I don't normally use the rib feature, but I have a set of 4 ribs that are on a vendor part that are perpendicular to a cylindrical surface and connect to a curved weld cap. Solidworks doesn't seem to like it all that well!
Both endpoints are coincident to their respective surfaces and the source sketch is on a plane at the appropriate 45 degree angle. Thoughts?
your direction arrow does not appear to be pointing in a useful direction. try switching this option:
Ha! I did notice that after posting. Sadly, not that simple. Flip material side gets it pointing towards the part and I believe the arrow toggle you highlighted is selected properly as I get the yellow offset of the rib thickness in the proper directions. But...
"The resulting rib did not intersect the existing model. Please try changing the "Extrusion direction" to fix the problem."
This error exists no matter which combination of extrusion direction and flip material side is selected.
How many bodies do you have in the part? Can you post it?
1 Solid Body. Here you go.
Well, still no success yet. I'm not going to tell you what to do, but, it's the end of the day here and I'm going to enjoy my weekend (storms not withstanding). Thanks for the help! I'll check back in on Monday.
The way you have it only the center of the rib will intersect the part. If the rib has any width at all, the width will go off into space. You have to either add a little straight line at the right end of the image you show, or lower the sketch at that end so the entire rib intersects material at that end. Common mistake on round parts.
Thanks Matt. I figured it was something like that but didn't want to assume. Of course, my next thought is that makes the rib feature a tad useless in my opinion. Not much faster than any other way to create a rib and if there isn't enhanced functionality (such as automatically following a curved surface) then I'm struggling to see its benefit. I could just as easily create a fully enclosed sketch profile and extrude mid plane and accomplish the same thing.
I've seen the help files, so I know there are some usage cases that it does make things easier. It's just frustrating that a fairly simple and common rib idea has to be managed in order to work properly.
Must be grumpy today! Time to top off the coffee.
The Rib feature is great for establishing design intent in a complex part.
Take a look at the attached part. Try to vary the pitch of the pattern and see what happens. Try to make this part without using the Rib feature and see how much more complicated the modeling would be.
Thanks Alin! Indeed, that is a fine use for the rib tool. A slightly less grumpy me says I would be hard pressed to call that a "rib" in the traditional sense but your point is well taken. That would be the alternative uses that I think it works great. It just seems weird that it falls flat on a simpler support rib usage case. Maybe this qualifies for one of those 5% more to make it follow established curvatures that would make it super handy!
Jim Mongiardo wrote:
Thanks Alin! Indeed, that is a fine use for the rib tool. A slightly less grumpy me says I would be hard pressed to call that a "rib" in the traditional sense but your point is well taken. That would be the alternative uses that I think it works great. It just seems weird that it falls flat on a simpler support rib usage case. Maybe this qualifies for one of those 5% more to make it follow established curvatures that would make it super handy!
Like any tool, it is best to understand the logic the developer used. Matt's answer is bang on.
Indeed! But I'm also a HUGE proponent of the developer programming with the logic of the end user in mind. I apply the same logic to myself of course. If I design something that's elegantly modelled using existing features but is a giant headache to actually fabricate using existing tooling, then that's a fail on my part no matter how elegant it looks.
If I'm smart enough (hopefully!) to be able to add a small line segment to make the feature work on a curved surface, it's not too much of a stretch of the imagination to expect the feature to act similarly without my direct management.
The way you have it only the center of the rib will intersect the part. If the rib has any width at all, the width will go off into space. You have to either add a little straight line at the right end of the image you show, or lower the sketch at that end so the entire rib intersects material at that end. Common mistake on round parts.