As an occasional user of catia, I am faced with a problem that I cannot solve despite the many avenues explored.
I'd like to make a 3mm rib that follows the sketch on the attached image.
I've already tried a rib of course, either it crashes or it makes a rib that doesn't follow the surface at all, I also tried in the Generative shape design workshop to create a surface by cutting with my projection and to come back to part design to put a shell, an extra thickness, but without result.
Thank you for your advice, but as already said in my message, it doesn't work:
In image 1 when selecting the bottom surface, the rib stops at the edge of the surface, and in image 2 I selected the next surface and the result is even worse, and it gets even worse if I select the 3rd surface where the guide curve passes.
Hello, the result is normal since as indicated by the reference surface option, the surface must cover the path, if you observe carefully, you will see that I did an extraction with continuity in tangency to have a continuous surface under the whole path (the projection).
After you work in hybrid mode, hence the greater rigidity of CATIA in the construction chronology of the GSD elements, the extraction of the reference surface must be created before the sweep curve and the rib profile.
I'm in V5-6R2017 if you the equivalent or SUP I can attach my file.
The ref surface must cover the entire guide curve, in your case you selected with the mouse the surface of the solid so CATIA does not take the continuity , it just selects the Tile "Extrusion.1\face.18" or for image 2 "Extrusion.1\face.7".
You have to go to the surface workshop to do an extraction with tangent continuity to have the complete surface (be careful to have the active work object before your guide curve and your profile).
In the command for ref surface you select The extraction you just did (In the graph) not in the graphics window.
EDIT:
A screenshot of the extraction function, I'm in normal mode, so in my case the surface elements are under a geometric set, and since it's not ordered, the order of creation doesn't matter.
I tried the extraction function, but if I do like you by selecting the bottom face as an element to extract, only this face becomes green, and my problem remains the same
If I select the next face, here it is:
The bottom face is not selected with it, why does it show "tangency discontinuity"?
yet the sketch of my basic extrusion is isoconstrained
You have a PB of tangency CATIA indicates it to you by the panel on ! and tells you the edge in question you must have the tangency symbols (two parallel lines) between the bottom segment and the two spokes.
