Is it Possible to Boolean Remove STEP File From Part?

[creilly]

Hi,
I have been sent a step file and want to use the inverse of its complex surface form in my catia model in order to design some tooling. To do this I would like to be able to use the Boolean remove function. I can do this to remove a part from a second part, but when the part to be removed is a step file (or a part file generated by saving the imported step file as a CATPart) this command does not to work.

Does anyone know if it is possible to do this, or if there is another way to achieve the same thing? I don't want to have to redraw the supplied step part as a catia part as the complex surface will be challenging and very time consuming to recreate.

Catia version: V5 R21 (this could be updated to a newer version if this would solve my problem)

Carl

 

[DBezaire]

Carl

Import the step file into a CATPart. Geometry in step files can be comprised of surface, solid or wireframe. If the solid failed to translate cleanly there will be some surface data plus some untrimmed data in sorted geometric sets. Clean up the surface data and create a Join in GSD. A simple check to verify the join is a closed shell is the Create Boundary command. It will fail if the Join is closed. This is a good thing and you can proceed to Part Design and use the Closed Surface command to generate a solid. It the generate boundary command creates some curves then you need to fix those areas to create a closed shell.

Alternatively, do you need the complete solid for your tooling? Could you use extracted local areas of the solid and use the Split or Sew function of Part Design to obtain your tooling requirements?


Win 7
23SP5/24SP3, 3DVIA Composer 2015

 

[creilly]

DBezaire thank you for the help. I've just tried to do this but run into some problems.

I have joined all of the surfaces and the boundary command states that it has no boundary., the problem is that the close surface command states that it is impossible. I have tried to analyse the surface using Connect Checker Analysis in Wire and Surface Design, this gives the below small gaps. Are these the issue and how do i close these up? I'm new to surface modelling in CATIA and can't work out how to do it.

Carl

 

[DBezaire]

The 0deg is just for tangency. That will not affect a closed surface. Perhaps you have duplicate surfaces. Do you have the Healing Assistant module? There is a command called Surface Connection Checker that will look for duplicates. What sort of tolerance did you use to create the Join?



Win 7
23SP5/24SP3, 3DVIA Composer 2015

 

[creilly]

Thanks, I've changed the tolerances and removed a duplicate surface and got it to work now. Thank you for your time.