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Suggested Technique for Using Skeleton Models to Achieve Top-Down Assembly Design

As of Release 18.0, version 9709 of Pro/ENGINEER, top-down design tools are available that allow for the creation of a well-structured, logical design which provides a more concurrent working environment and minimizes the creation of unwanted external references.  These tools include advanced component creation tools, assembly skeleton models, copied geometric and datum references, and reference control and investigation utilities.
Advanced component creation tools: provide the ability to create components in the context of an assembly.  With this approach, the assembly structure can be created using empty components which do not create external references.  As a result, when parts, skeletons, and subassemblies are created within the context of an assembly, the first feature in the model will not create undesirable external references.
 


 
 

Skeleton model: a property of an assembly that defines skeletal, space claim, and other physical properties that may be used to define geometry of components.  The assembly's skeleton model is exactly what its name suggests; it is the behind-the-scenes backbone of the assembly.  Skeleton models can be used to manage the references of their respective assemblies, or to represent space claims for them.
 


 
 

Copy Geom features: provide the ability to copy geometric and datum references from any other skeleton or part onto a selected skeleton or a part which is being modified, while preserving names, colors, line styles, and other properties assigned to the original parent entities.  Each Copy Geom feature may only copy references from a single skeleton or part, but multiple occurrences of these features may be created in a model.
 


 
 

Reference control and investigation tools: provide the ability to trace and easily understand the references that are made among features in a design.  Specifically, these tools clarify the external reference relationships that exist among models in an assembly.
 


 
 

Color: Allows the user to change the default color for the newly created skeleton models through a config.pro option (skeleton_model_default_color)set to RGB color values. The colors allow the user to change the color to any user defined color.
In this example, a desk chair will be created.  Since it is early in the design stage, certain important pieces of information about the model are still undecided.  For example, the chair may have five legs or six, or perhaps the diameter of the central shaft may change.  A skeleton model will be constructed that simulates the overall shape of the model, and allows for modifications to the overall design to propagate downwards to the individual components of the assembly. 

Procedure

  1. Create a part called "start.prt", which consists of three default datum planes and a datum axis between DTM1 and DTM2. Store the file to disk by selecting File, Save.  This file will be used later on in the process when adding new components to the assembly. Create an assembly called "chair.asm", and then create two empty subassemblies, "seat.asm", and "base.asm".  These subassemblies can be created directly from the model tree by highlighting the assembly to which they will belong, in this case "chair.asm", and depressing the right mouse button.  Select Component and Create from the pulldown menu.  This will cause the Component Create dialog box to appear. Enter the name of the object, choose the Assembly radio button in the Type section, and Empty from the Creation Options section, as shown in Figure 1.


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    Figure 1

  2. Create the skeleton model for the top-level "chair.asm" assembly by selecting Component, Create, and choosing Skeleton Model.  The default name for a skeleton model is assemblyname_skel.prt Accept the default name, in this case, "chair_skel.prt". Choose Copy From Existing from the Creation Options menu.  This will allow the skeleton model to consist of a copy of another part, which in this example will be the "start.prt" that was created in step 1.  The advantages of using the Copy option instead of using FILE, Save As to make a duplicate of a start part, is that the new part inherits the start part's parameters, layers, and basic features, but will not inherit any external references to other components that the original part may have had.  If a component which has external references is selected for copying, Pro/ENGINEER will abort the process.  Using Copy From Existing will assemble the skeleton part (which now consists of three planes and an axis) by placing the model at the default origin of the parent assembly.  Create the two protrusions, shown below in Figure 2, by selecting Modify, Mod Skel, followed by Feature from the SKEL OPER menu, and then Create and Protrusion.  The first is extruded, the second revolved.  Notice that the skeleton model now contains solid geometry.  This will not cause a problem downstream, because skeleton models do not appear in BOM and mass properties calculations.  Also note that the geometry of the skeleton model appears in light blue to differentiate it from other components. 
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    Figure 2

    Figure 3 shows the skeleton model in the Model Tree. Note that the icon for skeleton models is the same as the icons for regular parts, but transparent. 
     
