Course Title: Assembly Tips and Techniques in Autodesk Inventor

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1 Las Vegas, Nevada, December 3 6, 2002 Speaker Name: Neil Munro Course Title: Assembly Tips and Techniques in Autodesk Inventor Course ID: MA41-2 Course Outline: Investigate bottom-up, top-down, and middle-out design techniques using the latest version of Autodesk Inventor software. This class presents a number of practical examples on the use of layouts, master models, spreadsheets, and various flavors of adaptive design in the assembly environment. We'll also examine techniques for creating 3D routed parts in Autodesk Inventor assemblies.

2 Assembly Techniques in Autodesk Inventor Autodesk Inventor enables you to construct assemblies using a variety of techniques. Knowing what tools are available, and when to use them, can improve the intelligence, robustness, and manageability of assemblies of any size. Assembly Models An assembly consists of two or more components (parts or subassemblies) that are positioned relative to each other. In most assemblies, assembly constraints are applied between surfaces, lines, and points to position and orient the components. Autodesk Inventor s adaptive technology enables assembly constraints to modify the size and position of part features, and modify the position of subassembly components. In Autodesk Inventor 6, you can capture complex shape relationships between assembly components by projecting edges and loops from other parts in the assembly. You can also use Autodesk Inventor s derived component tool to share information between an assembly and its components, or between parts in an assembly. You can even use the derived component technique to create a valid, updateable assembly that contains no assembly constraints. An enhancement to the Promote tool in Autodesk Inventor 6 enables you to promote surfaces (non-associatively) between parts in an assembly. Promoted surfaces can be used as termination faces in the receiving part. General Assembly Strategies A number of techniques and strategies can be useful, regardless of the method used to construct an assembly. Subassembly Creation An assembly with all parts at the same level will become slow and difficult to mange as the number of components increases. Structuring the assembly in a hierarchy of subassemblies is fundamental to achieving good assembly performance. Break assemblies into logical subassemblies. This can often be defined by the actual makeup of the real world assembly. If mechanism movement is required within a subassembly, keep the subassembly near the top of the hierarchy if possible. Hierarchical parts lists can be generated in Autodesk Inventor 6, removing some of the previous challenges documenting assemblies with nested subassemblies. Consider grounding components (subassemblies and parts) that will not move after placement. You can suppress the component s assembly constraints rather than deleting them in case movement is unexpectedly required later in the design process. You can create separate subassemblies, and then place them in the parent assembly, or you can demote existing assembly components into a subassembly in the assembly environment. Note that assembly constraints between demoted components are retained, while assembly constraints between the demoted components and components outside the subassembly are lost. 2

3 Design Views Design views capture a specific view of an assembly, including component state (enabled or not), visibility, and color. Design views also capture global visibility overrides for work features, sketches and weld symbols. The current view state (camera, perspective, and so on) is also saved in the design view, including any assembly section state. A defect in Autodesk Inventor 5.3 caused some design views to affect software performance, but R6 fixes the problem. Multiple design views can be created for an assembly. You can use design views to: Create separate current work areas for multiple designers. Improve performance of large assemblies. Present information for a specific purpose. For example, you could change the color of all components up for review in a design meeting to make them easily identifiable. Project Files, Multiple Users, and File Locations If you want complete management of the modeling process, investigate the implementation of a third party EDM or PDM solution. Out of the box, Autodesk Inventor 6 has better file management tools than most MCAD products. However, it does not include key features such as vaulting, required for rigorous control and management of assemblies. In Inventor, you manage file locations through the use of a project file. A complete discussion of project files is beyond the scope of this class. However, there are some important changes to file management in Autodesk Inventor 6 that bear some investigation. Library search paths folders are now Read Only. 3

