Autodesk Inventor Content Style Guide

By Jimmy Jackson,2014-11-29 03:33
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Autodesk Inventor Content Style Guide

Autodesk Inventor: Content Style Guide

    By Neil Munro

    Most new Autodesk Inventor? users implement the software by integrating with or replacing an existing CAD application. Most companies have an extensive base of common components and designs that are reused as is or as the foundation for subsequent designs. Regardless of the CAD system, component libraries and reuse of existing data are crucial for efficient design. This style guide discusses tools and techniques for generating and managing these common components in Autodesk Inventor software.

    Autodesk Inventor Files

    Understanding how Autodesk Inventor stores data is fundamental to managing universal and project-specific components. At the file level, each part and assembly is stored as a separate file when saved to disk. An assembly file has references to the required part and subassembly files and also contains information on the position of each component and the relationships between components. Figure 1 shows an assembly model and the assembly browser.

Figure 1: Assembly model and browser.

    Drawings are also separate documents. The software generates drawing views from referenced models. Given this individual file approach, it is important to have file management strategies in place before you begin your first project with Autodesk Inventor software. An in-depth discussion of Autodesk Inventor file management is beyond the scope of this guide, but general strategies are discussed throughout. Subassemblies Most mechanical products consist of a hierarchy of subassemblies, often nested many levels deep (see Figure 2). Common “off the shelf” components, either internal designs or from outside vendors, often constitute the majority of components in a subassembly. It is good modeling practice to create a logical structure of subassemblies to build larger assemblies. This structure typically follows the manufacturing process of the product, in which subassemblies are created and then combined to form the top-level assembly. The default behavior of a subassembly is to act as a single component in the parent assembly. Only a few assembly constraints (position and orientation relationships between components) are required to position the complete subassembly. Because you don’t need the parent assembly to evaluate the constraints between components in the subassembly, the assembly is more responsive during constraint placement. Logical subassemblies can also reduce file management issues and promote component reuse. Since common components are incorporated into most subassemblies, a well-planned strategy for creating, storing, and finding these components is key to efficient assembly design.

Figure 2: Valve subassembly.

Figure 3: Patterned fittings.

    Modeling Strategies for Standard Components

    So, what does this mean to you in the context of creating standard components? The key to generating efficient standard components is to create the simplest model that will do the job. This strategy applies not only to standard components but also to all levels of the design, from individual parts to the top-level assembly.

    Many Autodesk Inventor users actually use the word fun in the same sentence as modeling parts and assemblies. Adding features can make the model look more realistic but can significantly degrade performance (see Figure 4). For example, 300 socket head cap screws with modeled serrations on the head and 0.1 mm fillets on every edge can slow view manipulation and assembly editing.

Figure 4: Simple part version of assembly.

    The degree of detail required in a model can vary widely. Some questions you might ask to determine the level of detail required are as follows:

     What is the purpose of this component? A simple model with additional detail in a few features may be all that is required. A more detailed representation of a component may be required if clearance between moving components is an issue. Don’t add detail to areas that will never be seen or that are unimportant to the function of the component. Detailed modeling of features inside a motor or valve is rarely required and does nothing but degrade assembly performance. Parts with large feature patterns are particularly adept at slowing modeling performance to a crawl. The Autodesk Inventor graphics engine enables you to apply image-based textures complete with transparency control to parts, features, and even individual faces (see Figure 5). Replacing complex model geometry with an image can save significant resources in any component.

Figure 5: Transparent texture.

Figure 6: Decal feature.

    Images can also be accurately placed and sized in a specific part feature to represent a decal or replace geometry that would be costly to model, as shown in Figure 6.

     Is the component significant in the calculation of assembly mass, volume, or other engineering properties? If center of gravity or inertial properties are crucial, you may have to generate a detailed model. You can, however, manually override calculated mass and volume of a part or subassembly (see Figure 7). These altered values are then used for mass and volume calculations in any assembly containing occurrences of the component.

