Parametric text in part description

[JasonT1124]

I've recently changed over from Solidworks and I'm having trouble linking some text in the parameter table to a dimension.

Basically I want to be able to put a part description (that shows in my BOM) that is parametric with respect to some dimensions on the part. What is the correct syntax to do so? and how do I know what #'s Pro/E has assigned to each dimension?

Thanks for the help!

 

[JasonT1124]

I've almost got it figured out....I can get it to display one dimension and only one dimension... I would like to display a dimension and a string of text.

The problem seems to be that parameters can drive dimensions but I want dimensions to drive parameters.... possible, or no?

 

[looslib]

There is a toggle on one of the menus. Format or Tools, that is labeled Switch dims. This will switch from displaying the dimension to the parameter.

What doe you mean by 'dimensions to drive parameters'? You can use dimension values in a parametric note, but they need converted to strings first.

What version of Wildfire are you on, as things are different depending on the version.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JasonT1124]

I am on Creo 1.0.

I switched the dims to their labels like you suggested already.

My problem is that I want to have a parameter called "Part_Description" and within that parameter I want to type "12 x 15 x dx" where x is a certain dimension that I am interested in. I then want to have one of the columns in my BOM reference that parameter and read "12 x 15 x 7" where 7 is the value of dim x.

 

[looslib]

You will need to use relations to build the text string off the values for a note in the BOM. You cannot use the parametric dimension directly.


"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JasonT1124]

I've been able to get the BOM note to output the value of dim x only, but as soon as I add any other text, the note fails.

What do you mean by add relations? I'm using the relations editor to link the parameter to the dimension now, so my question might be more about syntax.

This works:

Part_Description=@d0

but this does not:

Part_Description=12 x 15 x @d0... I've tried to isolate the text with ' ' marks, but this seems to force the note to output the string as d0 instead of the value.

 

[looslib]

This works because you have a single value being equated to Part_Description.

Part_Description=@d0

but this does not becaue you are mixing string and integer values.

Part_Description=12 x 15 x @d0

Try

Part_Description='12 x 15 x ' + istr(@d0)











"Wildfires are dangerous, hard to control, and economically catastrophic."

Ben Loosli

 

[JasonT1124]

I assumed that is why it is failing. I assume the relation is trying to perform an operation on the text string, which is not what I want.

Your syntax didn't work either...

 

[mjcole]

Try using &d#:fid_##

The d# is the dimension number or name such as DIA or Depth and the ## can be either be the feature name in the model tree, or the id number of the feature. If you type the feature name it should be converted to feat id automatically. No maatter what the name is changed to later on the ID will never change. You can show feature id in model tree by customizing collumns.

You might try making a string parameter and setting it equal to the dx and calling the &Value of that string.