Join a Surface and fills

[UGMENTALCASE]

afternoon, Ive searched and searched but can't seem to find anything. I have a surface whihc has been extracted from a block, however the block had holes in it, so I've filled said holes. I now want to join all surfaces, but create one smooth surface, as I need to cut another block with the new smooth joined surface, and for it not to leave round curves where the old holes were.

thanks in advance, picture attached

 

[itsmyjob]

when you join turn on the simplify the result option

Eric N.
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[UGMENTALCASE]

Hi 'itsmyjob', yeah I've done that but still end up with the holes shown, although it's one full piece.when i cut another surface with it, you'll end up with said lines, and it's being used for programming, and would cause issues!

Cheers

 

[amitpatel87]

Simplify results seems to only work in newer releases of CATIA. prior to something like R22, it never seemed to work. Which version of CATIA and release are you using?

 

[UGMENTALCASE]

r21. This could be why then

 

[jackk]

Based on the attached picture, I think it would be easier and quicker to just create a new plane passing through sketch, and then cut the other block with this plane.

 

[UGMENTALCASE]

Hi, i would but its not a flat surface, sorry forgot to mention that originally.

 

[itsmyjob]

i have R20 and Simplify the Result works for me

Eric N.
indocti discant et ament meminisse periti ​

 

[itsmyjob]

so if your surface is not flat you should use Surface untrim function more than fill function

Eric N.
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[m1mason]

I've gotten good results from the Rough Offset tool in the past. Not sure if you have access to it under GSD.
I would create an offset (say 5mm). it takes away the shapes and edeges and then I would Rough offset it back to where it was originally.

hope that helps,

Mark

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[m1mason]

I jsut thought of something else.

extract the outer boundary and then use the Fill command. it will be identical to the original wihtout the edges shown. I tried it on a none-planar object and it worked.

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[itsmyjob]

extract the outer boundary and then use the Fill command. it will be identical to the original wihtout the edges shown. I tried it on a none-planar object and it worked.

You used a ruled surface.

I will have some reserve on your method if the surface is not ruled.

Eric N.
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[UGMENTALCASE]

Thanks for the suggestions I'll check my toolbars and see if I have these options/licenses.
cheers all

 

[m1mason]

I just tried it with an Unruled surface and it worked as well. please see attached catpart

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[IrishMariner]

Another option is to use the 'Remove Face' command (it's in the Part Design workbench) on the hole in the solid block before extracting the surface.

 

[tbuelna]

If you defined the surrounding surface as a support when creating the fills, then you should have gotten a result that was very close to the parent surface. Even if the hole edges show up as boundaries in the joined surface, as long as the fill surface boundary has tangency or curvature continuity at the adjacent surface boundary, it should not create any problems for a CNC program. It would only create a problem for a CNC program if the fill surface boundary was created with point continuity, and thus leaving a defined sharp corner transition around the fill surface. CNC programs sometimes have difficulty interpreting what path to take with surface profiles that have sharp edged, discontinuous internal features.

 

[UGMENTALCASE]

Thanks for the tips I'll hopefully try it out today. We've had varying issues with our CNC department, lines they can't pick up in DXF files, surfaces that could only be read if they were exported as stp files and igs. God knows what they were going, as I've never had, seen or heard of these problems with external programmers

 

[tbuelna]

UGMENTALCASE-

The problems you describe are not unusual. As I said, CNC software tools can be quite sensitive to surface quality. And the problem is made worse when you convert the CAD model to an .igs or .stp format, and then import that model format into the NC software format. Converting the digital data file from one format to another is not an exact process, and usually produces small errors in the data during each translation. It's these small errors in the digital data definition of the part surface boundaries that cause problems in how the NC software calculates the tool paths. For example, if the file conversions produce enough of a numerical rounding error at the digital definition of the boundary between the hole fill surface edge and the parent surface edge, when the NC software sees the gap/overlap at this interface it will not know what to do, and will record an error. Some companies I have worked at require all CAD models to pass a surface quality check process before they are released to manufacturing. I have also seen similar problems with CAD models submitted to stress analysts. PATRAN seems to be especially sensitive to any flaws in the quality of the CAD model surface.

 

[lardman363]

Extract the face, extract the outer boundary, untrim the face, split by the outer boundary.