Figure 7: Mass property override.

     Is the component static or involved in assembly motion? Standard components not only are common items such as fasteners and fittings, but may also include company-specific models that are reused in many designs. These common parts or subassemblies may play a role in connecting or controlling the position of unique components in a dynamic assembly. Even if the component connects to other assembly components, add detail only as required. It’s important to accurately model interface features such as bores, flanges, threaded features, and clearance or tapped connection holes. Leave off detail in areas where it is not crucial. The model in Figure 8 has detailed end sections where it connects to other components, while the center section is represented

    simply. Eliminate all fillets and chamfers unless they are crucial to the role of the component in an assembly.

Figure 8: Model with simplified features.

     Is motion required between parts in a standard subassembly? If the standard component is logically a subassembly but does not require motion between its components, consider modeling the subassembly as a single part. You can add detail where required and change the render style (color and texture) for individual features or faces to convey the impression that the simple part represents an assembly. Although most standard components can be constructed as a part, components such as pneumatic or hydraulic cylinders (see Figure 9) require movement between subassembly parts. The default behavior of a subassembly is to act as a single component in the parent assembly. This behavior is usually desired since positioning the subassembly requires only a few assembly constraints. If motion is required between components within the subassembly, you can choose between at least two techniques. Split the subassembly into separate subassemblies or individual parts: for a cylinder, the cylinder body and associated mounting components in one subassembly or part, and the rod and its mounting hardware as a second component. The downside of this strategy is that bills of materials and parts lists are thrown into disarray. Specify that the subassembly be adaptive in the parent assembly. Generally, the assembly constraints of an adaptive subassembly are raised to the level of the parent assembly, so the subassembly components participate in motion at the top level of the assembly. However, only one occurrence of the subassembly can be adaptive in the parent assembly. Also, the motion of the subassembly components is the same in all occurrences of the subassembly.

Figure 9: Cylinder assembly.

    Model Sources and Formats

    When planning a model, ask this question first: Do I need to model this, or is it already available somewhere else? Vendors are increasingly likely to have 3D models of their products available in a file format that you can open in Autodesk Inventor. Several user websites dedicated to Autodesk Inventor software are good sources for standard components. In addition, Autodesk Inventor ships with a content library containing a wide range of parts in 19 different standards (ANSI, ISO, and so on). If you can’t find what you need, you can always build the model yourself.

    iParts The Autodesk Inventor community is a good source for models of standard components. Several websites have user-generated Autodesk Inventor models. These models may be in standard part or assembly format, but families of related parts, such as fasteners or fittings that vary in size, are often available as Autodesk Inventor iPart factories. You can also create your own iPart factories from Autodesk Inventor part documents. An iPart factory is a single part file that includes a table outlining the possible variations in the part. When you select an iPart factory for placement in an assembly, you see a series of key options that enable you to fully define which variation of the part you want to place. An iPart child matching your selections is generated (or reused if previously generated) and placed as a part occurrence in the assembly. Following is a step-by-step overview of generating an iPart factory for a dowel and then placing one of the variations (iPart child).

Figure 10: Dowel iPart.

    1. Create a model containing all features that may be included in any of the iPart children. Features that appear in some versions of the part can be suppressed in other versions. Resist the temptation to add fine details. Model only the features required for your specific circumstances (see Figure 10). 2. Rename the part parameters (sketch dimensions, extrusion lengths, and so on) that you will manipulate to create the different iPart children (see Figure 11).

Figure 11: Renamed parameters.

    3. Start the iPart Author tool. Renamed model parameters and any user parameters are automatically added as parameters that can vary between iPart children (see Figure 12). The current values of these parameters define the single version initially available.

Figure 12: iPart parameters.

