3D Geometry 2

CAD2015 · Sep 2, 2015

Hi,

I am working in an assembly.
I'd like to create a Pad on a component, extracting some geometry from another component.
To do this, I tried to use the 3 D Geometry tool who is located in Sketcher.
It didn't work!
I asked another designer that has over 20 years experience in Catia.
He said that the reason I wasn't able to extract geometry was because the other components can't be selected (become neutral) for geometry extraction, while in sketch.
Is there any way to do that?

Thanks

USSagittarius

JeniaL · Sep 2, 2015

tell to designer it is possible. just go to a sketch and project any geometry from another component. i'm doing that every day and it works.

CAD2015 · Sep 3, 2015

Thanks Jenial,

I am going to send tomorrow another picture that shows the issue.
I am wondering what I did wrong that had made my tentative to extract geometry from another component failing?..................

USSagittarius

jackk · Sep 3, 2015

do you get an error message when you try to select something? does the cursor change when you hover over other geometry?

I agree with Jenial, this is a pretty common practice with CATIAV5. I think you have a setting needs to be changed.

kr7530 · Sep 3, 2015

Like Jenial it is an everyday thing for me. However, there are a few things that can effect whether you can or cannot use external geometry.
Not sure what error you are getting so I will give some possibilities that I have run across:
- How are the parts contextual links are defined. Are the parts in different sub-assemblies?
- Would the link create a cycle/loop?
- In Sketcher are you set to "Pickable visable background"?

If you don't need to keep the link you should be able to toggle "Create Datum" and then "Project 3D Elements"

JeniaL · Sep 3, 2015

the designer with 20 years experience from first post need to dig deeper into catia.

lardman363 · Sep 4, 2015

You could have your context defined in another assembly.
You may need to publish the geometry from part A before you can link it to part B. Or you would need to turn off the setting that forces you to only link to published geometry. It depends on how your company wants you to handle linking to other parts.

CAD2015 · Sep 8, 2015

Hi,

Thank you all for replies.
Jackk:
- No error message; the cursor doesn't change when I hover over other component's geometry.

kr7530:
- The parts are in different sub-assemblies
- Sketcher is set to "Pickable visible background"

JeniaL, lardman363:
While working in Assembly and my component that I want to modify is active, I try to select a planar face from another component in order to create a plane or a sketch.
The face can't be selected! I can't copy or create any geometry from the other components!
Could it be a setting issue?
Or I do something wrong?................

USSagittarius

CAD2015 · Sep 8, 2015

The question is: What would make the Assembly's components neutral (unable to be selected) while working in another one?

USSagittarius

itsmyjob · Sep 9, 2015

Let us know if you have the option hybrid modeling turn on or not.

Eric N.
indocti discant et ament meminisse periti

ferdo · Sep 9, 2015

Hi,

Maybe when you are in Sketch (hope I understood well), you have the low light active and then indeed you can't select nothing. When you switch to Usual should be OK, see attached picture. This toolbar is near your Pickable visible background.

Regards
Fernando

https://picasaweb.google.com/102257836106335725208

- Romania

https://picasaweb.google.com/103462806772634246699/

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CAD2015 · Sep 9, 2015

Eureka!
The problem was in Catia Option settings (see the attached picture).
The issue was the two boxes (or maybe just one of them, I am not sure yet) in the Option menu:
1. Keep link with selected objects (should be unchecked)
2. Restrict external selection with selected objects (unchecked, either).

Please, feel free to comment this last comment.
You contribution in this matter would be highly appreciated.

USSagittarius

JeniaL · Sep 9, 2015

Keep link with selected objects shall be checked. if you uncheck this there will be no link to external geometry.

lardman363 · Sep 12, 2015

As JeniaL mentioned, I would leave the settings alone.

It sounds like the plane you want to sketch on in Part A is not PUBLISHED.
Place Part A in Edit mode (double Click on it to make it blue)
Select the plane you want to sketch on
From the menu pick Tools > Publication, Yes you want to publish the selected elements, Ok the publication window (a new feature appears at the bottom of your tree under the Publication Node)

Place part B in edit mode (again, double click on it to make it blue)
select sketch, then select the plane that you published from Part A (CATIA should automatically create a reference to the plane inside of Part B)

CAD2015 · Sep 13, 2015

Thanks lardman363!

USSagittarius

itsmyjob · Sep 13, 2015

CAD2015 said:
No error message; the cursor doesn't change when I hover over other component's geometry.

Well...

You need to check your screen because this is what you should see in your environment:

with the default option (keep link with unpublished element) you should have this:

The cursor is not the same and there is an error message (actually it tells you why you can't select the surface)

Glad you get the solution...

Eric N.
indocti discant et ament meminisse periti

CAD2015 · Sep 13, 2015

Itsmyjob,

Nice example, thanks a lot!

USSagittarius

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