Managing the Display of Assemblies Using Simplified Representations
Simplified representations improve regeneration, retrieval and display time, enabling you to design more efficiently. Simplified representations can be used to control which members of an assembly the system retrieves and displays, allowing you to include only the information requiring attention.
To demonstrate simplified representations, we will use the "simrep.asm" example shown in Figure 1.
In this example, it is not necessary to have the bolts displayed while working with the assembly. In larger models, having unnecessary components (RAM and swap or virtual memory) in the session can drain memory resources.
- From the top menu, select View > View Manager > Simp Rep > New, to create a simplified representation of the assembly
- Enter a name for this simplified representation
Simplified representations have a default rule assigned to each representation. This defines the default setting for all the objects in the assembly. To define the default rule:
- Highlight the desired simplified representation
- Select Properties >> from the View Manager dialog box (see Figure 2)
In Pro/ENGINEER, the default rule could either be:
Master Rep - Includes all components, unless otherwise specified
Graphics Rep - Includes all components in a graphical representation, unless otherwise specified
Geometry Rep - Includes all components in a geometrical representation, unless otherwise specified
Exclude Comp - Excludes all components, unless otherwise specified
The default representation is Master Rep and the rule is Exclude. To exclude all the bolts:
- Select Edit > Redefine from the View Manager dialog box
- Select the bolts from the Model Tree or graphics window. Each component should have 'Exclude' next to its name in the Model Tree
- Click the check mark to accept the specified changes and exit, then Close (See the results in Figure 3)
It is also possible to create rules that select components to be excluded or included:
- Set the simplified rep, click Edit > Redefine from within the View Manager
- Select the Setup Rule Actions button
- Click on the plus sign button to Add a new condition to define the reps content
- Click in the Condition cell and select New from the RMB menu (see Figure 4 and Figure 5)
- The Rule Editor dialog box will open to specify the selection criteria (see Figure 6)
Note: The default rule could also be Exclude Comp, with only the Block and Cover parts included. The default rule is based on preference and assembly size - if the assembly is very large and most of the components need not be seen, then using an exclude representation will select only the parts that should be included in the representation. This "exclusion" of parts is similar to suppressing components; i.e. the bill of materials will list only included parts in the assembly.
Excluding components in an assembly will decrease repaint time. If the assembly is later retrieved using Open Rep from the file open window, all the excluded components will not be brought into RAM memory, thereby improving retrieval time, overall performance and memory usage.
Creating simplified representations at the part level. Components can be retrieved in Part mode, or used in an assembly as either a graphics rep or a geometry rep. These two simplified representations types will provide tremendous performance increases, because only partial information about the part is retrieved into the session. Because limited information about the part is retrieved, the actions that can be performed on the parts are limited.
Graphics Rep - This is the quickest method of retrieval; Pro/ENGINEER only retrieves enough information to display the part graphically. However, the part cannot be modified or referenced, and may not show accurate detail, as the graphics representation is a facet model.
Geometry Rep - Requires slightly more time to retrieve and uses more memory than graphics representations but provides accurate geometry for the part. Hidden line removal, accurate mass properties and the Measure functionality are available for this representation. Geometry representations can also be referenced while working with assemblies. For example, a component can be assembled and mated to a geometry representation of another part.
These graphics and geometry representations can be used in assemblies while editing an assembly simplified representation.
When working on an assembly where only certain components need to be modified but all components need to be seen, you can set all unnecessary components to the graphics or geometry representation. This will optimize assembly retrieval times, and allow you to make modifications to the assembly, while all components can be seen for contextual purposes.
Looking at the cover part, Pro/ENGINEER can temporarily "suppress" all of the rounds on the cover in a simplified representation.
- Open 'cover.prt' and select View > View Manager > Simp Rep > New, to create a simplified representation of the assembly
- Enter a name for this simplified representation
After the simplified representation is named, four options are displayed in the EDIT METHOD menu (if this menu does not open automatically, highlight the rep name, then Edit > Redefine).
Attributes will open the REP ATTR menu. The default settings are Include Feat and Regenerate, which force the simplified representation to always be recreated by regenerating the master model.
Accelerate will use the accelerator file, which is an independently saved file that speeds up retrieval of the simplified representation.
Whole Model includes the entire model, making it fully associative and modifiable.
GeomSnapshot creates an independent read-only representation of the geometry; therefore, dimensions and other parametric information will not be included in the representation.
- Select Features from the EDIT METHOD menu
- With the Exclude highlighted in the FEAT INC/EXC menu, select the round to exclude it (see Figure 7)
- The "NO_ROUNDS" simplified representation will appear (see Figure 8)
Understanding part simplified representations. Part simplified representations cannot be used in drawings. If it is necessary to have drawings of parts with excluded features, utilize Family Table functionality for feature exclusion instead.
As an alternative display scheme, you can select only the surfaces of the part that are needed in the assembly. Using the Surface option from the EDIT METHOD menu allows only specified surfaces to be shown (see Figure 9).
There are two methods for utilizing part simplified representations within an assembly simplified representation. Parts simplified representations can be directly assembled into assembly simplified representations, or the simplified part can be substituted within the assembly's simplified representation. Substitutions are made by creating new representations in assembly mode or redefining an existing simplified representation:
- Highlight the simplified representation, then select Redefine from the RMB menu
- Select the Substitute tab in the Edit <simplified representation name> dialog box
- Selecting the part in the Model Tree will bring up the pre-defined simplified representations of the model selected
- Select the simplified representation "SURFACES"
- Click Accept and the Accept Changes button. Figure 10 shows the structure of the redefined simplified representation "simple"
- This substitution will cause the assembly to be displayed as seen in Figure 11
Substituting sub-assemblies. Substituting sub-assemblies in an assembly is analogous to substituting parts in an assembly as above. Simply create the simplified representation in the sub-assembly and Substitute it in a higher-level assembly's simplified representation. Members of Interchange Assemblies can also be substituted into a simplified representation.
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