Change contours in a pad 2

[jmuriarte]

Hello:

Is there any way to change the contour of a pad using parameters?
With the pad allready created use a parameter (string , boolean...) to say which is the correct contour(A or B).

Thanks

 

[solid7]

Technically, NO. But there may be a workaround, depending on how you want to define the contours. Are they overlapping, (as in laying on one another) or is there some distance between them?

One option is just to define one of the countours, and then use a split operation for the option of using the second countour. (could be 2 splits if it's an offset contour) Then, you can use a Boolean parameter to control 'Activity' of the split operation.

Drawbacks:

1) not generally a good practice to use boolean parameters in a part design (deactivated parts)
2) Only good for controlling 1 configuration
3) it's a workaround

You could very easily do this with some knowledgeware products.

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Catia Design|Catia Design News|Catia V5 blog

 

[itsmyjob]

You need knowledgeware to create a rule 'if then'

Then create 2 sketches A and B

Create a parameter 'curve C' (end of drop down list) and link it to sketch A

Define your rule your if ... then Curve C = Sketch A else Curve C = Sketch B

Eric N.
indocti discant et ament meminisse periti ​

 

[solid7]

Now that Eric posted his response, I see a confusing statement in my first reply. Instead of this:

You could very easily do this with some knowledgeware products.

I should have said this:

"You could very easily accomplish what you want to do, not with parameters, but with some knowledgeware products".

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Catia Design|Catia Design News|Catia V5 blog

 

[catiajim]

Actually, you can set up a Curve type Parameter with multiple values. The sketches would then become the "values" of the Curve parameter. Changing the Curve Parameter will change the definition of the Pad. It's been a while since I tried this (COE 2002 maybe?). It was in a COE university class on Advanced Parametrics in V5. I believe that Joe Konecny was the instructor. Joe is currently with Technigraphics (formerly MSC).

 

[solid7]

So without any knowledgeware, this IS possible?

Could you please post some more information on this? I would like to know more.

Thanks, Jim.

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Catia Design|Catia Design News|Catia V5 blog

 

[catiajim]

I tried looking for the manual from that session, but it has disappeared in sometime in the last move or two. It would take some experimentation to figure it out again. There may be something in the on-line docs (my network is trash this afternoon, or I'd look it up). I don't know what license it may take, as we have both KWA and KT1 in our base configuration.

 

[jmuriarte]

First thanks for your posts.

I will try to explain better what I´m trying. I want create a ounter contour of a part from a datum contour. It must be done with an automatic contour(offset from the datum..) or if I activate or deactivate a parameter from a manual sketch.

I think it could be like itsmyjob explains in his post but I dont know what kind of parameter is "curve C" and how can I link to a sketch

Thank you again.

 

[solid7]

I have to apologize - in my first response, I thought that you were creating a pad from a non-planar profile. (i.e. - a surface)

Do you have the knowledge advisor workbench, jumuriarte?

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Catia Design|Catia Design News|Catia V5 blog

 

[itsmyjob]

When you create a parameter using the f(x) function,
before your clic the "create parameter" button, select in the drop down list the parameter type (integer, string,.... at the end of list you find curve, point, surface)

then apply a formula like you do with any aother parameter, only this one is geometrical not numerical...

Eric N.
indocti discant et ament meminisse periti ​

 

[DBezaire]

jmuriarte - if purchasing KWA is out of the question, make 2 boolean parameters called ContourA & ContourB. You could activate the sketch using f(x),select sketch, look for sketch.???\Activity (using filter type boolean) - add the formula to this parameter. (this would be the boolean parameter created above)

Regards,
Derek

 

[jmuriarte]

I get it , thank you very much.