I am unable to create a rib using the sketch (shown in the image file). I understand the reason, but unable to create the rib. Any help is welcome
Welcome to SolidWorks forums Iyer.
You can create the complete closed sketch and then use extrude to create the rib.
You might also find this post helpful for your future reference
Thanks for the reply. I should have mentioned that the base is cylindrical as well. I have tried the closed sketch extrusion, but did not work. Because of the fillet at the top, when using rib feature, the outside of the constructed line are outside the model not intersecting. This caused the error. I can cheat the bottom by first having a square base and the cut after the rib was constructed to form the cylinder. It is the top fillet that is giving me trouble.
I am attaching a diagram showing what is intended.
catch the solution
Thanks for the post. However, as you can see that the rib is tnagential only at the sletch line and protruding out evrywhere else. What I wanted is that it is tangential to the fillet. That is why in my sketch, I showed it as flared, otherwise it cannot be tanget.
Without a transition, I don't think it is possible
At the base the rib profile is flat and at the top it has to blend with the radius. So in between there should be profile transition to match perfect.
The other option is to keep the outer edges to blend with the cylidrical radius and keep the middle of the rib bit lower than tangential line.
Would something like this work for you?
Thanks for your solution. Your solution is the one that satisfies the design intent. Eventhough, it would be difficult for any novice to know the method you have suggested.
I haven't actually tried this, but how about building the rib the way Deepak suggested, then putting a plane perpendicular to the end of your sketch line and adding a sketch on that plane. Now use the Intersection Curve command on the fillet face of the cylinder. Extrude a cut to shave the top of the rib down to match the fillet. Now cut your base to a cylindrical shape.
I have same problem..as shown i want to create rib between two circular surface.
It fails. same is easily created in PTC Creo and also follow the curved profile for rib thickness which not in SW. when i try to draw line just little below for both sides it works. But this is not i want.
The perfect way of making this rib as shown in the drawing needs an extra step with a revolved cut.
Make the rib sketch more than the bose dia and then pattern.
Make a new sketch with correct dimension and then revolve cut the ribs (both top and bottom edges follows the curve)
Hope this helps!
Thank you for quick response...
well i agree with Matt Lombard that rib feature need to be improve especially while creating them between curved surfaces.
It is easy to do the same in PTC Creo. As You can see.
Thanks Tom..you way little ok but is not what i want.
Hope that SW will improve in this area
What you're asking for can't be done with the rib feature in a single feature. When the line is tangential at the top, the width of the rib falls off the part because the top part is round. So you'd have to offset the sketch from the edges as shown in the 3rd picture. Then use the Move Face feature to move it where you want it. Ugly? Yes, but this is a definite limitation of the Rib feature.
The last picture shows an exaggerated rib thickness to show how this would work in the end. The Rib feature cannot do this on its own.
File attached in sw2012 format for reference.
Jignesh, will this way work for your part?
There is a better solution to this. Use loft to create it. Simple and sweet.
Jehan Kothari wrote: There is a better solution to this. Use loft to create it. Simple and sweet.
Jehan Kothari wrote:
But it consumes more resources
Not in my solidworks
I mean the control we get using loft would be better since there are very less feature to handle. The only thing is to handle the way split line is created. If you want to extend you might need to place sketch accordingly Surface cut acts weird sometimes but as you see adding any surface feature consumes the time. We can delete that body but still feature becomes larger! Finally it goes what user feels safe to move ahead May be I could be wrong somewhere since I don't deal with such parts regularly!
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