I'm trying to figure out how to put a reference or driven dimension a flat pattern so I can have the result show up in a family table. I want to have a table of flat sizes on a drawing.
We tried doing an unbend then putting a dimension in and bending it back, but this didn't work: the dimension changed to match the formed part. We ended up doing it by using relations to calculate the value. We'd like to find a way to use the actual developed flat to generate this value. Any suggestions?
First, in your config.pro file you need to have allow_anatomic_features set to yes. You can create an evaluation feature by analysis>measure>length and in the dialogue box changing the tab from quick to feature. This will create an evaluate feature in the model tree.
Next, in relations you can enter something like: STOCK_LENGTH=DISTANCE:FID_DIST_EVAL, where stock_length is the desired parameter for the length you wish to employ in you bom, and dist_eval is the name of the evaluate feature.
You can do this for length, width, and height, and unfolded length.
In sheet metal I create an unfold feature, do the evaluate features, and then bend back. Then I make a family table to include/exclude the last feature.