4 To edit components in a library path, create a separate project file that includes all library folders as workgroup search paths. Switch to this project file when editing is required. Although not unique to R6, library search paths are also ideal for referencing components from prior projects. Since the library name is stored as part of the reference, file name conflicts are eliminated. For example, you can have multiple parts named Widget.ipt in various library search paths. An assembly containing a version of each will not have problems with unintended component replacement. File versions Autodesk Inventor 6 no longer stores multiple versions of a model (or drawing) in the same document. You now set the number of Old Version in the project file, and on each save, the previous version is pushed onto a stack in an Old Versions folder under the folder containing the component. Semi-isolated work environment Both semi-isolated and shared work environments enable check out and check in of documents. The semiisolated environment requires one or workgroups (typically server storage locations that hold the final versions), along with a workspace (usually a local folder). On check out, files are copied to the workspace, where you can edit and save multiple times before checking back in to make changes available to the rest of the design team. Even in single-user shops, this data isolation can be a useful tool to manage design revisions. Note: These enhancements do not constitute a PDM solution. Although you can have multiple versions of an assembly, all versions will load the current version of all components. Speed Up With a Reload When you in-place edit a component, additional information is loaded from disk to enable component editing. This information is not automatically removed when you return to the assembly. Over time, this additional data can reduce the performance of the assembly. Closing and reopening the assembly (or even closing Autodesk Inventor and restarting) can improve the performance of sluggish assemblies. Other tips to improve assembly speed: Use an approved graphics card and driver. Turn off assembly constraint preview in the Place Constraint dialog box. Turn on Defer Update on the Assembly tab of the Application Options dialog box. 4

5 Bottom Up Design Bottom-up assembly design involves placing pre-defined components in an assembly, and positioning them with assembly constraints. All parts in the assembly, and within any subassemblies, are built separately, without reference to other parts in the assembly. This technique works well with well-defined components, or standard parts. This method, when combined with an appropriate subassembly levels, usually results in a stable assembly structure. Assembly Constraint Strategies If possible, build constraints using entities that are not likely to be modified or destroyed at some point in the future. The only features in a component that are absolutely guaranteed to be there (and never change) are the origin planes, axes, and center point. You can take advantage of their stability by building critical features about the origin geometry, and then using the origin geometry itself as a selection in assembly constraints. If you can t use origin geometry, try to assembly to the most stable feature possible. Mate or flush constraints between key planar faces are the least likely to cause problems. Failed assembly constraints are often the result of modifying geometry referenced by the constraint. If a face or edge is split as the result of subsequent editing, the internal ID of the face or edge can change, resulting in a Constraint was placed to geometry which is no longer available error. Use the simplest constraint strategy that meets the design requirements. Planar mates and flushes are the least likely to cause gremlins to creep into the assembly. Make use of subassemblies to reduce the number of constraints. Replacing Components Assembly constraints are also subject to loss during component replacement. Assembly constraints refer to the internal ID of the corresponding face, edge, and so on. When you replace a component with one that has no relationship to the original, the likelihood of retaining any assembly constraints is slim and none. You can increase the probability by replacing the component with one that was generated as a copy of the original component. If the incoming component has been modified such that the geometry referenced by the assembly constraints has changed, the affected constraints may fail. The best method to ensure the validity of assembly constraints during component replacement is to employ matching imates on both components. 5

6 imates imates are predefined assembly constraint halves. In Autodesk Inventor 6, imate behavior is greatly improved over previous versions. imate symbols are now off by default. The symbols for an individual component occurrence appear when the occurrence is selected. When you Alt-Drag, all matching unconsumed imates are displayed in the assembly. imates can also be inferred from existing assembly constraints. Adaptive Parts Inventor makes it easy to change a bottom-up design to an assembly with more intelligence. One or more part features can be made adaptive, enabling the feature to resize, or reposition in response to assembly constraints. The requirements for a feature to be adaptive are: If the feature s sketch geometry is to adapt, the sketch must be under defined (dimensionally or geometrically) to enable the desired change. The feature creation parameters, such as extrusion length are automatically made adaptive, even though they are defined as discreet values. You can toggle adaptivity of both sketch and parameters in the feature s Properties dialog box. The feature s adaptive property must be turned on. The part containing the feature must be toggled to adaptive within the assembly. Adaptive features and parts enable you to use assembly constraints to drive the part design. Because adaptive relationships are governed by assembly constraints, the relationship is stored in the assembly, not at the part level. In the assembly environment you can easily toggle the adaptive state of a part to fix its size, or change which part, or part feature is affected by an assembly constraint. It is good practice to turn off adaptivity (usually at the part level) once the final size or position of the affected feature has been achieved. This will increase the performance of the assembly when adding constraints, and especially when examining assembly motion. It is easy to turn it back on for further editing. 6

