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Hey, I'm having some problems doing a rib... I can't really understand why it doesn't let me do it, can someone hlep me?
I already tried to flip and the same error happens. and the sketch is terminating at the body, although it doens't look like it...
Look
I know Kelvin already gave you a great explanation but I was looking at other threads and found this solution
Extend the rib sketch into the circular feature. You'll still end up with the little "tag" but it will allow you to extend the rib to the circular feature with additional extrudes.
Shorten the sketch entity so that its ends float in space. a virtual extension of each end should run into the solid body. Make sure that there is just a single body to terminate the rib. Depending upon the sketch orientation, you might need to toggle the parallel to sketch or Normal to sketch options. There may also be an ambiguity with the lower end of the sketch (lower right of your pic) because it appears to exactly encounter the curved edge. Once you apply thickness to the sketched line, the curved edge will no longer terminate the rib. Try moving the lower right endpoint to the left so that the extended sketch line will see the cylindrical face rather than the edge.
I tested this. This sketch fails:
This sketch succeeds:
I tried all this ways and it still doesn't work... i don't understand
Rib feature uses the thin feature functionality. But it also extends open sketch ends until they encounter matter. It also applies a thickness. It also uses Up to Next end condition. When your sketch line is being extended, it hits the edge. So far so good. When the width is applied and the extrusion "fills" in the entire area, the portion I have outlined in red tries to extend until it is stopped by matter (up to next) but it would continue on to infinity and that's one good reason for a failure. In the above pic, I have used a simple thin feature extrude, not a rib feature to show you the difference between a simple thin extrude and a rib.
The below pic shows a typical failure mode of a rib:
You could follow my lead here and do this manually with two features: 1) a simple extrude as I did. and 2) two extruded sketched on the small remaining faces with converted edges and an up to surface end condition:
If this doesn't work for you, then we need to work with the part directly. Or submit it to your VAR in a support case.
Thx, Ben
Dumb question: Is that a solid body that the rib is going up to? Or is it a surface body?
hey. it is a solid body... I manage to do the ribs without the rib command... i draw it and did the projection in the cylinder and the did a loft... it's not perfect but it works, i tried everything and i couldn't use the rib command but thank you for trying to help
I saw some tutorials online and they don't have that box that says "selected body" and they can do it...
You have that box and it's filled out.
As can be seen in the image below, the extents of the rib width will not terminate at the circumference, thus causing a zero thickness error.
Dropping the termination point of the solid line down will allow the rib to be created.
i've done that and it still doens't work
Can you post the part for testing?
I already did the ribs as I explained in another comment... but i can still send you the part if you want
I messed around with the rib command. Changed a few things around. I tried the shapes like you have a rectangle on the left with a round extension on the right. If I move my sketch to the outer limits it fails if I move to slightly inside it works with the round extension. I made the right extension a square and move the sketch to the outer limits and it works fine. My assumption is the rib does not like the round shape when the sketch is at outer limits.
Round extension, line slightly offset to inside
Square extension sketch to outer limits and works.
That's what I was trying to show Kelvin, But you described it way better than me. Nice explanation!
Your material side arrow indicator is pointing out to space. Toggle the Flip Material Side switch so that the arrow points to the solid body.
Also, know that the extensions of your sketched entity must terminate at the body.