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Rib feature (how to merge / trim ends)

leemans69

New member
I am trying to create rib features that have trimmed ends. In other words I would like the rib to "extend to" or "up to" the surface of another rib. So far I have been unsuccessful. I have tried doing this with both ribs in the same body. I have also tried doing this with each of the ribs in a seperate .CAPart (therefore in seperate .CATParts).

I believe the correct option to make this possible is the "merge ends" check box within the rib feature dialogue window. Take a look at the screen shot image below. If you have any info please by all means let me know what you think.

BTW, I am working with V5R18

Thank You,

 

MrCATIA

Super Moderator
I was unaware of the Merge Ribs Ends option. According to the online Help, it sounds like it should handle your Rib design. But I've also been unsuccessful in getting it to work (I use R18 also)

To trim the Rib, I would make a surface at the vertical pipe and then Split the Rib with the surface. This method would create history in the tree that would be more descriptive than using the Merge Ribs Ends option.
 

MrCATIA

Super Moderator
Leemans, I think I figured it out

After reading the Help files again very carefully, the profile sketch of the rib must be inside the two ends! When the profile sketch is at the end of the rib center curve (where you would normally place it), the topological error occurs.

In my picture below, you can see the profile sketch (in red) is between the two vertical pieces (green)

rib.jpg

In your picture above, the profile sketch is in the middle, but you are trying to limit the rib to only one vertical piece. It seems like the Merge Rib Ends option requires two end limits!
 
Last edited:

rishabhjain

New member
merge ends of 2 intersecting pipes

hey mr. catia can you tell me how to merge ends of multiple ribs at a single point cause im getting a figure like this:

Leemans, I think I figured it out

After reading the Help files again very carefully, the profile sketch of the rib must be inside the two ends! When the profile sketch is at the end of the rib center curve (where you would normally place it), the topological error occurs.

In my picture below, you can see the profile sketch (in red) is between the two vertical pieces (green)

View attachment 515

In your picture above, the profile sketch is in the middle, but you are trying to limit the rib to only one vertical piece. It seems like the Merge Rib Ends option requires two end limits!
 

Attachments

MrCATIA

Super Moderator
Rishabhjain,

I don't think the Merge Ends option was intended to be used for design situations like yours. (although I think it is a great idea for a software enhancement).

To get all of the intersecting pipes to meet correctly will require some extra work to develope where the pipes intersect and split them to that end condition.

Are you doing this with the Part Design workbench? The Tubing Design product might be more applicable with specific tools to trim the ends.
 

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