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Catia V5 drafting view error
- Thread starter Azrael
- Start date
We run into this frequently. What version are you at? Up until R13, we recieved it frequently in Section View, usually with parts that contained surfaces imported from another package. The only fix we found was to move the section slightly.
At R13, the section view Red X problem went away, but we are now seeing it occasionally on Projection Views. Usually running a CATDUA on all of the parts fixes it.
Are you running with VPM? If so, another thing that may cause the Red X prolem is parts with Slashes in their Part Name (not Part Number, but Part Name). Somehow, R13 doesn't like this very well. I can't verify this yet, but it is something to look for.
At R13, the section view Red X problem went away, but we are now seeing it occasionally on Projection Views. Usually running a CATDUA on all of the parts fixes it.
Are you running with VPM? If so, another thing that may cause the Red X prolem is parts with Slashes in their Part Name (not Part Number, but Part Name). Somehow, R13 doesn't like this very well. I can't verify this yet, but it is something to look for.
We've seen it when sectioning very large assemblies and where there is one part covering everything. Also had problems sectioning a view with a complex surface model within.
I'm not sure where the problem is but probably Catia memeory management and/or Windows memory limitation.
There's three things I would try:
1. Increase memory to 2Gb
2. If using XP Pro, increase memory to 3Gb and rebuild XP for using 3Gb data segment. You'll need to rebuild Catia too.
3. Create a sectioned model of the largest model so you don't have to section it in the view. Then create the section view.
Good luck![[spin]](/data/assets/smilies/spin.gif "[spin] [spin]")
I'm not sure where the problem is but probably Catia memeory management and/or Windows memory limitation.
There's three things I would try:
1. Increase memory to 2Gb
2. If using XP Pro, increase memory to 3Gb and rebuild XP for using 3Gb data segment. You'll need to rebuild Catia too.
3. Create a sectioned model of the largest model so you don't have to section it in the view. Then create the section view.
Good luck
Hi,
I don't think memory management has nothing to do with the X. I am making some test win2000 / XP (2/4gig).
I had memory error, yes but not a single X.
Usually the X comes when 1,or more
file is corrupted. The user needs to clean the file, force update on solid. We have plenty of V4 file like that.
R14 should give a report when a view creating failed, I should make some test to see if we can find the name of the corrupted file from this report.
Eric N.
catiav5@softhome.net
I don't think memory management has nothing to do with the X. I am making some test win2000 / XP (2/4gig).
I had memory error, yes but not a single X.
Usually the X comes when 1,or more
file is corrupted. The user needs to clean the file, force update on solid. We have plenty of V4 file like that.R14 should give a report when a view creating failed, I should make some test to see if we can find the name of the corrupted file from this report.
Eric N.
catiav5@softhome.net
- Thread starter
- #6
It was an assembly containing both solid and surfaces and I´ve now isolated the problem. It was an surface from styling that gave us this problem, after analyzing it I found consistency problem (boundaries show that there should be more visible surfaces then it was). The solution for me was to disassemble the surface, it gave me the non visible surfaces and made the problem go away.
Thanks for your support
Thanks for your support
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