Quick question

[fjodor]

I would welcome some help in removing part in assembly.
I did managed to solve problem using GSD-part combination but I'm wondering is there a better way. My first part is eliptical cap (for gas containers) and the other is clynder.
What I need to do is cut cylnder bottom to match cap shape, clynder is little smaller then hole in the cap.
Picture speakes 1000 words so here it is (it's solidworks design but principle is the same)

 

[norkamus]

So you would like the bottom of the little cylinder, the end we can see in the picture, to follow the same contour of the part (cap) it is assembled into?

I'm thinking to create the cylinder as a pad, in context with the cap (in a product), Then use the caps' interior contour surface as the termination. The surface will then become an external reference in the little cylinders' part file.

If I've got it wrong, perhaps you could elaborate...

cheers,
Nick

Light structural commercial aircraft parts
PCDMIS 4.3 CAD++, CATIA V5 R20, NX6
APM Consortium Inc.
Cambridge Ontario, Canada

 

[fjodor]

That's right, I need it to be in two parts for further manifacturing and drawing, I could also copy/paste sketch from eliptical cap and then groove clynder, but I'm lookin for a way to trim the lump in product and not in part...so yes, I would like for cylnder to follow the curve from cap and for two things to be seperate parts

 

[norkamus]

If you want the cylinder to be whole (as it is pictured) as a CATPart, but modified to conform to the cap in the CATProduct, I don't remember how to do that. I do think you can perform design functions in a CATProduct without affecting the original CATPart files. I think it's called associativity.

When I was taking the 5 day course with our CATIA vendor, we created an assembly (Product) and added a hole feature through two of the components. The hole definitions only existed in the Product; the Part files were not affected by the holes. I think this is similar to what you're going for.

Unfortunately, I can't go any further to help you. Perhaps someone else can pipe in here on associativity. I think that's what it's called.


Nick



Light structural commercial aircraft parts
PCDMIS 4.3 CAD++, CATIA V5 R20, NX6
APM Consortium Inc.
Cambridge Ontario, Canada

 

[DaSalo]

In the assembly workbench go to Insert=>Assembly Features. There will be a list of various boolean type operations that can be performed at the assembly level. There is a split function there that would likely do the trick or you could use one of the subtract type functions. I haven't used these much so can't give you exact process.

You will likely need to create an additional CATpart that will be used only as the cutting tool to perform this operation. For example, create a CATpart and link in the inside surface of the cap. Now extrude the edges down to a plane created at the bottom edge of the cap and sew on the top surface so you now have a solid that represents the interior space of the cap. Since it is driven by a live link to the original cap everything should stay associative if you make modifications. Now use this new solid to perform a boolean subtract at the assembly level from your cylinder. That would give you the shape you want. I'm sure there are dozens of other ways to do this also.

Hope that helps.

CATIA V5 R20
PC-DMIS 2011 MR1

 

[DaSalo]

One more thing. Since you will be creating a drawing remember to turn off the "visualize in bill of materials" check box in the properties of the new CATpart created for the boolean so it doesn't show up as part of your assembly.

CATIA V5 R20
PC-DMIS 2011 MR1

 

[jackk]

Fjodor,

Your original problem can easily be done with Contextual design links:

1. First create an assembly with the two parts constrained to each other. I will assume you have already modeled the cap and the cylinder in each part.

2. Modify the cylinder:

a. double-click on the cylinder to make this part active and to switch into the Part Design workbench

b. double-click on the cylinder again, this time to edit it.

c. change the limit type to UP TO SURFACE, and then select the inside surface of the cap.

d. click OK and you got it.

 

[DaSalo]

I agree that jackk's way would be the easiest if you want the cylinder to have the gas cap shape on the end all the time, not just at the assembly level. For some reason I was under the impression that you wanted it to be a cylinder at the component level and then take on the contour of the gas cap only at the assembly level.

CATIA V5 R20
PC-DMIS 2011 MR1

 

[fjodor]

jackk, nice and fast way. THX

 

[norkamus]

Isn't that what I originally posted?

Nick

Light structural commercial aircraft parts
PCDMIS 4.3 CAD++, CATIA V5 R20, NX6
APM Consortium Inc.
Cambridge Ontario, Canada