These tips are designed for quick reference in your everyday use of Pro/ENGINEER Wildfire 4.0.
TIP 1: Using Shrinkwrap functionality to speed up the rendering of a large assembly
The Photorender process will render all model surfaces; include surfaces on the interior of a large model that may not be visible in the finished image. Rendering these extra surfaces can needlessly add to the amount of time required for the process to complete. One way of excluding these surfaces from the Photorender calculation is by using Shrinkwrap functionality. Shrinkwrap is available with the Advanced Assembly Extension to Pro/ENGINEER Wildfire 4.0 Foundation.
1. Retrieve the assembly to be rendered into session (see Figure 1 for the bulldozer assembly). Notice all of the inner surfaces and edges (represented by the hidden lines). Unless the parts in the foreground are transparent, these internal surfaces will not be seen when the model is rendered.
2. Click File > Save a Copy, and set the Type to Shrinkwrap. Enter a new name or accept the default, then click OK. Accept all of the default options in the CREATE SHRINKWRAP dialog box and click OK.
When Pro/ENGINEER Wildfire 4.0 finishes the process, the shrinkwrap model will be saved in the working directory. Click File > Open, and select the shrinkwrap file that was just created (in this case "bulldozer_sw0001.prt"). This part that Pro/ENGINEER Wildfire 4.0 has created only contains the external surfaces of the assembly; no internal surfaces that would not be seen in the rendered model are included.
3. Pro/ENGINEER Wildfire 4.0 has kept only a third of the surfaces from the original model. This new model will consist of only surfaces. See Figure 2 for the surfaces created in the shrinkwrap part.
4. Any appearance information (except for texture mapping) assigned at the various component levels will be saved with the shrinkwrap model as well. Textures, bump maps, or decals should be applied to the shrinkwrap model directly. In this case, the PTC logo was applied to the shrinkwrap model but the colors were all applied in either the individual parts or the assembly. See Figure 3 for the final rendering of several of the shrinkwrap parts patterned together.
TIP 2: Creating geometric tolerances
In Pro/ENGINEER Wildfire 4.0 geometric tolerances can be created in Part, Assembly, and Drawing modes. To create them in Part and Assembly modes, select Insert > Annotations > Geometric Tolerance, and then from the menu manager window that opens select Specify Tol. To create them in Drawing mode, click Insert > Geometric Tolerance. In either case, the Geometric Tolerance dialog box will open as shown in Figure 1.
Once the Geometric Tolerance dialog box opens the procedure for creating a geometric tolerance is the same in Part, Assembly, and Drawing modes. The procedure is as follows:
1. Select the type of geometric tolerance to be placed. The possible types are displayed on the left hand side of the Geometric Tolerance dialog box, as shown Figure 1. In this example, the position tolerance type has been selected.
2. Select the model to create the tolerance in. The model may be selected from either the Model drop down list or by clicking Select Model... and selecting the model from the screen. In Drawing mode, the list of available models will include all the models currently used in the drawing as well as the drawing itself. For assemblies, the list of models will include the assembly as well as the components that make up the assembly. For parts, only the part can be selected as the model.
3. The next step is to assign datum references to the geometric tolerance. Clickthe Datum Refs tab from the top of the Geometric Tolerance dialog box and select the datums for the primary, secondary and tertiary references. For each reference, the material condition may also be set.
In order for datum planes or axes to be selectable for use as datum references, they must have previously been set. For example; to set a datum plane select the datum so that it highlights in red and right-click Edit > Properties. The Datum dialog box will open, select the and the On Datum radio button > Ok.
In this example, the primary datum is set as datum "A" with a maximum material condition (MMC) as shown in Figure 2. The secondary datum reference is set as a compound datum B-C with an RFS (no symbol) material condition as shown in Figure 3. For position and surface profile geometric tolerances, a Composite Tolerance can be set with or without a datum reference. Figure 4 shows the composite tolerance being set with a value of 0.005 and the primary datum (datum "A") being selected as the reference.
Clicking the Unordered check box will allow multiple datums to appear in the same portion of the feature control frame.
4. The next step is to set the tolerance value for the geometric tolerance. Click the Tol Value tab, click the Overall Tolerance check box, and type the desired value. The Material Condition for the overall tolerance can also be specified. In this example, the tolerance is set to 0.020 at MMC, as seen in Figure 5. For straightness, flatness, perpendicularity, and parallelism, a Per Unit Tolerance may be set. In this example, a Per Unit Tolerance is not applicable.
5. The next step is to set the Symbols and Modifiers and Projected Tolerance Zone, if desired. Click the Symbols tab and click the appropriate check boxes under Symbols and Modifiers. The available check boxes vary depending on the type of geometric tolerance being defined. A Projected Tolerance Zone may need to be established depending on the tolerance being set. In this example, a Projected Tolerance Zone will be placed below the geometric tolerance with no specified Zone Height, as shown in Figure 6. If a specific Zone Height is desired, click the Zone Height check box and type the desired height into the input field.
6. The reference entity should then be set under the Model Refs tab. Under Reference, select one of the available options from the Type drop down list. Once the desired reference entity type is selected (e.g., Edge, Surface, etc.), the Select Entity... option will become depressed and the reference entity can be selected from the screen.
7. New to Pro/ENGINEER Wildfire 4.0 is the Additional Text tab. This is an enhancement to the "Additional Text on right" check-box of Pro/ENGINEER Wildfire 3.0 and offers several more options. It can be used to place additional text above or to the right of the geometric tolerance, or add prefixes or suffixes to the tolerance entities. Figure 7 displays an example configuration.
8. Once the geometric tolerance is fully defined, it can be placed as desired. Under Placement, select one of the available options from the Type drop down list. The possible placement options will vary depending on the type of geometric tolerance being placed. The list of possible options is Dimension, Free Note, Leaders, Tangent Ldr, Normal Ldr, and Other Gtol. For this example, the geometric tolerance has been placed With Leader while in part mode. The Place Gtol... option will become available after selecting the placement type. Continue placing the geometric tolerance using the prompts from the message log.
Figure 8 shows the geometric tolerance created in this example.
9. After the geometric tolerance has been placed, it is still possible to make changes to the definition. Once the definition is complete, choose from any of the following options:
o Click New Gtol to accept the current geometric tolerance and begin creating a new one.
o Click Cancel to quit the creation of the current geometric tolerance and exit the dialog box.
o Click OK to accept the current geometric tolerance and exit the dialog box.
After completing the geometric tolerance using one of the previous options, it is still possible to redefine it. Select the geometric tolerance from the screen (the selection filter may need to be set to 'Annotation') and select Edit > Properties. The Geometric Tolerance dialog box will open and the geometric tolerance can be redefined as desired.
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