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).
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.
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).
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.
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
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
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)