Looking for info on translation problems

I'm putting together a presentation for a user group on model translation
problems and fixes, so naturally, my best resource for information is here.
Obviously the Parasolid format is preferred, but when you can't get a good
translation, what do you resort to? Do you do the Import Diagnosis, manual
surface or solid modeling, roundtrip translations, import settings,
translation services, return to the supplier for better data, etc? Do you
ever have to rebuild 3D solids from 3D wireframes? Do you ever use or find
useful FeatureWorks? What are your top 5 translation issues?
One of the things that would be useful to me is examples of poorly
translated models, stuff that comes into SW broken. I would prefer the
original translated format rather than the SW file with imported data. I
could use it in a wide range from slightly broken to massively busted.
Please don't send proprietary data, since this will be used in a
presentation for SW users, and will be posted to my website for anyone
You can post replies to this thread, or send models to
m__lombard_"AT"_frontier__net"DOT"net (remove underscores and change
obvious spam munge). Please zip the files before sending, and if you have
files over 8 Mb, contact me for FTP info (or use spanned zip files).
In return for your help by sending data, I may be able to fix your files
(no promises), and will definitely give you a copy of the final
presentation, which should have lots of tips and examples.
Previous presentations are also available at my site:
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Matt Lombard
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One thing I observed: Diagnosis and repair in SW2004 is MUCH better than in SW2003. I repaired models in SW2004 that wouldn't rrepair in SW2003.
Sometimes repair comes by brute force: deleting bad faces and creating new ones.
Sometimes translating a STEP214 file into STEP203 and back to SW converts Flat and cylindrical B-surfaces into actual planear and cylindrical surfaces.
I wrote a program that assigns random colors to all faces in a model. I originally wrotwe it just to demonstrate API principles, but it found use as a tool to examine imported bodies for missing faces.
matt wrote:
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I've been having translation problems importing ACIS solids in 2005. I sent a report to my "VAR" (TriHarder or something or other), but ended up with a pathetic reply from SolidWorks with no solution.
Basically, if you have an AutoCAD solid, let's say a 1"x1"x1" cube, it will import into SolidWorks as a 1 meter x 1 meter x 1 meter cube.
The answer I got from SolidWorks was, no problem! Just change the units back to inches after you import the file (at least that's what I interpereted from the cryptic, poorly written message).
I hope I don't have to explain to anyone here why that won't work.
Mike Wilson
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Mike J. Wilson
Mike, There might be a way to fix that by editing the *.sat. If you look at the file in a text editor; the first value on the third line is a scale factor relative millimeters, e.g.
1 = mm 10 = cm 1000 = meter 25.4 = inch (it's often 25.39999...., 25.4 is good enough) and finally -1 = unitless
Some programs allow defining the units on a unitless file when imported. Could also be that some make assumptions. Since Parasolid uses meters as the internal value (?) it could be that it is making the "meters" assumption?
Anyway you can change the value. Experiment with your 1 unit cube to verify that you can get what you want.
(Acad / MDT recently had a bug and would export at some value other than drawing units.) -------------------------------------------
SW "outsourcing" tech support, too? 8~)
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Jeff Howard
Mike, Do you use sp0.1 ? I have no problems with the above mentioned. SW2005 prompts me what units to use when importing the solid. Tested w ACAD200 and Sw 2005 Sp0.1
Bert Muijtstege
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Item 1
I will agree with Mike that mm-in or in-mm units are a big issue. Right now my work around is to use the Scale command in SolidWorks. You have to apply the Scale command 2 times because you cannot multiple 25.4 or divide by 25.4. So the first Scale factor is 10 and the second Scale factor is 2.54.
Item 2
I believe for the new user who is trying to import autocad data, there has to be a judgement call on the time it takes to import and convert 2D sketches with the 2D-3D tools and the time it takes to convert an autocad sketch to construction geometry and begin the part again in SolidWorks. I have seen autocad drawings with small gaps between line segments create problems in a SW sketch because the orginal acad file was not created properly. You can create geometry in acad that looks fine on the screen but endpoints are not connected. The Check Sketch for feature in the Sketch Tools toolbar is one of my favorite tools after importing.
Good topic.
Regards, Marie
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On imported parts, I always run the diagnostics. This is getting more robust with each release and will usually fix any bad faces and fill any gaps automatically. Let's say 80% of the time.
When it doesn't fix all of the bad faces, the first thing I do is have it delete them. Then I'll try to patch it up and knit it back together. This works more often than it doesn't-let's say 80% again.
On models with big problems-gaps that won't fill and patches that don't knit, I have a sort of dumb-ass thing that I try-and it often works . I will take the model with the gaps and/or bad faces and export an sat file -version5. This I then import to Cadkey99R1. I run the healing routine on it in there and go get lunch whle it chugs away on my old Dell 750 machine. It rarely heals it 100%, but often fixes enough bad edges & vertices that I can then import it to SW from CK and the resultant model will heal into something usable. This works about 1/2 the time that I resort to it. So if my math is right, 2% of the time, I cannot heal an imported part into something that I can work with. This is when I kick it back to my customer.
FeatureWorks does not help with bad faces or gaps. Where I use it is when I have a valid model that isn't moldable because there is no draft anywhere or I need to add angles for shut off purposes. I will run FW and ask it to just recognize fillets. FW is pretty good at this now. Then I can suppress the fillets and apply draft.
In 2005, I have used the rotate face routine a little, and have had mixed results with this.
I rarely model a solid over a wireframe. I used to do this in Cadkey and that is why I bought SW- so I wouldn't need to anymore.
Top 5 issues isn't relevent. It either will heal into something usable or it won't. I don't know enough about other platforms to guess as to what they are doing over there that results in garbage on my end.
Translation aside, I also have issues with SW models that I get. If the part designer modeled the thing with the `verification on rebuild' option unchecked, then I often get a model that won't scale for shrink. This is the first thing I check when I get a SW model. When shrinkage won't work I will do a tools, check and always find general faults on various faces. These need to be fixed before i can proceed.
Sorry to be so long-winded.
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Ah yes, the ol edit with notepad trick. That's a good tip.
Thanks, Mike
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Mike J. Wilson
Hmmm. I do have SP0.1, but didn't see a prompt. I was importing a .SAT file. I'll try some more experiments.
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Mike J. Wilson
Thanks to all who contributed to this thread. There is so much information, it's really impossible to condense it all into an hour long user group presentation. This is not a comprehensive treatment of the topic by any means, but it was more info than I could really present to a group of users in an hour or so. This actually gets a bit into functional surfacing for import repair and editing.
Anyway, if you would like to see the powerpoint and some additional supporting info which I culled from the SW Knowledge Base, it's up on my site now, on the User Groups page, Imported Data and How to Fix It.
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thanks for sharing these presentations with the masses matt. much appreciated
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No, Lyle, I haven't looked at it. And as I remember dealing with you is the reason why I don't use another product you carry. Remember that folks here don't care much for peddling sales folk posting trolls.
"Lyle and Laurel Fischer" wrote in news: snipped-for-privacy@enews2.newsguy.com:
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