    4. Add items from the other tabs as required:

     Properties: Standard and custom information associated with Autodesk Inventor documents. For example, you can add the part’s material property to the table and then vary the material of different iPart children. Suppression: Add features that can be suppressed or computed in different iPart children (see Figure 13). iMates: Add predefined assembly mating conditions for the component. See the section on iMates later in this document. Threads: Add thread information from any defined Thread Features and Tapped Holes. Other: Add additional columns such as a user-defined file name. Columns containing file name, render style, or material information must be tagged as such.

Figure 13: iPart feature suppression.

    5. Select critical parameters as keys for the iPart, as shown in Figure 14. Key values are presented during iPart placement to provide a hierarchical selection of the iPart child. In this example, the diameter and length of the dowel are the only selections required to fully define the dowel. Diameter is set as the primary key, and length as the second key. When placing the dowel in an assembly, you first select diameter, thus limiting the length selection to those iPart children matching the selected diameter.

    6. Add rows to define each iPart child. You can edit the table in Microsoft? Excel to speed up row additions and create relationships between table cells. In Figure 15, the 5/16” diameter dowels have the Chamfer2 feature suppressed. Note: Red cells indicate a value computed in Excel. The file name for each variation of this iPart is a concatenation of “Dowel_” and the values in the key columns.

Figure 15: Multiple iPart variations.

    7. Save the iPart factory to a folder specified as a library search path. See “Managing Standard Components” at the end of this document for more information on project files and search paths.

    8. To place a version of the iPart in an assembly, you select the iPart factory from the Open dialog box during component placement. A dialog box presents the iPart keys, so you can place the desired iPart child with only a few selections (see Figure 16). The software generates the selected iPart child (or reuses it if it already exists) and places an occurrence in the assembly. Each child placed in the assembly contains the iPart table, so you can replace the occurrence with another iPart child simply by selecting new keys in the table.

Figure 16: iPart placement.

    Note: The iPart factory just described is called a standard iPart since every variation of the iPart is defined in the table. You can also create custom iParts where the user defines one or more values during placement of the iPart in an assembly. Custom iParts are often used when an infinite variety of values may be required, such as the length of the iPart occurrence.

    Reusing Existing Data Some or all of your company-specific standard components may already exist in DWG or other formats. Several options are available for bringing these components into the Autodesk Inventor software application. The Autodesk Inventor DWG File Import wizard makes it easy to import 2D geometry and 3D solids from AutoCAD? drawings (see Figure 17).

Figure 17: Imported AutoCAD solid.

    You can easily import an AutoCAD solid as a base solid in Autodesk Inventor. A base solid does not contain feature information and so cannot be used as an iPart factory. If the imported solid contains unimportant details such as fillets and chamfers, you can use the base solid editing tools to permanently remove these features, as shown in Figure 18.

Figure 18: Simplified solid model.

    Drawing files with multiple 3D solids are imported as an Autodesk Inventor assembly with a separate part file generated for each 3D solid. Autodesk Inventor software cannot import AutoCAD surfaces or 3D wireframe geometry.

    A more common consideration is how to reuse existing 2D AutoCAD data. Carefully consider how the component will be used before deciding on a course of action.

     If the 2D data can be used as is for the creation of a single component, use the DWG File Import wizard to bring in the minimum amount of information required to define features in the part. You can import AutoCAD data directly into a part feature sketch and immediately create extrusions or other features from the imported sketch profiles. To keep the representation simple, do one or more of the following: Simplify the AutoCAD geometry before import. Select only the key sketch entities during the import process (Autodesk Inventor? 7 only). Simplify the sketch geometry after importing into Autodesk Inventor. If the 2D data is to form the basis of an iPart factory, it is almost always better to build the part from scratch in the Autodesk Inventor application, using the 2D AutoCAD drawing as a guide. Imported 2D data often requires considerable work to build in the design intent (geometric relationships) that is easily captured in native Autodesk Inventor feature sketches.

