How to pass part parameters into drawings

[abm23]

Hi,

How do I add part parameters (part name, part number, material, etc) to the part file so that when I create a new drawing those parameters automatically appear in the appropriate fields in the drawing? I believe the fields already call out the various part parameters, I'm just having trouble figuring out how to enter those parameter values into the part file.

Thanks,

Aaron

 

[mbp231]

&PARAMETER

If your part's parameter is PART_NAME, you would put &PART_NAME in a note and the model's parameter value would be shown. It will pull the parameter from the active model in the drawing. The id will automatically be set after you confirm the note.


So you'll put in &PART_NAME. Once you confirm the note it will add the id and will be &PART_NAME:3 or whatever the id is for the part.

For drawing parameters you enter &PARAMETER.

 

[ttroglio]

Aaron,

If you have a part parameter named "material" for example, in the drawing you would just create a note and the text of the note would read ""&material". No quotes of course.

 

[abm23]

I tried adding "&material" (which I confirmed is one of the values in my parameters) to the format file that is used in my drawing, but when I create a new drawing the cell in which I added "&material" just shows up as "&material", not the actual material (which is called out as ALUMINUM in my parameters). Any ideas?


Thanks,


Aaron

 

[alibahadir]

Make sure that the active model of your drawing file has a parameter called "material" already assigned as "Aluminum"





Ali

 

[abm23]

If I add a note to the drawing it works. But if I add a note to the format from which I am creating new drawings, it doesn't (just shows up as "&parameter"). Anyone know how I can include the note in my format file so I don't need to insert new notes every time I make a new drawing?


Thanks,


Aaron

 

[dr_gallup]

In formats the parameter must text be in a table.

 

[abm23]

Ha! Victory! Thanks, dr_gallup, that worked


Aaron

 

[audctrl]

And the ever popular &pro_mp_mass or &pro_mp_volume when working with castings.

 

[eddie]

<DIV>


I thought I would point out one other aspect of parameters in drawings. The examples above willdisplay a parameter from the model which is what you want in most cases.


However, you can also extract a parameter from a drawing that is unique to the drawing by adding a colon D D) to the end of the parameter designation on the drawing. Example &DRAWING_NO


This could be used in many ways. The application of that for us is that we often have multiple drawings for the same model;a marketing drawing, a manufacturing drawing and a transparency templatefor example. The OA folks assign unique drawing numbers that are not necessarily part numbers for each. The QA assigned numbers may change as the product moves through theproduct development and life cycle. We solve that by putting a parameter in the drawing file; DRAWING_NO. It can easily be changed without affecting any PDM relationships (no renaming file names). The drawing number parameter becomes a searchable attribute in the PDM system. It becomes controlled by release level also.


I hope this did not muddy the waters.</DIV>

 

[ozamora]

Hello everyone

I need to convert some information in a table from mm to inches, i will maually input the mm valus and i need it to be transform into inches, all of this in a format environment (.frm) any suggestions ?