7 An important limitation (currently) is that a part can only be adaptive in a single assembly. In addition, only a single instance of the part can be adaptive in that assembly. All other instances of the part are driven by the adaptive instance. You can save copies of the original, and then drive the unique copies independent from the original. However, the copies have no link to the original part. Cross Part Sketch Projection In Autodesk Inventor 5 and higher, you can create an adaptive link to geometry projected into a part sketch from other parts. You can easily capture complex shape relationships between assembly components. Loops and edges projected from other parts in an assembly can now update when the underlying geometry is modified. The end result is similar to cross part associativity in other modelers, but these links maintain the simple manageability of other adaptive relationships. Be cautious when using cross part projections, they are subject to failure if the underlying geometry is modified. Complete loop projections for gaskets and mating flanges are good candidates for cross part projections. Adaptive Work Features and Sketch Planes Part level work features can also play a role in adaptive relationships between assembly components. During sketch creation and specific feature termination, Inventor can automatically create adaptive work planes in response to your selections. You can select planar faces and work planes on other assembly components as the To and From termination faces for an extrusion. You can create a sketch in the current part by selecting, and optionally dragging off, a planar surface on another part. The work plane, feature, and part are marked as adaptive, and the plane s position is controlled by an assembly constraint. You can easily modify the offset value of the created assembly constraint(s) to further adapt the size (termination) or position (sketch plane) of the feature. 7

8 Promoted Geometry In Autodesk Inventor 6, you can use the Promote tool to copy geometry from other components to an in-place activated part. You can promote individual surfaces or a surface body representation of a solid body. For example, use the Thicken/Offset tool in one part to create an offset surface. Then activate another part in the assembly and promote the offset surface into the active part. The lower (blue) part in the following figure uses the surface in a Replace Face feature. The same surface is then promoted to the upper (yellow) part and used as the termination face for an extrusion. In this release the promoted surface is not associative to the underlying geometry. If the geometry in the original part is modified, you can use the Redefine option for the promoted surface to reselect the geometry to promote. Even though this release of Inventor tries to update dependent features to use the newly promoted surface, you often need to edit downstream features to reselect the redefined promoted geometry. Template Parts You can use template parts (not iparts) as a method to generate multiple similar parts that can be adaptive in the same assembly. Use the ability to select planar faces on other assembly components as the termination faces to make features adaptive (works great with simple structural components). The content library supplied with Autodesk Inventor 6 includes a variety of standard structural steel shapes that are generated as fully editable Autodesk Inventor models. Adaptive Sub-Assemblies In addition to parts, subassemblies can also be made adaptive within a parent assembly. Again, the one adaptive occurrence rule applies to assemblies as well as parts. An adaptive subassembly enables the following: The assembly constraints within the subassembly are solved at the same level as the parent assembly. Instead of acting as a single lump, the subassembly components can be manipulated in the same manner as other first level children of the parent assembly. Under constrained subassembly components can be dragged, or be repositioned to meet assembly constraints placed between components inside and outside the subassembly. 8

9 Adaptive part features can be resized / repositioned by assembly constraints that cross the subassembly boundary. Adaptive subassemblies can be nested, but keep the hierarchy flat for best performance. Grounded components in the subassembly behave as follows: If the subassembly is not grounded, ungrounded and grounded subassembly components can be moved (dragged), while obeying all assembly constraints. If the subassembly is grounded, all grounded components in the subassembly are grounded. Again, turn off subassembly adaptivity when it is not required. Assembly Layouts You can use assembly work features, and / or a layout part(s), to define a framework for an assembly. The framework can be used to define key assembly positions or orientations. Components are then assembled to the framework. Editing the framework drives changes to the assembly components, some of which might be adaptive. This technique can also be used in creating master model or skeleton based assemblies. See the discussion later in this handout for more information on skeleton modeling. Spreadsheet Driven Assemblies You can link a common spreadsheet to an assembly and to any or all components in the assembly to provide a single edit-point for the assembly. Sketch dimensions and feature parameters of individual parts can be linked to spreadsheet values. Assembly constraint values and component pattern parameters from the assembly can be linked to the same spreadsheet. This can become unwieldy with large assemblies, but can be useful for complex systems, or assemblies that fit well with table driven results of calculations. This technique can be used to control some or all aspects of the design. In addition, you can combine it with adaptive features and parts, layouts, or other assembly methods. LAYOUT 9