     

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    Figure 3

  3. The skeleton model created in step 2 is a very crude representation of what the finished chair will look like, but it occupies roughly the same space, and will serve as a reference to how the final geometry should look. The "base.asm" subassembly will consist of the central shaft, and the legs, spurs and wheels. In the top-level skeleton model, it is represented entirely by one feature, a revolved protrusion. Information about the geometry representing these areas can be copied from the top-level skeleton model, and used to define the components of the subassembly. Create a skeleton model for the "base.asm" subassembly by selecting Modify, Modify Subasm, and select "base.asm" from the Model Tree.  Then select Component, Create, and create a new skeleton part, named "base_skel.prt". Select Modify, Mod Skel and choose Feature, Create. To copy the important information from "chair_skel.prt" to "base_skel.prt", select Geometry from the FEAT CLASS menu, followed by Copy Geom. Choose Surface Refs from the COPY GEOMETRY dialog box, and select Define. Pick the five surfaces shown below in Figure 4, Done Sel and Done from the SURF SELECT menu. Then choose OK from the dialog box. This will create a copy geometry feature in the skeleton model of "base.asm" which contains surface copies of the central shaft, and the disk that represents the legs, spurs and wheels. These surfaces can now be used as a reference to build the components within the "base.asm" subassembly. If any geometry in those components reference these surfaces, it will update if the surfaces update. The surfaces will update if the top-level skeleton model changes.
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    Figure 4

  4. Retrieve the "base.asm" assembly into its own window. Select Modify, Mod Skel, select the skeleton part "base_skel.prt", and create a >radial pattern of datum curves, as shown below in Figure 5. At the endpoint of the curves, create a reference pattern of datum points, and a radial pattern of axes which pass through the datum points and are normal to the flat circular surface. This is shown in Figure 5. 
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    Figure 5

  5. Highlight "base.asm" in the Model Tree, and use the right mouse button pulldown menu to select Component, Create. In the New Object dialog box, enter the "leg" for the Name, and choose Part for the Type, and Copy From Existing from the Creation Options section.  Enter "start.prt" for the name of the part to copy.  This will bring up the start part (consisting of the three default datum planes and a datum axis) in the assembly window, and will allow it to be assembled into the "base.asm" assembly. Mate DTM3 in "start.prt" against the flat circular surface in "base_skel.prt", Align axis A_1 in "leg.prt" with axis A_2 in "base_skel.prt", and Align DTM2 in "leg.prt" with a datum created on the fly in the skeleton model. To create this datum plane, select Make Datum, and constrain it by using Through both axes A_1 and A_2 in "base_skel.prt". This will assemble "leg.prt" as shown in Figure 6, and due to the fact that a "make datum" plane was used, "leg.prt" will be able to be reference patterned to the endpoint of every curve in the skeleton model. For more information about reference patterning components, refer to Suggested Technique for Using Reference Patterns to Assemble Components. 
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    Figure 6

  6. To create features in "leg.prt", select Modify, Mod Part, and pick the part from the Model Tree, or in the graphics window. Select Feature, and Create the protrusion shown below in Figure 7. The feature was sketched on DTM3 of "leg.prt", and used DTM2 as the horizontal reference plane. While sketching the feature, the round at the tip of the part was concentric to axis A_1 in "leg.prt", and the arc at the inside of the part (which curves to match the profile of the center shaft) was concentric to the center axis of the skeleton model, "body_skel.prt", and aligned to the circular surface of the central shaft. This creates a dependency, or external reference, in the protrusion to the skeleton model, which in this case is desired because now, if the diameter of the central shaft changes, the size of the leg will update to match that size. Create the coaxial hole shown at the tip of the leg. Use axis A_1 in "leg.prt". Reference pattern the component around the base of the chair. This will place a leg at each location of a curve in the skeleton model. 
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    Figure 7

  7. Create a new part within "base.asm" from the model tree. Name the part "spur", and choose Locate Default Datums from the Creation Options dialog box, as shown below in Figure 8. 
     


