Suggested Technique for Removing a Portion of a Part or Feature to Expose Internal Features in Pro/ENGINEER Wildfire 3.0
In Pro/ENGINEER Wildfire 3.0, a portion of a feature or part may be removed in a drawings local cross section to strategically expose internal features or parts. More specifically, the cutting plane(s) of the local cross section view allow the surfaces that lie in front of the planes to be "cut away" to expose the cutting planes. If the cutting planes cut through space rather than solid geometry, the surfaces immediately behind the cutting planes are exposed and the cutting planes act as if they are transparent. It is this feature that is used to create a "cutaway" view.
Follow the simple steps below to expose internal features:
Figure 1 and Figure 2 show the example of a hollow box part, 100 x 100 x 100 with a six-wall thickness, and a revolved feature formed therein. This scenario could easily be used for an assembly, where the revolved feature could be considered as a separate part assembled to the inside of the box.
In this example, the front of the box will be "cut off" to provide a section through which a breakout will be created to expose the geometry hidden behind the front of the box. (Figure 3)
In the model, part (*.prt) or assembly (*.asm), the cutting plane will first be created for the cross section by adding an offset datum plane — DTM1. (Figure 4)
From either the *.prt or *.asm menu, select Insert > Model Datum > Plane
Select Front as the reference (Figure 5)
Click Enter Value from the OFFSET menu, and enter an appropriate value in the appropriate direction of the green arrow so that the datum plane is located as shown in Figure 4
The datum plane will cut through the box only at the edges (notice the cross section depicted in Figure 4) and the area of the plane inside this cross section will act as a window to expose the revolved feature when DTM1 is parallel to the viewing plane in the drawing. (Figure 3)
Create a cross section using the VIEW MANAGER (View > View Manager) and this newly created datum plane
Name this cross section A
In the drawing, click Insert > Drawing View > General
For the 'Visible Area' select Full View and position the view accordingly (using datum plane 'Front')
For 'Sections' select: 2D cross-section
Click + to add a cross-section and select A for the cross section name
Change the section type from Full to Local
Select the center point for the breakout as the center of the revolved protrusion (Figure 6)
Sketch a spline, as shown in Figure 6, to expose the revolved protrusion. Complete the sketch of the spline. The result should be similar to Figure 7
An existing view of this model may be modified to display as this cutaway view by first re-orienting an existing view.
Select a view, click Edit > Properties and then View Type
Click on the existing view, and selecting General
Under Visible Area select Full View, followed by Sections as is done in Step 3. The view may be completed with the remainder of the procedure in Step 3
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