Catia V5R20
Catia V5R20
(OP)
Hi,
I have a CATPart file, with a few solids.
I need to create a drawing file, using only one of these solids(a tube).
How could I hide in the drawing view the solids that I do not want to be shown?
Thanks
I have a CATPart file, with a few solids.
I need to create a drawing file, using only one of these solids(a tube).
How could I hide in the drawing view the solids that I do not want to be shown?
Thanks
MZ7DYJ





RE: Catia V5R20
1. When creating a new view, select the bodies to be included just before you select the view plane.
2. To modify an existing view, right-click on the view and use Modify Links to choose which bodies are to be used.
RE: Catia V5R20
Please, have a look at the attached file(picture).
I'd like to use the "3D elements to add:" domain, but it doesn't work for me: What I am doing wrong?
I can't select another bodu from the 3D file.................!
Regards,
MZ7DYJ
RE: Catia V5R20
MZ7DYJ
RE: Catia V5R20
MZ7DYJ
RE: Catia V5R20
Thanls
MZ7DYJ
RE: Catia V5R20
RE: Catia V5R20
"Overload properties"?..................
How is that?......Can you send more details, please?
MZ7DYJ
RE: Catia V5R20
-right click/modify links
-then go to 3d and pick on solid you want to show
-when you go back to drawing you will see the component in the bottom "3d elements to add"
-click "add all" and that will be the only body visible
even though the fields look grey out, they are still active
RE: Catia V5R20
It works!
MZ7DYJ
RE: Catia V5R20
To see a 3D centerline in a view, go to the view Properties and turn-on the option for 3D Wireframe. (If you have lots of wireframe geometry and only want to see the centerline, move the centerline to a new Geometric Set and then use Modify Links to add that new Set to the list.)
RE: Catia V5R20
Another inquiry:
Catia sketch is always hidden in CATPart. I have a pipe that uses a sketch as a guide. How could (should) make this sketch seen in drafting view, other than making it visible in the CATPart?
Thanks
MZ7DYJ
RE: Catia V5R20
But for the many reasons, the easiest way is not always the best way! So, I suggest:
1. move the centerline sketch (or sketches, or other curves) to be seen into a Geometric Set
2. Show (unhide) the centerline sketch(es)
3. turn-on the 3D Wireframe option for the view (or views) you want to see the centerline
4. use Modify Links for each view that you want to include the Geometric Set of the centerlines
RE: Catia V5R20
I got the centerline of my pipe in drafting view by using View Generation Mode option "Approximative".
No need to do anyting elce in the 3D model!
MZ7DYJ