with importing surface models that did not translate well from the original CAD software. Inventor provides a Repair environment for repairing poorly translated surfaces. Once repaired, imported surfaces must be promoted to the part environment for use in parametric modeling or so they can be seen in an assembly. To access the Repair environment, you simply select the imported geometry from the browser and choose Repair Bodies. In the Repair environment, you can use the tools covered in the following sections to fix the following types of imported surface geometry issues:

·     Self-intersecting surfaces or curves

·     Intersecting faces

·     Modeling uncertainty (miscellaneous topology and geometry errors)

·     Irregular surfaces

·     Face normal direction is pointing the wrong way

·     Gaps between surfaces

·     Holes in surfaces

·     Overlapping faces

You can find further information about the Repair environment in the Inventor Help files, including helpful Show Me Video instructions.

Edit Solid Tools

Other times you might find that a model imports well but you need to make some modifications. In these cases, you can add features to the base solid by sketching on any of the desired faces and using the standard Inventor part-modeling tools. But you can also use the Edit Base Solid tools to manipulate the model quickly as well. To explore the basics of editing an imported solid body, follow these steps:

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

2.  Browse for and select the file mi_14a_003.ipt located in the Chapter 14 directory of your Mastering Inventor 2015 folder and click the Open button.

3.  Once the file is open, right-click the Base1 feature in the browser and choose Edit Solid.

This will activate the Edit Base Solid tab and display the base solid editing tools, as shown in Figure 14.11.

4.  Next use the ViewCube® to rotate the model so that you can see the circular face shown in Figure 14.11.

5.  Select the Move Face tool from the Modify tab and then click the circular face.

6.  Click and drag on the blue Z arrow in the triad and lengthen the shaft of the part by 25 mm, as shown in Figure 14.12; then right-click and choose OK.

7.  Select the Offset tool from the Modify tab and then click the cylindrical face of the shaft.

8.  Click and drag the manipulation arrow up and down to see the diameter of the shaft shrink and grow, as shown in Figure 14.13.

9.  Settle on an offset value that reduces the diameter shaft by 4 mm; then right-click and choose OK.

10.Select the Extend/Contract Body tool from the Modify tab and then select YZ Plane from the Origin folder (in the browser).

11.Ensure the Expand button is selected in the Extend or Contract Body dialog box; then enter a distance of 15 mm and click the OK button.

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Figure 14.11 Editing a base solid

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Figure 14.12 Using the Move Face tool to lengthen the part

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Figure 14.13 Using the Offset tool to change shaft diameter

Figure 14.14 shows the Extend Or Contract Body dialog box.

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Figure 14.14 Using the Extend/Contract Body tool

In these steps, you used the Edit Solid tools to modify a base solid that was originally imported from another file format. These tools can be quite useful for making small modifications to models obtained from supplier websites. You can close this file without saving changes and continue to the next section.

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Use Edit Solid to Modify Purchased Parts

Oftentimes you're able to locate a STEP file of a purchased component from a supplier website but then find that you need to make modifications to it for use in your assembly design. For instance, you might find an accurate model of an air cylinder of the correct size from a designated supplier's website. Then you realize that you need a similar model but one that is longer. You could use the Edit Solid tools to create a new longer version from the existing model.

Viewing DWF Markup

Autodesk® Design Review (ADR) software offers Inventor users and anyone they work with a simple and effective way to view and mark up both 2D and 3D DWF files. Design Web Format (DWF) files are lightweight versions of your Inventor files that you can publish from Inventor and email to a collaborator to be viewed and redlined with ADR. Non-Inventor users can download and install ADR free from the Autodesk website.

The DWF markup process begins from within Inventor where you will publish a DWF from your Inventor files. Once the DWF is published, it is sent to the reviewer and marked up with ADR. You can then bring those markups into your Inventor file and change the status of a markup, add comments, or accept the markup. You have the additional choice of publishing to DWFx format, allowing reviewers to access the file directly through Internet Explorer.

A typical DWF markup process is as follows:

1.  Publish You write out the DWF file from Inventor 2D and/or 3D files.

2.  Receive The reviewer receives the DWF file from you and opens it with ADR to check for errors and omissions.

3.  Review The reviewer can comment on and mark up the DWF file using callouts, text blocks, shapes, dimensions, stamps, and custom symbols. Then they save those markups to the DWF file.

4.  Return The reviewer then sends the markups back to you for your review.

5.  Revise You load the marked-up DWF into Inventor and revise the Inventor files as required.

6.  Republish After revising, you write out the DWF file from Inventor 2D and/or 3D files again.

Publishing a DWF or DWFx File

With the file that you intend to publish open in Inventor, click the Inventor button and select Export  Export To DWF, which opens the Publish dialog box. There are three options for publishing the DWF or DWFx:

1.  Express Publishes only the active sheet without the 3D model.

2.  Complete Publishes all sheets and all 3D models except sheets excluded from printing.

3.  Custom Chooses sheets and 3D models to publish, depending on the type of file you are publishing. Extra tabs appear in the Publish dialog box for each file type as required. Here's what's included for each file type when you are using the Custom option:

1.  Drawing Files The DWF or DWFx file includes all sheets and tables as well as the complete referenced 3D models.

2.  Assembly Files The following assembly options are available:

§  The DWF or DWFx file includes the assembly with view and positional representations as well as enabled BOM views.

