resolving import errors

Recently I have had to import some IGES (and also tried STEP) files
from a client who uses ProE. In both formats I get a couple import
errors, and I cannot see how to resolve these, or if there is a way.

The two parts are sheet metal, and in one case, the check utility says
it has a "face-face inconsistant" condition, but the part has stitched
together properly - but remains with the error warning.

The second part is a thin sheet metal shield, and it fails to stitch,
resulting in 2 invalid faces and about 600 open surfaces in the FM.

Any ideas how to resolve these? I am also going to ask for the original
ProE files, and see if I can import those directly.

Cheers,
Daniel

 

I should also mention that I had thought that if I deleted the faces
that caused the problem, or made anther feature that absorbed the
problem area, the error warning would go away - but it does not.

Daniel

 

Here is kind of a broad outline on how to approach this:

1. Have the IGES healed by a service bureau like Capvidia or purchase
the software to do this.

2. Use the manual method.

Turn on Verification on Rebuild in Tools/Optiions/System/Performance
Run Tools/Check to verify the geometry is good or not
Run import diagnostics

Find the problem areas *
Fix the problem areas **


* Finding problem areas
a. Create a cut feature and slice the part in half
b. Find the half with the error
c. Repeat a & b till the error is located
d. Fix the problem **

** Fixing errors
There are many tools to do this.
Delete and replace faces.
Atomic Bomb of Fillets
etc.

 

If you are able to communicate with the parties sending the files, try
this...

Have the person translating from Pro/E change the tolerance type from
"relative" to "absolute". This will result in a better IGES or STEP
file.

Pro/E defaults to a tolerance scheme called "relative", where edge
tolerances are adjusted based on the average feature size of the model.
This can cause problems if the model has small features attached to
large faces. It also causes problems with creation of IGES, STEP, etc.

With "absolute" tolerance, the user must enter a value for precision
for the model generation. Typically, setting this to .0005 inch is
sufficient. It also has the effect of producing much cleaner IGES and
STEP output.

 

There is a KB article on this.

 

ha ha... good one

d is the hard one.

Yes, I have done this to one part that imported as a single imported
solid. However, if I make a cut or feature that absorbs the problem
area, the imported solid in the FM continues to show the yellow error
flag. My goal is to eliminate that too. it seems strange to me that the
flag remains after eliminating the error area.

As the for part that imported as 600 unique surfaces... too much of a
pain to deal with.

 

I am asking for my client to check that and resend the files if the
setting is not set to "absolute" or 0.005mm (slightly tighter than your
spec.)

As I said, it is only the complex sheet metal parts, and not the
complex plastic or other parts that are giving problems. Hope this
solves it. In this case it is not a crisis, and these are not critical
parts for my work, but I prefer to have a complete and correct assembly
for my documentation.

Thanks for the tip,

Daniel

 

You could try exporting from SW and re-importing the good half. That would
get rid of your error bit. If you use Parasolid it takes no time at all.

 

Thats a good idea and will work for the one part that is a single body.
However, the 600 surfaces...well... I'll give it a try.

Cheers,
Daniel