I have problem when apply rib feature how it solve????????
It's currently not possible to make a rib like this as at the end of the rib on the cylinder side there will be a slight gap left which SOLIDWORKS doesn't know how to deal with so it fails in the creation. If you move the line down a little bit on the cylinder end you will see that the rib will then create.
A workaround would be to just draw the shape out in that Front (or whichever that view you're looking at is) plane and then extrude it midplane, making sure your sketch intersects the cylinder slightly.
Hope this helped,
This is interesting. I recently started back on Solidowrks (3 months ago) after not using it for 11 years. i have 15 years of Pro-E experience. in Pro-E, you can create a contour rib which will do exactly what the OP wants to do. the top edge is anchored to the edge of the cylinder so you don't end up with a weird flat/corner by extending the rib horizontally into the cylinder as proposed elsewhere in this thread.
I swore up and down before my company decided to move to SW that SW was easier to use and faster to learn and I still believe it, but I'm also learning that there actually are some things Pro-E does seem to handle better.
By no means am I advocating my solution to the OP question is the only method to develop a SW model.
But no matter the software, when a 'line' intersects the edge cylinder and is projected at a distance the geometry will develop a flat, now the line can intersect the cylinder just below the edge and generate a nice intersection.
Currently you can only add rib (using rib feature) as shown as blue line
the issues is the end point touching the cylinder when SW goes to make rib it does not know how to terminate the face to cylinder
add a line in red it will work...
Very good workaround.
I was hopeful that making the sketch line terminate in space (ie, not directly on the cylinder edge) would have been a good workaround, as you don't need your sketched line to terminate directly onto geometry for a rib to work. But I tested that out Tony Cantrell's model, and had no such luck. Looks like you've got the best solution.
Thank you for great Response
But i want create that type of topology how i can make it any idea about it ?????
Create the feature sketch simular to what Jason has sketched but don't use the "Rib" tool. Just extrude it.
Create a flat rib and remove unwanted portions.
Thank you, Steve Calvert
but i already tried using extrude at that time zero thickness error occur. means it's not possible.....
That's why you have to do a sketch similar to what Jason has shown you.
Here's a workaround
but it's not start at top of the cylinder !!!!!!
Jason Edelman provided a suitable workaround so that the rib starts at the top of the cylinder.
As Tony stated it's a workaround. So with this method you would make the round part 1/4" taller than you desire. After creating the rib you cut 1/4" off the top of the cylinder. It's not the way you desire to make it but it gives you the result you desire, that is what a workaround is. Short of that or extending the line into the round part as mentioned by Jason your only other option seems to be get different software that will do the rib the way you desire.
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