Catia V5R20 2

[CAD2015]

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

MZ7DYJ

 

[jackk]

There are two ways when dealing with multi-bodied CATParts:

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.

 

[CAD2015]

Thanks Jackk,

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

 

[CAD2015]

The "3D elements to add" domain is not active!.....

MZ7DYJ

 

[CAD2015]

Do I need to modify something in Option?

MZ7DYJ

 

[CAD2015]

Also...let's say I need to bring the centerline I used to create a pipe in 3D: How could I place it in drawing view after the view has already been created??

Thanls

MZ7DYJ

 

[jopal]

I believe "3d elements to add" is only for adding catparts or products. I believe you can use overload properties which will work with multiple bodies.

 

[CAD2015]

Thanks Jopal,
"Overload properties"?..................
How is that?......Can you send more details, please?

MZ7DYJ

 

[jopal]

my mistake, overload properties seems to only work with catparts, not individual part bodies. To do what your are asking;
-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

 

[CAD2015]

Thanks jopal!
It works!


MZ7DYJ

 

[jackk]

As jopal said; Modify Links works with choosing Bodies within a CATPart drawing. It also works with Geometric Sets. And Overload Properties is similiar, allowing you to hide/show Parts within an Assembly drawing.

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.)

 

[CAD2015]

Thanks again Jackk, great tip!
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

 

[jackk]

The easiest way to see one sketch in a drawing is to hide all sketches but the one you want to see, and turn-on the 3D Wireframe option in the view properties.

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

 

[CAD2015]

hello guys,
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