Using skeleton models_to_achieve_top-down_assembly_design

Using Skeleton Models to Achieve Top-Down Assembly Design
http://www.ptc.com/cs/cs_26/howto/aba986/aba986.htm[7/25/2011 5:17:55 PM]
Suggested Technique for Using Skeleton Models to Achieve Top-Down Assembly Design
Pro/ENGINEER incorporates top-down design tools 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. Part components, subassemblies, and subcomponents (components of subassemblies) can
be created to any degree required (any level of assembly) before any geometry is actually created. Once this structure is defined, the
component geometry can be defined by selecting the part or assembly from the Model Tree and clicking Edit > Activate.

Skeleton models are specialized components of an assembly that define skeletal, space claim, and other physical properties that may be used
to define geometry of components. Users can make use of skeleton models for managing external references by making all other components
(at that level of assembly; not necessarily subcomponents) reference only skeleton geometry, though this is not mandatory. Typically quilt
features and datum features are created (including curves and planes) in the skeleton part and are then used as references to act as the behind
the scenes backbone of the assembly. [Note: to help further differentiate specifically skeleton geometry from normal part geometry, the
config.pro option, "skeleton_model_default_color", can be used to configure the color of quilt features and solid geometry (if any) in the skeleton
part.]

Copy Geometry features provide the ability to copy geometric and datum references from any other component (including skeletons) into a
selected skeleton or a regular part being modified, while preserving not only the names, colors, line styles, and other properties assigned to the
original parent entities, but also the relative positions of these entities based on the assembled positions of the components. Each Copy Geom
feature may only copy references from a single skeleton or regular part, but multiple occurrences of these features may be created in a single
model. Note: Although not discussed in the context of this document, external copy geometry features can also be used for copying geometric
information.

Reference control and investigation tools, including the Global Reference Viewer 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.

In this example, a rolling desk chair will be started: the chair assembly structure will be defined in the model tree, but only portions of the base
subassembly will actually be created in this article. 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 wheels 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 an empty part called start.prt to act as the start model for the components (do not use the default template). The part will consist of
three default datum planes and a datum axis between DTM1 and DTM2. Store the file to disk by clicking File > Save. Create an empty
assembly (again, not using any templates) called chair.asm, and then create two empty subassemblies, base.asm, and seat.asm. These
subassemblies can be created by clicking . This will open the Component Create dialog box. Enter the name of the object, click the
Subassembly and Standard radio buttons in the Type and Sub-Type sections as shown in Figure 1. Next, click Empty > OK from the
Creation Method section of the "Creation Options" dialog box as shown in Figure 2.

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Figure 1
Figure 2
2. Create the skeleton model for the top-level assembly by clicking , and clicking Skeleton Model as the Type. The default name for a
skeleton model is assemblyname_skel0001.prt. Since only one skeleton model will be used in this assembly, remove the "0001" and accept the
default name, in this case, chair_skel.prt. Click Copy From Existing from the Creation Method section of the Creation Options dialog
box, and Browse to the model, start.prt, in the working directory. This will allow the skeleton model to consist of a copy of another part,
which in this example is the start.prt that was created in Step 1. The advantage of using the Copy From Existing option is that the new
part will not inherit any external references to other components that the original part may have had. The Copy From Existing pick 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 two quilts in the skeleton part, shown below in Figure 3, by selecting the skeleton part (from the screen or from the Model Tree), right-
clicking and selecting Activate. Click to create the seat and back such that the axis, A_1, is normal to the seat surface. Next, click
to create the central shaft and base revolved about the axis, A_1. Be sure to click from the dashboard to create the features as surfaces.
Note that the geometry of the skeleton model appears in light blue to differentiate it from other components.

Figure 3
Figure 4 shows the skeleton model in the Model Tree. Note that the icon for skeleton models is different from the icons for regular parts.
Figure 4
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 for how the final geometry should look. The base.asm subassembly will consist of the central shaft, 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 be used to define the components of the
subassembly. Create a skeleton model for the base.asm subassembly by activating the base.asm and clicking . Create a new, empty skeleton
part, named base_skel.prt. Next, activate base_skel.prt and click Insert > Shared Data > Copy Geometry. Click to de-activate the
Publish Geometry collector. Select all the surfaces produced by the revolved surface in the chair_skel.prt.

Next, click References from the dashboard and click in the References collector to activate the selection of datum references. Select axis,
A_1, from chair_skel.prt as shown in Figure 5. Finally, click to complete the feature. This will create a copy geometry feature in the
skeleton model of base.asm which contains surface copies of the central shaft, axis, 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 directly reference these surfaces, that geometry will update if the surfaces are modified in the top-level skeleton model. For more

information on the copy geometry feature, refer to Suggested Technique for Copying Geometric and Datum References.
Figure 5
4. With base_skel.prt still active, insert a sketched datum curve -- -- on top of the disk to represent one leg, spur, and wheel. Constrain one
endpoint to axis, A_1 and the other endpoint to the outer edge of the disk surface; make sure that there is an angular dimension for later radial
patterning (HINT: to sketch the curve, select either datum plane DTM1 or DTM2 as the Reference plane for sketching). Next, insert a datum
axis passing through the outer end/vertex of the curve and normal to the flat circular surface (these should be the only two references necessary
to create the feature). Lastly, insert a datum plane through axis, A_1, and through the axis just created. Select the datum curve, axis, and plane
just created, group them together by right-clicking and selecting Group, and rename the group "leg." Finally, pattern this group: with the group
still selected, right-click and select Pattern, select the angular dimension for the curve and enter a suitable dimension increment and number
of instances (in the example, 60 degrees was the increment with 6 instances). The assembly is shown in Figure 6 below (the datum point
display is turned off in the image).

