Deleting Useless Features:

[tsqman]

The problem first: I have a part with many features on it (see FeatureTree.jpg) and these features are controlled by a spreadsheet (see SpreadSheet.jpg). When I resolve this part using the Catalog Editor, CATIA creates 21 new parts using the spreadsheet to control, which features are active and deactivated and everything is working, as it should be up to this point. The problem is that all the newly generated parts contain allot of useless deactivated features (see FeatureTree.jpg).

My question is: Is there a way to use the spreadsheet to instead of deactivating the useless features but to delete them. There may be many different solutions to this problem namely using Macros and Rules to name two but one thing it can’t lose, is the spreadsheet must control it because we must be able to use the CATIA Catalog Editor to resolve the individual parts.

Any help in this matter would be greatly appreciated.

Thanks Again

 

[tbuelna]

Older versions of CATIA V5 (R15)actually have a function called "Delete Useless Elements". I don't know why they removed it. It's in the Tools pull down menu.

 

[Azrael]

It's still there, a GSD feature so it only works on non solid elements/features. Have you tried to make a search favorite?, searching for deactivated features, save the search to reuse on other parts later.

 

[tsqman]

Dear tbuelna:

FYI "Delete Useless Elements" is still there in R16 but it does not work for Useless Features and that's what I'm looking for.

Thank you for your reply

 

[tsqman]

Dear Azrael:

I have tried this but was not able to get it to work correctly.

Thank You in Advance

 

[jackk]

DELETE USELESS ELEMENTS erases geometry (lines, curves, surfaces, etc.) that are not used as parents to other geometry. To my knowledge, it does not delete solid features.

It also does not erase deactivated features.

 

[slcad]

I´m not sure if this is what you´re looking for, but to quickly identify and erase inactivated features, try this:

- Tools menu - Parametrization Analysis...
- in the "Filter" drop-down menu select "Inactivated features"
- in the window underneath, the system will display all the inactivated features
- here you can Shift-select all of them and delete them

Hope that helps

Regards,
Stely

 

[solid7]

John - As I posted in another forum, I think that your best bet is going to be writing a script that deletes deactivated features during part resolution.

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[tsqman]

Dear solid7

I agree with you 100% this is what I need to do but that is where the question lays.

1. How do I execute a macro from a spreadsheet?
2. Or how do execute a rule from a spreadsheet?
3. Maybe a combination is needed create a rule first and have that rule execute the macro?

If you would look on the other CATIA forums you will find my email address and if your interested in helping me I will send you some sample models that will better explain my question.

Thank You in Advance solid7

 

[solid7]

Someone here can correct me if I'm wrong - but I don't think that you will want to execute the macro from a spreadsheet. I think that you will want to create a project that contains 2 event triggers;

1) an event to resolve the part you select {from the spreadsheet}
2) an event to scan the resolved part for deactivated features after the "End Sub" in item #1

What those events are depends on your application. (mouseclick, batch script, etc, etc, etc) Those events will, of course, correspond to the scripts that they are activating. You will end up with a project with several modules.


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[itsmyjob]

Well, a macro (vba or vb) can be launch from catia when the resolve is done and as a second step of a complete process, go thru the folder where the resolved catpart are, open each of them and 'clean' them. it does not need to be link with the resolving process... if you really really want that, then it will be easier i guess to include the resolve in the macro...(actually i do not know if this can be done, but you can find that by yourslef...)

have fun

Eric N.
indocti discant et ament meminisse periti ​