Patterning a Feature in Part Design 2

[VN1981]

Hello,
I need to model a stiffened cylinder...basically a cylindrical shell with lots of horizontal & circumferential stiffeners. The stiffeners will be integral i.e. machined...I need to radius any exposed edges of the stiffeners.

Initially I thought, I will radius one of the stiffeners and use circular pattern to place the finished stiffener. Turns out I was wrong. Catia is not allowing me to pattern a feature. I tried selecting both the pad (upon which fillet feature was applied) & fillet but Catia gives me an impossible topological error. I kinda understand why Catia is giving me the error...But hoping the experienced users here can provide me pointers on a rapid way to pattern/copy pads along with features in Catia V5?

 

[LWolf]

Put the stiffner in a separate body, pattern the body.
Add the stiffner body to your cylindrical shell.
Create a fillet, make it as intersection, point to the boolean add.

This way you will dynamically make the fillet on the pattern, no matter how many instances of the stiffner


regards,
LWolf

 

[VN1981]

LWolf,
Thanks again for your reply. Your procedure sounds very interesting.

If I've understood it correctly:
Fillet Stiffener after adding it to the cylindrical shell? One of the fillet edges will be intersection of stiffener pad with cylindrical shell.

And sorry, how to make the fillet an "intersection"? I will look up intersection in Catia. Probably not aware of the command...

 

[LucasC]

Intersection fillet is an option within the fillet command. I think its only available in Release 25 and higher.

 

[VN1981]

LWolf,
I tried following your suggestions but I was not able to get the desired result.

I am following screenshots of what I am trying to accomplish...hopefully you can respond again with more lucid procedure for people like me.

To illustrate, lets say I have a tapered cylindrical shell and I want to insert stiffeners.

The red lines are the edges I want to fillet (highlighted in this image & the next)

The model tree on the right shows that I have created stiffener in a separate body and added it to the original body.

Please suggest on how to proceed from here. I tried choosing "intersection" in propagation but for some reason Catia is not allowing me to choose "Shaft.2" as it is already absorbed by another feature or something like that...

 

[LWolf]

so, right click on your Shaft.1 and find the command "insert in New Body"
the two rib-fillets (longitudinal 2 edges and transverse 2 edges) need to be done manually with the larger ones first, in the rib body.
the pattern is done on the entire rib-body (complete crown)
the last edge-fillet is intersect one, point to the boolean Add.2 to get the desired result

regards,
LWolf

 

[ferdo]

Here is another way to do it. You need to follow your company/client methodology. For example, what I did is not allowed for one of my clients.

Regards
Fernando

https://www.youtube.com/playlist?list=PL9mSHa4SOedV3dr0D3kfIWFUg7mIYm94k

https://www.youtube.com/playlist?list=PL9mSHa4SOedVUEkEojiX_kdzpe0sDbaz2

 

[VN1981]

LWolf, thanks for the reply. I will try it out...