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
interested.

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:

www.frontiernet.net\~mlombard

Thanks!

Matt Lombard

 

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.

 

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

 

Basically, if you have an AutoCAD solid,

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~)

===================================

 

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

 

Matt,

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

 

Ah yes, the ol edit with notepad trick. That's a good tip.

Thanks,
Mike

 

Hmmm. I do have SP0.1, but didn't see a prompt. I was importing
a .SAT file. I'll try some more experiments.

Mike

 

I am trying to convert from a ACIS based cad program (Cimatron) to
soliworks.
There is a very big assembly (more than 8000 parts) which are very
well organized in the native CAD and every part and sub assembly has
it s own part number as file name.

Trying to translate it to SolidWorks is not a easy work.
I tryed several formats and no one has ended with a good result.

1- SAT:
Solidworks's memory requirements quickly grows up it crashes.
Translating the subassemblies instead of the main one is a way but
the iggest problem is that when translating from SAT the file name is
replaced by random serial number.

2- IGES:
It also takes a lot of memory but at least the file name and
assembly hierarcy is maintained.

3- STEP:
Best in memory requirements and file name and assembly hierarcy is
maintained

4- Parasolid:
Export in this format is not supported.

Even in STEP or IGES, not all the filenames were correctly preserved.
Sometimes assemblies were replaced by IGroup12.sldasm and parts by
Body23.sldprt. I don't know if the problem is from the exporting stage
or the importing translator.

Any Ideas?

 

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.

http://www.frontiernet.net/~mlombard/

 

thanks for sharing these presentations with the masses matt.
much appreciated

 

Matt,

Have you taken a look at the Gold product FormatWorks for translation,
repair and healing for SolidWorks users?

Lyle

 

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.