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Trying to make a "generic" dimension in Wildfire...

swcalvert

New member
Add a dimension and edit the text to say 'L'. You then have to make the table on your drawing to show what 'L' is. There may be a different way, but I'm not yet up on all the Pro/E functions



Steve C
 

swcalvert

New member
I'm sorry, Paul. I can't make it happen either. I know I watched someone do this before, so I know it can happen.



Steve C
 

lcoates68

New member
Edit the dimension and replace the dim text @D with @O(letter O) and then your letter L. The O stands for overwrite and will blank the dim value. If you need the number back then replace the O with D and the number will be back to the default.
 

Brian_Adkins

Moderator
Another more-associative method is to set the symbol for that dimension in the part to 'L' (Modify/DimCosmetics/Symbol). Then, on the drawing, use @S instead of @OL.



@D = actual dimension

@O = out of scale (you can put whatever you want)

@S = dimension's symbolic name (i.e. 'L' or 'd145')



-Brian Adkins
 

donha

New member
There is a problem with changing the symbol of a driven (created) dimension in Pro/E. Let's say I have created a driven dimension on the print, changed its Symbol to be L, then somehow it gets erased. You can never use the Symbol L in the drawing again because the erased driven dimension will never re-appear. I would suggest the {1:mad:O}{2:L} approach and would suggest changing the driving dimension in your table symbol to L. Changing the driving dimension to the appropriate symbol to agree with your table, makes it easier to fill out your table as well as view your family table and associate columns to dimensions.
 

Brian_Adkins

Moderator
>> There is a problem with changing the symbol of a driven (created) dimension in Pro/E



Never thought of trying that... Are you talking about inserting the 'L' value in two separate places?



I'd just put the 'L' in the part model and then put @S on the drawing and be done with it. It will automatically show up as 'L' in the family table as well as well as the header text on a tabulated chart on the drawing (table showing value of 'L' for all instances)... This is done with a family table repeat region.



Many companies have ModelCheck set up to look out for '@O' on drawings which can definitely be a hazard.



-Brian Adkins
 

donha

New member
Doesn't the dimension disappear from the drawing if you insert @L in the table? Yes, you cannot display a driving dimension shown in a table. You must use {1:mad:O}{2:L}. The practice I use is the result of someone erasing a driven dimension on a print and never being able to use the symbol again. I tried erasing a driven dimension with a changed symbol from the print. The dimension could be shown again. This was on a simple block part. If the part is much more complex, the dimension might be lost forever.
 

Brian_Adkins

Moderator
This is how I do drawings of family tabled parts:



1) create part

2) change symbol for dims that are to be 'tabled' (i.e. 'L' and 'DIAM' below)

3) create family table

4) create drawing and add a Fam-Tab repeat region (see below)

5) create drawing views and show dims

6) for family-tabled dims, change @D to @S on the shown dims



Here is resulting drawing (No out of scale or driven dims used)

View attachment 258





Here is how the drawing table is created:

View attachment 259
 

dr_gallup

Moderator
I don't think you can change the drawing table values when they are in a repeat region, you have to change the part family table. So there is no chance for error. I find it MUCH better to tabulate drawings rather than having seperate drawings for each instance. Much easier to keep up with all the paperwork when there is only one drawing to revise.
 

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