Non connex error

[feaplastic]

Hello,

I am creating midplace surface model from my solid part for analysis purpose. when i try to join two surfaces i get non connex error. For example, flat surface (100*100 mm) is connected with another flat surface (50*50 mm) which is perpenticular to first surface.

I get this error at both edge points where both surface meets. If i remove check connexity, it works. But no connectivity during meshing between two surface mesh.

How to solve?

Thanks,

feaplastic

 

[solid7]

Non-connex is one of the few things that I have found that has never been incorrect. If it says you aren't connected, believe me, you are not.

Removing check connexity simply means that it will join the surfaces, while ignoring their condition. It does NOT mean that you will be able to use those joins for subsequent operations. You find out early, or you find out later on. (nice to have choices, right?)

Solve it by extrapolating the surfaces, and re-trimming them to one another.

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[tbuelna]

feaplastic,

The surface analysis and healing functions in CATIA V5 are very good, once you learn to use them.

What level of surfacing functionality do you have? Do you have GSD or freestyle shaper?

Are these native CATIA surfaces or are they imported from some neutral file format?

 

[feaplastic]

Thanks for your replies.

Solid7,

I believe non connex error. I tried your option extrapolate and trim. But it does not work. It works only both surface dimension matches. If i do with one small surface with big perpenticular surface, then it does not. Could you please explain me further.

tbuelna,

I am a new user. I have GSD and Shaper. But for these simple operation, should i use those modules.

Looking for your replies.

feaplastic

 

[solid7]

I believe non connex error. I tried your option extrapolate and trim. But it does not work. It works only both surface dimension matches. If i do with one small surface with big perpenticular surface, then it does not. Could you please explain me further.

When you do the trim, do you have the "automatic extrapolation" option checked? Because if you do not, you would have to have matching boundaries. (both the same length) With it checked, it will trim uneven boundary lengths.

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[Azrael]

IF solid7 suggestion doesn't work, turn up the merging distance in the join operation

 

[solid7]

Yes, although I would note that I did not previously suggest merging distance, because the surfaces were described as flat. On flat surfaces, there should not be any problems that would require manipulation of the tolerance. It would be better to get a proper diagnosis of the problem than to raise this tolerance. Keep in mind that .025mm is the maximum useable join.

If extrapolating surfaces to re-trim, make sure the surfaces extend well past the intersecting surface before attempting to trim them back.

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Catia Design|Catia Design News|Catia V5 blog

 

[feaplastic]

Hello,


When automatic extrapolation option is turned on, two times i did split operation.

1. Trim first surface with respect to second.
2. Trim second surface with respect to first one.

Earlier, i was doing only the first operation. Now, It works fine.Any way i try other options also.

Thanks for your replies. Please note that my surfaces are at an different angle, not in same plane.

feaplastic.

feaplastic

 

[solid7]

Yes, you will have to do the split twice. You can do "trim" operation, by tearing down a sub-icon from the "split", and uncheck the "trim support" options. But it will be joined when you finish. (ok, if that's what you want)

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