Figure 6
5. Activate base.asm in the Model Tree, and insert a new part called leg.prt; click Copy From Existing from the Creation Method section of the
Creation Options dialog box. Again, Browse to start.prt in the working directory. 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
leg.prt against the flat circular surface in base_skel.prt, Align axis A_1 in leg.prt with the axis in the pattern leader Group LEG in
base_skel.prt, and Align DTM1 in leg.prt to the plane in the pattern leader Group LEG in base_skel.prt. This will assemble leg.prt as shown

in Figure 7 (the datum planes in base_skel.prt are blanked in the image), and later, leg.prt will be able to be reference patterned to every
Group LEG in the skeleton model. For more information about reference patterning components, refer to Suggested Technique for Using
Reference Patterns to Assemble Components.

Figure 7
6. Activate leg.prt, select and sketch the extruded protrusion shown below in Figure 8. Sketch the feature on DTM3 of leg.prt, and use
DTM2 as the Reference plane for sketching. While sketching the feature, the round at the tip of the part should be concentric to axis A_1 in
leg.prt, and the arc on the inner portion of the part (which curves to match the profile of the center shaft) should be concentric to the center
axis of the skeleton model, body_skel.prt, and should be aligned to the circular surface of the central shaft (HINT: specifically select the central
shaft surfaces from the Copy Geometry feature in body_skel.prt, not the revolved surface in chair_skel.prt). Lastly, the depth should be ,
and the bottom surface of the Copy Geometry feature in base_skel.prt (not the bottom of the revolved surface in chair_skel.prt) should be
selected. Note that this (and aligning the inner arc of the sketch to the central shaft Copy Geometry surfaces) 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. Next, create the coaxial hole shown at the tip of the leg using axis A_1 in leg.prt. Finally,
Reference pattern the component around the base of the chair. This will place a leg at each location of the Group LEG in the skeleton model.

Figure 8
7. Create a new part within base.asm called "spur", and click the Locate Default Datums and Axis Normal To Plane radio buttons from
the Creation Options dialog box, as shown below in Figure 9.

Figure 9
8. 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 initial features without forcing external dependencies. The Creation Options dialog 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 or planar surface 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.
After selecting the references, the component is automatically activated 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 Axis Normal To Plane, 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 at the bottom of the coaxial hole and the axis A_1 in leg.prt, as shown below in
Figure 10. 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.
Figure 10

9. Before creating the base protrusion in spur.prt, click Tools > Assembly Settings > Reference Control. Select None on the Objects
tab of the External Reference Control dialog box and All Forbidden References from the Selection tab. See Figures 11 and 12 below.
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.

Figure 11
Figure 12
10. Create a cylindrical protrusion in spur.prt. Sketch on DTM1 in spur.prt and make the feature coaxial to A_1 (in spur.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; therefore, simply make the
diameter of the protrusion equal to the value input for the diameter of the coaxial hole in leg.prt (since the sketched circle cannot be aligned to
the profile of the hole). Reference pattern the component. This will place a spur at each location of the leg.

11. Figure 13 shows a view of the Global Reference Viewer opened from the top-level assembly. Note that only two parts 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 the other, and the protrusion created in leg.prt is dependent on
the Copy Geometry feature in the base_skel.prt skeleton model because of the extruded protrusion's sketch and depth references. For more
information on using the Global Reference Viewer, refer to Suggested Technique for Using the Global Reference Viewer to Manage External
References.

Figure 13
12. Since skeleton models were used to create this assembly, it is highly configurable, and easily modifiable. The chair could have five legs instead
of six, simply by changing the number of patterned groups in the base subassembly's skeleton model. If a larger diameter is required for the
central shaft, the surface in the top-level skeleton model can be modified, and the location and size of the legs will update accordingly (see
Figures 14 and 15 below).

Figure 14
Figure 15
This example is designed to introduce the user to the philosophy of top-down design through the preceding tasks. This example can be further
expanded by adding another skeleton model to drive the geometry of the seat subassembly, and additional subassemblies and skeleton models
could be added to the base to create the wheels. It is extremely important to stress, however, that in the use of top-down design, as much information
as possible should be put in the top-level assembly skeleton model (from which subassemblies' skeletons should ideally copy data). Thus, if this chair
were a real-world project, one might consider creating the feature groups containing the datum curves, etc, that define the legs in the top-level
skeleton model.
This centralizes the overall assembly's information and makes the design more organized for the benefit of multiple users. Further, it is considered
good modeling practice to organize the information in the top-level skeleton model into Publish Geometry features (not discussed in this article).

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