First off I wanted to thank people that have answered my questions in the past, and let folks know I did search for this answer. We are finally out of the dark ages (SW 2004) and running SW 2008. We're going to run it for a few months before setting up PDM Works.
I'm trying to setup my Drawing Template to be more automated, and I can't figure out how to get it to callout the Material I choose in the Feature Tree of the part file. I've added this to my Drawing Template: $PRPSHEET:"material" but when I insert a part view into my drawing sheet, this doesn't update with the material info I had selected in the parts Feature Tree.
I would advise not using the Material value directly. There's three problems with this when it comes to materials and the SolidWorks material database library. First, the material names used in SolidWorks standard library are not the correct or even common names for those materials. Second, if you need accurate specification, the standards that define the materials are not even mentioned of the library, making references to material incomplete. Third, the names of the materials are not capitalized, so they are not formatted correctly to be used directly on a drawing in the first place.
Solution, change your library to add this info and correct formatting (create a new library to do the same) OR enter the info manually on the part in a custom property, then have that value pulled into the drawing via the method mentioned above.
If you choose to use a custom property in the model, simply link to that value in an annotation note on the drawing using the method above. If you still wish to use the material value of a model directly, you'll need to do one extra step (also involving the use of custom properties):
In the drawing, create a custom property called something like Material or whatever you wish. Do the same in the model. For the value of the drawing's Material property, type "$PRP:"Material" For the value of Material property, just click on the down arrow of the entry field and select Material. Back on the drawing, create an annotation link that links to the DRAWING's custom property Material.
That's it. Easy? Well, not really, but not hard once you know.
Thanks for the answer. I can understand the problems in linking now. However I think I'll follow your suggestion and make our own custom material database. 90% of our parts are out of 6061-T6 so as long as I add that (instead of 6061 Alloy like it defaults to) we should be fine.
The thing I don't understand is, even if I do want to use the SW Material Database, I still can't get that to show up in in my drawing when I add $PRPSHEET:"material". The only way I can get it to show up is if I had a custom Material in the Properties box.
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