Solid from surfaces? and selection question 1

[JakeLiv]

Hi


I need to find a way to "solidify" surfaces.
I have a completely closed surface, made of several surfaces. It passes a healing and a joining, but I don't know how to make a proper solid from it.

another question, how do I select a chain of curves (especially tangent ones)? for instance when making a boundary for joining and so forth.

 

[Albigger]

1. heal the surfaces into one surface (volume) then go to part design and use "close surface" feature.


2. extract -> tangent continuity. Then join the extracts.

 

[JakeLiv]

thanks.

close surface doesn't work, says I need more then 1 planar surface for making it into a solid, but it's really closed since when I export it into step and read it in SW, it imports as solid.

when I extract the curves, and then join them, won't I need to select the curves manually?


TIA

Jake

 

[itsmyjob]

for the curve selection, in the JOIN, go right clic in the dialog box first curve... find some option for propagation (angular for tangency...)

About your solid. You do not need to create a VOLUME (GSO license) a JOIN is OK, check the boundaries or your join, you should not have any. Do some Connect Checker on the JOIN (with internal edge option ON).

Then in PartDesign you have the option to create solid from surface (insert / surface based feature / close volume).

If it works in SW it may be because of the accuracy. What is the result when you open this STEP in V5 ?

Eric N.
indocti discant et ament meminisse periti ​

 

[JakeLiv]

when I import it back to catia it's imported as a surface.. ehich means there is probably something wrong there, but it's within the acceptable tolerance of the STEP file.

 

[DBezaire]

Jakeliv - in tools - options - compatibility - iges set export representation to solid - shell.

Regards,
Derek

 

[begnor]

I know this is an old thread, but here's something that helps me find the open edges of a surface model I want to close:

Tools->Options->General-Display

Slide over and get to the Visualization tab. The last option with a pulldown is probably not checked on, Surfaces' Boundaries. Check that box on, use the pulldown to change the color to your choice, and the thickness option next to it as well. Use the Shading With Edges option, and it will highlight all the free edges in your surface model. All the closed edges will show black(default here). Once the colored edges are gone, Close Surface in Part Modeler will create the volume with no problem.

 

[solid7]

It should also be noted that checking surface continuity is something that requires more than just a blind trust in the tools.

The tools will always tell you what the gaps are - but it's harder with an overlap. It does not always catch overlaps, and this is a big problem for joining - because you can't catch a discontinuity if it doesn't register as a connection.

begnor - checking the edges is a very good idea. Many people won't do it, however, because it requires WORK. And, it's very challenging on large models.

Nonetheless, it's a very good idea.

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[begnor]

I have gotten used to chasing edges, from working in a couple other CAD systems, and I have reservations about letting the system decide what is best to close a gap when using the Heal command.

Overlaps are a pain, but the edge highlight will let you know that they are not connected. How one chooses to correct the overlap/gap is up to them. It is a lot of work sometimes, but luckily for me, I am dealing with small surface models that usually don't take more than a day to straighten out.

 

[slcad]

When dealing with surfaces, I always use an associative Join (so I can play with the merging tolerance) and an associative Boundary of my Join feature. Than I color the boundary in bright pink and give it a thick line so I can see it clearly. In case of a big model, a good option to see how many boundaries are left is to make a non-associative boundary of the Join feature, and the result will be "x" isolated curves (x = no. of boundaries). Right-click "Reframe on" to every curve, and you clearly see them.

 

[slcad]

Btw, Boundary command outputs overlapping areas too, not just the gaps.

 

[solid7]

Btw, Boundary command outputs overlapping areas too, not just the gaps.

Boundary is by far one of the best diagnostic tools for surface modeling in Catia V5.

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