§  The DWF or DWFx file includes all members and the iAssembly table with view and positional representations.

§  The DWF or DWFx file includes the assembly with view and positional representations as well as enabled BOM views, weld beads, and weld symbols.

§  When an assembly is at any LOD other than the master, only that LOD is published to the DWF or DWFx. All view and positional representations, as well as enabled BOM views, are also published.

3.  Part Files The following part options are available:

§  The DWF or DWFx file includes only the part model.

§  The DWF or DWFx file includes the folded model and flat pattern (if one exists).

§  The DWF or DWFx file includes all iPart members and the iPart table.

§  The DWF or DWFx file includes only the iPart model.

§  The DWF or DWFx file includes the model with stress/constraint indicators as well as a stress scale.

4.  Presentation Files The DWF or DWFx file includes the presentation views, animations, and assembly instructions as well as the complete assembly.

DWF or DWFx files can be published with the ability to measure, print, and enable and disable markups. They can be password protected for security also. Figure 14.15 shows the publish options for an iAssembly factory.

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Figure 14.15 DWF or DWFx publish options

Once you choose the appropriate options, click Publish to specify either the DWF or DWFx format, and specify a location to create the file. The resulting file can be opened in Design Review to create markups.

Reviewing and Marking Up DWF and DWFx Files

Once a DWF or DWFx file is open in Design Review, you can create markups in the form of callouts, text blocks, shapes, stamps, custom symbols, and measurements. Figure 14.16 shows the Markup & Measure tab.

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Figure 14.16 Markup & Measure tools

When markups are created, they are listed in the Markups palettes and organized by the sheet on which they reside. Most markups contain the following collection of properties: Status, Notes, History, Created, Creator, Label, Modified, and Sheet. Drawn markups such as lines do not have properties.

Each markup can have its own status. The status can be <None>, For Review, Question, or Done. When you click a markup in the Markups palettes, the screen will zoom to the markup at the same zoom scale at which it was created. Once markups are complete, the DWF or DWFx file can be saved. Figure 14.17 shows a view marked up in Design Review.

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Figure 14.17 Marked-up view in Design Review

Accessing DWF or DWFx Markups in Inventor

To open a markup set in Inventor, select the Get Started tab and click Open; then choose DWF Markup File from the Files Of Type drop-down and select the DWF file to bring in. The DWF markups will be overlaid onto the Inventor drawing, and the Markups browser will display the markup set in the tree view. You can then edit the status and properties of each markup by right-clicking the markup in the browser, as shown in Figure 14.18.

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Figure 14.18 Markups loaded into Inventor

To experiment with markups, you can open the file mi_14a_016.idw from the Chapter 14 directory of your Mastering Inventor 2015 folder and use the file mi_14a_016.dwfx to import the markups.

DWF in the Real World

When communicating with vendors and clients who have never used Design Review and are accustomed to receiving PDF files, I recommend you do not force DWF on them. Generally, you will have much better luck getting the uninitiated to use and eventually request DWF files if you send them both PDF and DWF files initially. Include a link to the Design Review download on the Autodesk website in your email and mention that the download is free and that the files can be viewed in 3D. This approach allows the person on the other end to make the choice at their convenience. Typically, once they have used Design Review, this is the format they will request.

Once you've reviewed all markups, you can save the markups back to the DWF or DWFx file. You can choose to republish only the sheets that are marked up or republish all sheets. You can access these commands by right-clicking the DWF or DWFx filename in the Markups browser, as shown in Figure 14.19.

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Figure 14.19 Saving and republishing markups

The Bottom Line

1.  Import and export geometry. In the design world today, you most likely need to transfer files to or from a customer or vendor from time to time. Chances are, the files will need to be translated to or from a neutral file format to be read by different CAD packages.

1.  Master It You are collaborating with another design office that does not use Inventor. You are asked which you would prefer, IGES or STEP files. Which one should you request?

2.  Use Inventor file translators. Inventor offers native file translators for CATIA, Pro/ENGINEER, SolidWorks, Unigraphics, and other CAD file types. This allows you to access these file formats with Inventor and translate the files into Inventor files directly.

1.  Master It You are a “job shop” and in the past have been required to maintain a copy of SolidWorks in addition to your copy of Inventor to work with customers who send you SolidWorks files. You would like to eliminate the cost of maintaining two software packages. What is a good strategy for doing that?

3.  Work with imported data. Using the construction environment in Inventor, you can repair poorly translated surface files. Often, a file fails to translate into a solid because of just a few translation errors in the part. Repairing or patching the surfaces and promoting the file to a solid allows you to use the file more effectively.

1.  Master It You download an IGES file from a vendor website, but when you attempt to use the component in your design, the surface data is found to have issues. How should you proceed?

4.  Work with Design Review markups. Design Review offers you and the people who collaborate with you an easy-to-use electronic markup tool that can be round-tripped from Inventor. Design Review markups can be made on both 2D and 3D files.

1.  Master It You want to use Design Review to communicate with vendors and clients to save time and resources, but you have found that others are unsure of what Design Review is and how to get it. What are some good ways to help others begin to use this handy application?