Help with sheet metal part

[Govyn]

Hello everybody,

I'm having problems unfolding a cylinder. Using the sheet metal workbench. I've read some of the existing threads, but I'm still unable to have the part recognized.

Any assistance is appreciated.

Thank you in advance

CATIA V5R17

 

[Govyn]

Quick update,

I redid my part starting from a rectangular sheet. I was able to perform all the necessary manipulations, and I now have the part I want. However, when I unfold it I'm given my original rectangular sheet. Is there a way I can unfold it with the geometry I need.

The part in question is a cylinder with the top cut away for mating with the bottom of a tank. The bottom of the tank looks like a dish/bowl.

When I unfold it, I'm looking for a "v" shaped pattern that I can use in the shop.

Again any help is appreciated.

Thanks again

 

[cadddict]

Hi Govyn

Try it this way.
1. Instead of trying to use the "Recognize Walls From an Existing Part" tool, rather generate your cylinder using the "Rolled Walls" tool
2. Then unfold your part and proceed to carry out the required manipulations.

 

[Govyn]

OK here goes.

My first try, I used the shaft tool to create my cylinder and then I cut away the extra bit with the groove tool. The sheet metal apps do not want to recognize it because I don't have a planar surface. The bottom and top open the dialog box, but it still can't recognize the features.

My second try, I made a rectangular part and rolled it up with the sheet metal apps. I cut away the extra bits using the groove tool. When I unroll it, it goes back to a plain old rectangle.

My third try, I made a cylinder using circles and an extrusion. I couldn't even get it recognized. It wanted me to alter the geometry.

With all this I now have another question.

How do I draft/print my unfolded model. I tried to draft my rectangle, but it only comes out as my modified cylinder.

Thank you very much for your help.

 

[Govyn]

I didn't realize I could only upload 1 file at a time, here is the other one illustrating my cylinder.

Thanks again

 

[cadddict]

Hi Govyn

You should not mix sheetmetal tools and part design tools to design your part unless you are using the user stamp tool in the Generative Sheetmetal Design.

You should use the Sheetmetal Pocket either in the folded or unfolded state to modify your cylinder...

I have attached a file for your reference.

Cheers

 

[Govyn]

Thank you cadddict it's great advise, but it doesn't quite work the way I need. The "cutting" sketch is not a straight cut but a revolved cut. It models the shape of the bottom of a bowl. This cylinder serves as a leg for a vertical tank with a dish bottom.

My deadline has already past but I'm still interested in making it work, for ego purposes.

Thank you for your help, I'll try to build on that and see what I can come up with.

I appreciate any extra input you may have.

govyn

 

[cadddict]

Hi Govyn

Post your part file with your revolve feature in it, I will have a look see... Also state what release of V5 you are using

Cheers

 

[cadddict]

Hi Govyn

The other option is to use the Point or Curve Mapping tool in Generative Sheetmetal Design.

First revolve your profile with the surface revolve tool.
Then Extract the external faces of your cylinder.
Then create Intersection Curves between the Extracts and the Revolved Surface.
Next Use the Point or Curve Mapping tool to unfold the Intersection curves.
Finally unfold the part and create a sketch using the unfolded curves as your profile to cut away the material.


In order to generate the drafting view of the flat pattern you need to select the Unfolded View tool in the drafting workbench.

I have attached the files for you to have a look.

Cheers.