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Three Ways to Make Life Easier in Pro/ENGINEER
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We get so many technical questions on Pro/ENGINEER each month, that we've devoted a whole feature story to them. Here are the answers to three of your most commonly asked questions.
Suggestions for working with relative and absolute accuracy in Pro/ENGINEER
What is accuracy? Certain types of geometry in Pro/ENGINEER - like a cube, cylinder, or cone - require little computational effort in order to determine an exact solution. Other types of geometry, such as the intersection of two blended spline surfaces, require much more complex mathematical calculations to determine a solution.
The accuracy command gives you the ability to control the quality of model geometry calculations and affects the representation of the solid geometry to allow efficient memory usage, storage, and display.
How can the above statement be approximated in a mathematical form? Below is a documented approximation representing the Pro/ENGINEER mathematical solution for describing model geometry.
A < F * (S/D)
A is the recommended relative accuracy
S is the smallest distance between entities
D is the diagonal of an imaginary box that encloses the part model and whose sides are parallel to default coordinate system axes
F is a factor based on the geometry of the part model
This equation suggests that decreasing the value of relative accuracy increases the ability of Pro/ENGINEER to measure shorter distances and finer detail in that model. The (F) factor adjusts this equation to depict more accurately how Pro/ENGINEER describes model geometry. The (F) factor is determined by the part geometry, and is always less than 10. In general, this factor should take values of three or less.
Typically, a default relative accuracy of 0.0012 allows geometry to be calculated with a reasonable amount of computation and within a reasonable amount of time.
An alternative to relative accuracy is specifying the absolute accuracy. This is roughly the equivalent of setting the value for smallest distance (S) in the equation above, regardless of model size. Absolute accuracy should only be used when working with imported features or when the absolute accuracy of two parts must be matched (such as during an assembly "Merge" operation).
When is it necessary to modify the accuracy of a model? A good answer is to use default accuracy until you a have reason not to do so. Typically, decreasing the accuracy results in both an increase in regeneration time as well as increased file size and memory usage. Generally, as more computation is required to calculate geometry, more space is required to store additional information.
But, accuracy may sometimes need to be modified to achieve the design intent. For instance, when placing a very small feature on a large part, intersecting two parts of different size, or matching accuracy of imported geometry to its destination part.
The adjustment of part accuracy has a direct effect on the display of edges in a model. In the vast majority of cases, however, there is no need to increase accuracy for this purpose. Instead, change the quality of the edge display (accessible using config.pro option edge_display_quality) in the model. This display option does not increase part size or regeneration time.
There is no effect upon the model accuracy when adjusting the relative accuracy of mass properties computations. Mass properties accuracy affects only the iterations used to determine model mass properties.
In general, it is better to save modifying accuracy as a last step after attempting other techniques for creating features, such as changing the regeneration order of the features in the part, changing the types of features on the part, or modifying features to avoid extremely detailed or tiny geometry.
Assigning different colors to Pro/ENGINEER family table instances
This tip will help you apply different colors to family table instances. Here are the steps to accomplish this simple, but useful workaround in Pro/ENGINEER.
Start by retrieving the Pro/ENGINEER model in which a family table has been previously specified. We're going to assign red, blue and yellow colors (Figure 1) to each instance of the family table.
In a separate Pro/ENGINEER window open the first instance of the model.
Select all the surfaces (pick a surface, click right-mouse button and select Solid Surfaces) in the model.
Copy and paste the surfaces in one single feature using CTRL + C and CTRL + V key operations as shown in Figure 2. It is recommended that this copied surface is the last feature in the model tree, such that it includes all features in the model.
Assign the color (Figure 3) to the copied quilt using the Appearance Editor.
Use identical steps for the remaining instances in the model. Adjust the family table content once these steps are completed. The table content should look identical to the one shown in Figure 4.
Converting previous Pro/ENGINEER Mechanica material files to Pro/ENGINEER Wildfire 3.0 format
This tip is designed to help those who added materials to the mmatl.lib file in previous releases of Pro/ENGINEER Mechanica, and now need to convert them to Pro/ENGINEER Wildfire 3.0 format. You should not have to follow these steps if you did not customize the mmatl.lib file.
The mmatl.lib file (in previous releases located in Pro/ENGINEER Mechanica installation loadpoint/architecture/lib folder) contains all the materials that you used during simulation analyses. The content of this file can be viewed when specifying material assignments as shown in Figure 5.
Pro/ENGINEER Wildfire 3.0 materials are structured in a new file format (*.mtl extension) and can be shared between Pro/ENGINEER and Mechanica. In order to use pre-Wildfire 3.0 materials you need to convert them using Pro/ENGINEER Mechanica tools.
Create (or open) a new Pro/ENGINEER part. Move the mmatl.lib file in the current working directory. Access Mechanica functionality (use > Applications > Mechanica) and > Properties > Materials in order to access Wildfire 3.0 material library (Figure 6).
Change Look In to your current working directory and select > File > Convert pre-Wildfire 3.0 library and click the OK button until all materials are converted as shown in Figure 7. Complete this operation by clicking OK.
You can move these converted files to your material directory, or create a new directory and point Pro/ENGINEER to read these material files using the config.pro pro_material_dir option.
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