Solutions Current Issues > January/February/March 2007 > BENNY & BRUCE
Email LinkIMPORT/EXPORT DUTIES
(or, How to Share Data Among Various Design Programs)
by Benny Foreman and Bruce Sumpter
Editor’s note: Our engineers here at RL Hudson & Company
use Pro/ENGINEER® solid modeling software to design parts, and we
know that many of our customers’ engineering departments also
rely on Pro/E®, which is, after all, the standard by which all other
modeling programs are judged. With that in mind, we at Solutions have
enlisted two Pro/E experts – Benny Foreman and Bruce Sumpter – to
share some design insights with our readers. Both Benny and Bruce served
as application engineers and independent consultants for PTC (the company
that developed Pro/E) prior to joining our engineering department here
at RL Hudson.
Benny Foreman graduated from the University of Oklahoma in 1995 with a Bachelor’s Degree in Mechanical Engineering. Since then, he has split his time between working as a manufacturing engineer and as an application engineer designing manufacturing software. Benny has been part of RL Hudson’s engineering team since 2003.
Bruce Sumpter earned a Master’s Degree in Mechanical Engineering from Oklahoma State University in 1985. He now has two decades of experience working with engineering and enterprise-level software solutions. Bruce joined RL Hudson’s engineering team in 2004.
Gentlemen, take it away…
Benny: Okay, this time let’s look at importing and exporting of data. Pro/E allows users to exchange data files with a host of other programs and applications. You can work with everything from graphics packages for logos to spreadsheet data for families of parts to other CAD files from programs like SolidWorks or Unigraphics (UG). For the purposes of this discussion, let’s focus on importing and exporting CAD files.
MENU OPTIONS: This is the menu to access
when you need to “heal” imported
files.
Bruce: Of course, some file formats are easier to import than others. For 3-D data, we prefer to receive STEP – Standard for the Exchange of Product Model Data – files. We also like IGES – Initial Graphics Exchange Specification – files. UG files are acceptable as well. We also receive STL – Standard Tessellation Language – files, though receiving data in this way is not preferable because the accuracy of the part is compromised as a result of being translated into a series of triangular surface patches. With STL files, we must recreate the model as a precise solid.
Benny: For the most part, the process of importing is pretty standard, regardless of whether you are working with STEP, IGES, or UG files. If you just want to review – but not work on – a file, you can just open it from within Pro/E.
Bruce: But when I know I’m going to be working on an imported file, I like to first create a new part file in Pro/E so I can use our company’s standard views and attributes as a starting point. Under the “Edit” menu, I then select “Insert Shared Data” and navigate to the file to be imported.Benny: And keep your fingers crossed that it comes in intact. Depending on the complexity of the design, don’t be surprised if one or more surfaces need to be cleaned up after importing.
Bruce: And by “cleaning up,” you’re referring to things like closing surface gaps, yes?
Benny: Exactly. For us to be able to work efficiently with the imported data, the object needs to be a CAD 3-D solid. A lot of times, we’re simply looking at a design to determine volume or part weight for quoting purposes, so if it’s not solid, we can’t easily calculate these things.
Bruce: The easiest way to see if you have surface gaps is to display the file in wireframe mode. Typically, when viewed as a wireframe, if the model shows two different colors for the part edges, there are gaps at those locations in the design.
Benny: Pre-Wildfire, yellow was the default color for gaps or open edges. Wildfire highlights these gaps in pink.
Bruce: If gaps do appear, of course they must be fixed. The easiest way to fix gaps is to use Pro/E’s built-in “Import Data Doctor” tools.
Benny: The way to get to those tools is by editing the definition of the import feature. One way to do that is by going to the Model Tree, right clicking on the “Import” feature, then select “Edit Definition” from the pop-up menu.
Bruce: Once you do that, you’ll see that the basic menu bar (typically residing along the top of the screen) now contains a heading called “Geometry.” Select that, then select “Heal Geometry” from the pull-down.
Benny: And now comes another choice: “Automatic” or “Manual.” Try automatic first.
Bruce: Unless you have a “Type A” personality, in which case choose manual.
Benny: But be careful! The clutch in manual tends to stick.
Bruce: Assuming you choose automatic healing, a menu box appears asking you to select the surfaces to be healed. I generally just select the “All Surfaces” option. Click “Done,” then another box appears. Click “Compute.” Depending on the complexity of the file, this computation will take anywhere from a few seconds to a few minutes.
Benny: Once the computation is complete, Pro/E will show you what it intends to do, giving you the chance to accept the changes or quit the function. Be sure to examine the changes closely before accepting. Pro/E may suggest changes you might not want because they would somehow alter the design in undesirable ways.
Bruce: But for the most part, this function works well. In some cases, the auto healing function will fix everything that was lacking in the data. In other cases, even after the auto healing, you’ll still see some surface gaps.
Benny: If so, you may need to shift gears, ahem, into manual mode.
Bruce: And discussion of manual mode could take a week!
Benny: Briefly, though, you follow the same steps outlined previously, but select “Manual” rather than “Automatic.” A dialogue box with several options appears. The two options to focus on are “Zip Gaps” and “Fix Tangency.” Since both are similar in process, let’s take you through the first one. Choose “Zip Gaps,” then in the next menu choose “Auto Select” and click “Zip Gaps.” After reviewing the potential change, select either “Accept” or “Reject.”
Bruce: If these tactics don’t work, consult the PTC web site!
Benny: But assuming you now have the gaps completely removed, you can then solidify the model by selecting the “Edit” menu and dropping down to “Feature Properties,” then selecting “Make Solid” from the pop-up menu. Don’t forget to select “OK”! If the part won’t solidify, it means you still have a gap lurking somewhere.
Bruce: In which case, see my previous comment!
SURFACE GAP: The difference in line colors shown
above indicates there
is a gap in the design, a sure
sign that you’ll need to do some
fix-up work
Benny: To exit the “Data Doctor” environment, select either the green checkmark to accept all changes or the red “X” to cancel all changes. Be certain you’re completely happy with the product before accepting the changes. Once accepted at this point, they cannot be undone. The only way to circumvent them would be to reimport the original data and start over.
Bruce: If all has gone well, you should now have a solid geometry that can be evaluated, such as for volume or weight, or manipulated, as with the addition of features like holes or fillets.
Benny: Once done, you’ll probably need to export the file. You start that process by going to the “File” menu and selecting “Save As,” then choosing the type of file you need, such as STEP, IGES, or STL. In all cases, you will then select the coordinate system you want to use as your origin.
Bruce: In the case of STL files, which are typically used for rapid prototyping, you will also have other specifications you can make. The one I always address is “Chord Height.” This affects the accuracy of the STL approximation of the part’s precise geometry.
Benny: I typically set the Chord Height value to 0. Doing so prompts Pro/E to set this to the smallest value possible. Select “OK” and Pro/E will create the file in whatever format you’ve chosen.
Bruce: One final recommendation…For parts with complex geometry, you may want to open the newly-created file in Pro/E to check that it doesn’t have any residual geometry issues. In most cases, all will be fine, but better safe than sorry, right?
Benny: Very good idea. Send us an e-mail if you have other insights into the importing and exporting process in Pro/E. As always, you can reach us at benny&bruce@rlhudson.com. Pro/E is a wonderful program, so make full use of its capabilities!
Pro/E® and Pro/ENGINEER® are registered trademarks of Parametric Technology Corporation (PTC).