10 Skeleton or Master Model Layout parts can also be used to define feature sketches for any or all parts in an assembly. Sketches, work features, surfaces and solid bodies from the master model can be derived into each part. This geometry can then be used to create features in the part. Subassemblies, parts, and multiple features within a part can be derived from the same master model. This technique can be used to reduce or even eliminate the need for assembly constraints in static models. If you reference the same plane during in-place component creation, the components will be positioned as defined in the master model. You can then ground the components to retain their position as defined in the master model, without the need for assembly constraints. Any change made to the underlying geometry (master model) will be reflected in the derived components. The result can be a very stable, easy to modify assembly. Tip: This is an extremely versatile and robust assembly modeling technique Highly Recommended. This workflow can also help in dynamic assemblies where assembly constraints are difficult to apply or the required geometry for an assembly constraint is not available. You can derive information from a skeleton or master part at any point in the modeling process, and you can derive information from multiple parts (separate derive operations). MODEL COURTESY OF KENT KELLER, STROBE DATA INC. 10

11 Weldments and Assembly Features The big news in R6 assemblies is the new weldment environment. Just as a sheet-metal part is a special part type, a weldment adds functionality beyond a standard assembly. You can now create a weldment assembly from scratch using a weldment template, or you can convert a standard assembly into a weldment. However, you cannot change a weldment assembly back to a standard assembly. The weldment environment presents three weld groups in the browser, Preparations, Welds, and Machining. These groups capture the typical processes required to create a real weldment The weld groups hold time-dependent features. You can add weld preparations such as chamfers in the Preparations group, weld beads in the Welds group, and post-machining features such as holes and cuts in the Machining group. If you later activate the Preparations group, the welds and post-weld machining features are not available. You can represent a wide variety of weld beads with a cosmetic edge treatment (see the left image in the following figure). Optionally, you can represent a simple fillet weld as a 3D solid feature (see the right image in the following figure). Weld symbols display in the model, but you can easily control their visibility. Use cosmetic weld beads wherever possible. Although the use of 3D fillet welds is currently limited to fairly simple weld paths, these welds are particularly useful when you require a 3D weld bead for interference analysis or mass property calculations. Autodesk Inventor 6 now supports assembly-level features, which is necessary for the new weldment environment. An assembly feature affects component occurrences in the assembly. It does not modify the geometry in the component. Features added in the weldment Preparations and Machining groups are examples of assembly-level features. You can add assembly features to any assembly, not just weldments. Assembly features are limited to extrude cuts, holes, and chamfers in this release. In addition, you can edit an assembly feature and then add and remove components affected by the feature. 11

12 API A great deal more of the inner workings of Autodesk Inventor have been exposed in the latest release. The assembly environment is almost fully exposed in the current API. If there is something that is not currently available, your can probably write a VBA macro, or an Add-In using VB or C++ to meet your needs. A couple of examples of assembly related macros that I have written are: Assembly COG + Tracks the center of gravity of an assembly. You can add a target marker to the assembly to enable dynamic tracking of a point in the assembly relative to the assembly COG. Animator for Autodesk Inventor (Co-author with Sean Dotson, Create sequence-based animations in an assembly using a list of assembly constraint drives. Multiple constraints can be driven at the same time, and you can save and restore sequence information between sessions. 12

13 3D Routing Routing of pipe and tubing systems can be accomplished using Inventor s 3D sketches. Although a bit intimidating to begin with, you can create complex, 3D sweeps that adapt to match changes in the referenced geometry. New in R6 are part-level grounded work points that are independent of any geometry. A 3D triad tool enables you to quickly and accurately place and edit grounded work points. In addition, you can now create a 3D curve at the intersection of two surfaces. This technique can be used to create spline-based paths that remain associative to the underlying geometry. Plan ahead when creating 3D sketches. One method is to create all work points within the 3D sketch. Using in-line work features, browser clutter can be kept to a minimum. In many instances, the 3D sketch can be described as a series of connected 2D sketches. Consider the following when planning and creating 3D sketches: If there are more than two or three direction changes on a single plane, consider creating a 2D sketch (perhaps on an adaptive work plane), and then include the sketch geometry as part of the 3D sketch. You can position the 2D geometry relative to other parts in the assembly by making the sketch adaptive, and then adding assembly constraints between the sketch geometry and existing geometry. If a number of work points reference common geometry (an axis or plane), consider creating the work feature prior to starting the 3D sketch. Become familiar with in-line work feature creation. It is possible to nest in-line work features to any depth. You can now edit the position of endpoints of line segments created with the line tool in the 3D sketch environment. 13

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