    In addition to native Autodesk Inventor models, you can open .sat, .stp, .iges, and Pro/ENGINEER? part and assembly models (V20 and earlier). When you open a 3D solid model saved in a nonnative format, the resulting Autodesk Inventor model is a single base feature similar to an AutoCAD solid (see Figure 19). IGES files usually contain surface information rather than solids. Autodesk Inventor software imports IGES surface files into a construction environment where you can stitch the surfaces together to form a closed boundary and then promote this to a solid model. These single-body solids are usually sufficient since the intention is to use the model as a standard component that will not be modified. When saved, imported components are stored as native Autodesk Inventor files.

Figure 19: Imported STEP model.

    Autodesk Inventor Content Library Autodesk Inventor software includes a library of standard fasteners, bearings, keys, and other mechanical parts. These components are available in a wide range of international standards, including ANSI, ISO, DIN, BSI, and JIS. The library browser is a separate pane in the assembly browser, as shown in Figure 20.

Figure 20: Content library browser.

    As with iPart factories, the software generates a selected component the first time you place it in an assembly. Standard library parts include appropriate iMates (see the iMates section of this guide for more information) attached to the geometry typically referenced when assembling the part. In addition, you can easily replace one or all occurrences of a library component with a different version. Components are placed from the library catalog using Autodesk’s i-drop? technology. Once the size parameters of the part have been specified in the library browser, you click in the component image window to fill the i-drop symbol and then drag to the Autodesk Inventor graphics window to place an occurrence in the assembly (see Figure 21).

Figure 21: i-drop of library part.

    With i-drop technology you can drag content from other servers, including web-based servers, directly into your assemblies. Tools to add to existing libraries or create your own i-drop-based content libraries are not yet available. You must create iPart factories or use other methods for components that are not included in the supplied content library.

    The content library also includes custom library parts, currently limited to common steel shapes such as channels, flanged beams, and angles. As with custom iParts, you specify the length of the custom library part during placement and provide a file name and location to store the custom part. Unlike standard library parts, custom library parts are editable and you can add features after placement (see Figure 22).

Figure 22: Custom iPart with additional features.

    Model Creation Summary So, how do you decide which method to use for standard part creation? None of the methods described is perfect, and a solution that uses all the creation tools is probably the answer for most companies. iParts are currently the most flexible solution, but generating iPart factories may require considerable work. The content library requires little setup, but the inability to add new content or edit the standard parts generated from the library may limit its usefulness for some companies. Reusing existing data and creating new non-iPart models will likely be a part of your standard component strategy, so take the time to create simple, efficient models.

iMates Standard components are typically assembled using the same geometry and constraint type. For example, a bolt is typically assembled to a hole with a single Insert assembly constraint using the circular edge under the bolt head. iMates are predefined, named assembly constraint halves that are attached to key geometry and are ideally suited for use with standard components. The iMate definition is stored with the part and can be used to assemble the part to other components using one of the following techniques:

Figure 23: Use iMate during component placement.

     When you place a component with one or more iMates in an assembly, it can be automatically assembled to matching iMates on other components (see the Use iMate check box in Figure 23). The iMate name, type, and offset values must match, and you must specify that automatic iMate matching be attempted. iMate symbols for the component are displayed when the component is selected in the assembly. You can then hold down the Alt key and drag the symbol. The iMate constraint geometry on the component is highlighted, and any matching iMates in the assembly are shown (see Figure 24). You can drag the symbol over visible iMate symbols or any geometry that satisfies the requirements for the selected iMate.

Figure 24: Press Alt and drag iMate symbols.

    You can combine individual iMates to form a composite iMate. As with single iMates, you can elect to search for matching composite iMates when placing a component, or you can press Alt and drag the symbol to connect matching composite iMates after component placement. Regardless of the methods you use to create standard parts, consider adding iMates to all your standard components. All standard parts in the content library include appropriate iMates, iParts can include iMates, and standard parts and subassemblies can also contain iMate definitions. Component Metadata All Autodesk Inventor documents include a standard set of properties called iProperties (see Figure 25). These include summary properties, project-specific information, file status information, and physical properties such as material, mass, and volume. You can also add custom text and numeric properties to any document.

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