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Parametric dimensioning

Parametric dimensioning

Parametric dimensioning

Say I have a part with four holes of equal size. On the drawing, I want to say 4X the size. Is there a way to drive that 4X from constraints on a sketch or a similar method? Such that, if I added a 5th hole to the part, the dimension would automatically update. Similar question for corner rounds. Can the count on their drawing dimension be driven by the model feature?

Jeff Parham
Mechanical Engineer - Design
New Product Development
Colorado School of Mines '09

RE: Parametric dimensioning

It can if you created the holes as a pattern. The pattern will have a parameter such as P1 and if you edit the dimension text and put &p1 X in front of the dimension it will update the drawing with the model.

I'm not aware of a way to get an edge count for rounds but there should be a way as the software obviously knows how many edges were selected when creating the feature. This could only work if you select all the edges during the creation of the feature.


The Help for this program was created in Windows Help format, which depends on a feature that isn't included in this version of Windows.

RE: Parametric dimensioning

Creo doesn't keep count and it would be handy if it did. One difficulty is that what you seen in the sketcher isn't what you see on the drawing. Sketcher is a graphical solver that passes certain geometric information to the calling function, which might be a datum curve or a solid model feature. The dimensions you see in sketcher are pointed to by the calling function and I think are independent data structures. While sketcher could keep count, I don't think there is a matching structure in the calling function that could use it.

It is pesky that PTC never implemented that; it would be very handy.

The rounds is a tougher case because a single edge selection can, via tangency, end up selecting any number of other edges. Those edges may or may not be ones that humans would classify as worth counting as additional, so users would be fighting that incorrect count instead of making the correct count themselves.

The pattern option is the closest one can get, but I don't recall if the count is correct if one of the pattern members is discarded by unfilling its pattern indicator.

RE: Parametric dimensioning

try doing NR_HOLES = p365 in model, relations
and call it in a note as &NR_HOLES:8 x M16x20 (note the space after 8)
8 is part session number. you have to include a space if nr_holes is an integer, i don't know how to get rid of it.

EDIT: method from the first sentence doesn't work, i've tried it.

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