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Can't get drawing parameter to display in dimension


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I'm trying to get a parameter to display as part of a dimensions text. I created the parameter CSKDIA (type real_number) as a drawing parameter. When I bring up Info for the parameters it is listed with the correct value. I access the dimension text through properties and enter &CSKDIA. I end up with the actual text string &CSKDIA

If I enter one of the Drawing Lables like &model_name that displays the value of model_name correctly in the dimension text. I tried one of the other listed local drawing parameters by entering &PROI_VERSION as part of the dimension text and that displayed correctly also. I tried Designating CSKDIA but that had no effect (although CSKDIA is not a file based attribute in Intralink I wouldn't think that would be the problem.)

I entered &CSKDIA in a Note instead of as part of Dimension Text and that displayed the value 0.212 just fine.

What am I missing?

Where in dimension text are you typing &CSKDIA? In the prefix, postfix, or as a separate field?

If you're trying to override the dimensional value, are you using &O (capital 'o', not number zero)?

Is it a feature parameter? That might require the format &CSKDIA:fid_featnum where featnum is the feature ID number or name of the feature that owns it.

These are just ideas. I don't actually know if you can include parameters in dimension text.
What I'm trying to do is include the countersink dia and angle in with the diameter dimension for the hole. I created drawing parameters (type real number) CSKDIA anc CSKDEG and they are set equal to d45:70 and d46:70 repectively. When I show parameters the correct values are reported.

I noticed that when I typed &CSKDIA in as part of a note text that Pro/E added the syntax &CSKDIA:D which I assume defines CSKDIA as a drawing parameter (as opposed to a part or assembly parameter). I tried adding this to the text fields in the dimension text. Interestingly the result was that what appeared on the drawing was CSKDIA (droping the & from the text).

I didn't know you could override the dimensional value with &O I'll have to experiment with that as it would solve the problem I've had with not being able to create a drawing that references a table for dimensions. That's such a basic fuction I figured there had to be a way to do it but it's not covered anywhere in the PTC manual Drawing for Designers. At least not that I could find.

>These are just ideas. I don't actually know if you

> can include parameters in dimension text.

Some parameters you can. I was able to get it to include for example &model_name which is another local parameter that's created (I believe) as part of the drawing template.



You cannot include a user parameter in a show dimension type. Use NOTE->OFFSET, then select your dimension and then the location of your text and type &cskdia.

I have successfully accomplished what you have requested:

Remember to use the part number suffix when more than one part appears in a single drawing. In this case the part suffix is :0

View attachment 363

Sometimes, the variables you insert change when you close the Dimension Properties dialog box. Trust that it has worked and Switch Dimensions a time or two to verify - it doesn't always appear to have worked the first time even if you have inserted the variables correctly.

A couple more notes of interest:

It appears that driving dimension parameters (&dX:X) may be inserted into driving dimensions and driven dimension parameters (&adX:X) may be inserted into driven dimensions, but the two may NOT be intermixed.

Only &adX:X type driven dimensions parameters can be inserted into into other driven dimensions. To change the driven dimensions style from &addX:X to &adX:X type, update your file statement to read as follows: create_drawing_dims_only no

Thanks. That does indeed accomplish what I'd set out to do. What's interesting is that you did exactly what I attempted the first time around. Having closed Pro/E and intralink and starting fresh today I noticed that the dimension references had changed from d45:70 and d46:70 to d45:32 and d46:32. I'm not sure what caused this but an additional complication is that the part I am detailing is a family table member. It's likely that the confusion was the result of replacing the generic in the drawing with the family table member and/or a failure to verify the family table.

Although this solution is more direct for this need I'm still wondering why I can insert the value of the parameter &proi_version but not my user created parameter. I guess I should experiment with part and assembly parameters instead of a drawing parameter.


I'm guessing here, but I think the reason Pro/E won't permit inclusion of variables directly into dimensions is because there would not be a way to apply and relate tolerances to them.

I use the technique above because the holenote callout format doesn't permit assignment of decimial places, dimension style or tolerance values to any of the many variables that the callout can include. Were PTC to correct this shortcoming, I'd merely use the holenote callouts instead.