     

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    Figure 8

  8. Using the Locate Default Datums option provides the ability to create a component with default datums, define its placement constraints to locate it relative to the rest of the assembly, and create some initial features without forcing external dependencies. The Creation Options dilaog box displays three options for the Locate Datums Method: Three Planes, Axis Normal To Plane, and Align Csys to Csys:
     


     
     
    Three Planes - select three orthogonal planes in the assembly. The system then creates a new part with datum planes, which it uses to place the new component with respect to the rest of the assembly.
    Axis Normal To Plane - select a single datum plane in the assembly and an axis that is normal to it. The system then creates a new part with datum planes and an axis, which it uses to place the new component with respect to the rest of the assembly.
    Align Csys to Csys - lines up the x,y, and z axes of the selected coordinate systems.
    This automatically opens the FEAT CLASS menu to allow features to be created in the new part. The features will automatically use the part default datum planes for their references, thereby avoiding the creation of external dependencies on the assembly. Once a feature is created, the system places the new part in the assembly the way that its default planes are mated (by Mate Offset with zero offsets) to the selected references in the assembly. In the case of AxisToPlane, the system also aligns the part's axis with the selected assembly axis. The offset dimensions can then be modified, or the component placement redefined, if so desired.

    Select Axis Normal To Plane, and choose the flat surface inside the coaxial hole and the axis A_1 in "leg.prt", as shown below in Figure 9. Note that this does not create external references because the system is mating and aligning the default datums and axis of this new part to the selected references, and not using them as sketching and orientation planes for the base feature in the new part. 

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    Figure 9

  9. Before creating the base protrusion in "spur.prt", select Reference Control from the Utilities pull down menu or Ref Control from the DESIGN MGR menu. In the Scope of Components to be Referenced section of the dialog box, select None, and choose Prohibit Out-Of-Scope References from the Reference Handling section. This will prevent any external references from being created. For more information on reference control, refer to Suggested Technique for Controlling the Scope of External References. 


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    Figure 10

  10. Create a cylindrical protrusion. Make the cylinder coaxial to axis A_1 in "base.prt". Since the reference control is set to None, selecting any other axis (for example, in the skeleton model or "leg.prt") will not be allowed. Reference pattern the component. This will place a spur at each location of the leg, as shown in Figure 11. 
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    Figure 11

  11. Retrieve the top-level "chair.asm" assembly.  This is shown in Figure 12.  To simplify the display, a visualization state was used to shade the legs and spurs while leaving the chair's skeleton model in hidden line and the base's skeleton model blanked.  For more information on visualization states, refer to Suggested Technique for Creating Visualization Modes. 
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    Figure 12

  12. Figure 13 shows a view of the  Global Reference Viewer.  Note that only two components have external references.  The Copy Geometry feature in the "base_skel.prt" skeleton model is dependent on the geometry of the top-level "chair_skel.prt" skeleton model because it was created by copying surfaces from one model to another, and the protrusion created in "leg.prt" is dependent on the Copy Geometry feature in the "base_skel.prt" skeleton model because an arc was aligned to it in Sketcher mode.  Notice that "leg.prt" has no external references, even though it was created within the context of an assembly.  This is a tremendous advantage, because this part can now be used in other assemblies without the worry of having this parent assembly in session. For more information on the reference viewer, refer to Suggested Technique for Using the Reference Viewer to Manage External References. 


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    Figure 13

  13. Since skeleton models were used to create this assembly, it is highly configurable, and easily modifiable.  The chair could have six legs instead of five, simply by changing the number of patterned curves in the base subassembly's skeleton model.  If a larger diameter is required for the central shaft, the protrusion in the top-level skeleton model can be modified, and the location and size of the legs will update accordingly.  For easier control of the design intent the skeleton models can be declared to a layout, and the parameters driven from there.  For more information on layouts, refer to Suggested Technique for Using Layout Dimensions to Control Assembly Design Intent.  In this example, another skeleton model could be created to drive the geometry of the seat, and additional subassemblies and skeleton models could be added to the base to create the wheels.  This technique allows for the design to be controlled from the top-level downwards, without the creation of unwanted, and often times confusing external references. 
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    Figure 14


 

 

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Laatst bijgewerkt: 23 September 2002