A question about the product tree

[rbarata]

Hello, my friends

How can I use a sketch created after a feature to modify that same feature?
Imagine I have a pad and after it has been created I decide to make it not normal to a plane. I create then a sketch with a line (for ex.) to use it as a orientation line for th pad.
The problem is that I can't use it because it was created after the pad. I tried several solutions (reorder included) but it is not possible.
Is there any turnaround for this problem?

Thank you

 

[TibiX]

Hello rbarata,

I'm sensing two questions...
[ol 1]
[li]Modifying an existing feature is easy... double click it (and for your example, the pad which is not normal to the sketch plane, use a line created in a Geometrical Set to indicate the direction of extrusion);[/li]
[li]If you wish to create a feature which shouldn't be the last one, just right-click and Define in Work Object on the feature you want to precede the feature you want to create.[/li]
[/ol]
Hope this helps,
Best of luck!

CATIA V5R21 – mold tool design engineer

 

[jackk]

Rbarata,

Move the sketch into a Geometric Set. Then the sketch can be used anywhere within the Body.

 

[rbarata]

I see...geometrical sets are like places where we can store sketches to be used in the construction of more than one body feature. Obviously, if we create one of these sketches right at the beginning, probably it won't be a problem. But if we get to the conclusion that we missed some sketch in the initial stages, we can create it inside a geometrical set and use it in any body feature.

One thing I noticed....in my pad (example above), if I select the complete sketch from the geo set, the direction reference in the pad definition window does not change. I need to select literally the line in the main window. Is this normal behaviour? And if the sketch has more than one line, for example? It only let me choose one.

 

[jackk]

yes - Geometric Sets are places to store construction geometry. By default, the Geometric Set is un-ordered so features can be in any sequence. (be careful not to use Ordered Geometric Sets.) Where I work, our Best Practice is to keep ALL sketches in various Geometric Sets, so they can be used in multiple bodies, plus easily hidden or shown.

If I follow your second comment; no - that is not normal. Regardless of where the sketch is stored, the Pad dialog should default to NORMAL TO PROFILE.

 

[rbarata]

If I follow your second comment; no - that is not normal. Regardless of where the sketch is stored, the Pad dialog should default to NORMAL TO PROFILE.

Let me explain better...the issue comes when I want to use a sketch with more than one feature, two lines, for example. It is possible to select the complete sketch in the tree but the pad definition window does not change (the reference field in the Direction window). Of course I have previously deselected the Normal to profile option. I must select one of the lines from the sketch. Maybe that's because I can only use one line at a time to establish the pad direction. But if that's the case, I would expect some warning from Catia.

 

[jackk]

thanks for the clarification.

Sketches are noramlly a group of geometry (points, lines, curves), and using a sketch means using all the geometry within the sketch. If your sketch had more than one line, the PAD dialog won't recognize it as a single direction.

You could have drawn a sketch with only one line to define the direction.

Or evem better, just draw a line in 3D. Or use an Axis.

You could also use a straight edge to define the direction. But that might cause problems later, and is considered "bad practice"