This is a problem for me as well. I tried using the tolerances but ended up adding a part or section for weld shrinkage.
I have also made derived configurations and use one for pre-welding sizes and then use the original for the "real" sizes.
This will allow you to leave the original model in tact and you just add the derived configs.
Thanks Francisco. I guess if we clearly define this process in our organization we can train our manufacturing personnel to only grab the configurations that are made for manufacturing use. We often burn plate shapes a bit larger to account for weld shrinkage or burn a shape small if it needs to fit between two other plates.
We used to use configurations for this type of work, but now we use Insert => Part. Open a new part file for the manufacturing engineering version of the part and then go to Insert => Part and select the designed part. This will give you a starting point that is the designed part and you can do whatever you want to it without affecting the designed part, i.e., screwing up the part and pisshing-off the designer. If the designer makes any changes to the design part those will show up in your manufactured part file. We found this to be a far superior method versus using configurations. Your manufactured part can use the Scale function if that gives you what you need or you can make cuts and material additions to represent your manufacturing operations. Give it a fair evaluation, you might find it to be just what you were looking for.
Just food for thought here- have you considered using the Scale feature?
In a former and unrelated industry (tungsten carbide inserts, sintering process), I did essentially what Francisco mentions above (and I'm curious as to Francisco's method...did you manually adjust the dimensions individually for your 'pre-welding' configurations?).
In my process I would model the part to the desired finished size and then create a new configuration and scale it accordingly to account for shrinkage. The scaled model was then used to create the molds/tooling. This was possible, effective, and relatively simple since the shrink factor was predictable and typically uniform (though sometimes not..). It may not be as straight forward for your process but I could see how this might apply to what you are doing if shrinkage is predictable & repeatable (of course w/ respect to material, material thickness etc.).
The Scale Feature can be applied to specific bodies in a muli-body part. And it can be applied uniformly, or in the X, Y, and/or Z direction independently.
It's just an idea, maybe something to try?
If I had to model in weld shrinkage for structural members then I would use the face-offset feature. I would model the theoretic shape of the machine and add it at the end to all joints and group the features in a "ShrinkAllow" folder. If it was a weldment part, i would then use two configurations.
A - for the finished size (ShrinkAllow suppressed) that I can use to dimension the weldment. B - for the individual body drawing & Bom (ShrinkAll Unsuppressed) that I can use to dimension the members.
Granted that your shrink allowance is predictable and you have your manufacturing part figured out.