Automatic feature classification into geometrical set

[Vertx]

Hi,

I would like to know if somebody has a method/script/macro to automate the classification of features into respective geometrical sets (CATIA V5).

Example : Creating a "Line" would put it under the geometrical set "Line" even if this particular geometrical set is not "defined in work object".

I group all reference elements independently from my surfaces so I can hide all the wire-frame geometry at once.

Alternately, a macro for showing/hiding all wire-frame geometry would work, but I would prefer to have the same features grouped together for the tree's sake.

Thank you very much

 

[ferdo]

Hi,

If I understood you well, that means after creating a feature (for example a line) you want to run a macro to pick-up the feature (line in this case) and put it in a specific GS (selected by you or predefined), isn't it ?

This can be done without problems.

Regards
Fernando

 

[Vertx]

Precisely, except that I would rather have something that does it in real time if possible, instead of a macro that has to be launched.

Thank you for your reply Fernando, much appreciated

 

[ferdo]

In real time I believe is not so easy because there are too many ways to create a feature...let me think...

Regards
Fernando

 

[ferdo]

I just realize that it will be much easier to do what you want if you search a specific feature at the end of the work (let say lines) and just CHANGE one type of feature (lines) in a specific Geometrical Set - Change Geometrical Set

Regards
Fernando

 

[ferdo]

This is just a simple CATScript


Language="VBSCRIPT"

Sub CATMain()

Dim partDocument1 As Document
Set partDocument1 = CATIA.ActiveDocument

Dim selection1 As Selection
Set selection1 = partDocument1.Selection

selection1.Search "CATPrtSearch.Line,all"

Dim part1 As Part
Set part1 = partDocument1.Part

CATIA.StartCommand "Change geometrical Set"

part1.Update

End Sub


Regards
Fernando

 

[Vertx]

I get this error message...

Source : Microsoft VBScript compilation error
Description : Expected end of statement
Statemenet : Dim partDocument1 As Document

I'm a newbie with scripts...

Thanks Fernando

 

[ferdo]

Check please the attachment.

Regards
Fernando

 

[Vertx]

Wow, works perfectly! I owe you a beer

I've created some for planes, points, sketches also...
Where can I find the feature name's list to correctly designate the other one? (Spline or 3D curve perhaps)


Another quick question ; let's say I create an extrusion and I define the direction by creating a line within the extrusion direction's contextual menu. The line will be under the extrusion's node in the tree, hidden. That's fine by me... Is there a possibility to skip the features that are defined this way?

Again, thank you very much for your time
Best,

Mat

 

[ferdo]

First question: push CTRL+F and look in Advanced Search Tab for Part Design Workbench.

Second question: you have the possibility to exclude from a selection different things, you just need to find the criteria...maybe an example uploaded here it will be much helpful to find a solution.

The CATScript is done by simply recording and just add a StartCommand line at the end...is really nothing fancy...and for sure can be improved (in catvba, with graphic interface, buttons, less clicks, a.s.o.), you need just a little time - unfortunately I don't have now so much..


Regards
Fernando