Ref 2018 SP5. -- This may be obsolete if issue does not exist in Structural Systems of newer versions.
When I have to add to and edit existing weldments, I avoid breaking the structural member references (which need redefined) by adding new lines to the 3D Sketch instead of extending/trim etc the line to a new length. This particularly applies when two endpoints are shared, and I want to make one longer. I'm not suggesting to fix fundamental issues with sketch trim and extend for Weldments, but rather workarounds. Maybe SS is more stable anyway, so this may never be addressed in future Weldments.
What I was doing was:
Add new colinear line to the end of another line.
Add that new line to same Structural Member group.
Combine (addition) both bodies into one to remove the split.
Its fabrication drawing gets an annotation of associative weldment profile description and cut length placed in one isometric view. $PRPWLD:"Description", $PRPWLD:"LENGTH" LG
What I consistently get in the case of two bodies combined is that its cut length called out was EXACTLY TWICE of what it should be. It took me several failings (i.e. wrong unchecked drawings released to the floor) to narrow it down and catch the source of the problem. I did not test if three bodies combined would call out exactly three times its actual length.
What to do instead: Avoid Combine in Weldments, if using cut length datum. Use Move Face instead.
I've heard many of you bemoan Move Face in the "Things your coworkers do.." thread, but sometimes it applies. In this case, is it present as a stable workaround to another more serious and time consuming issue which is automatically wrong in its results.
To edit my procedure above, only perform the first previous step. Use Move Face (translate, up to vertex or other) instead of adding it to SM group and then combining. This creates stable accurate cut lengths in parametric annotations. I tried several methods of move face: blind, up to vertex, and up to surface, which all returned correct lengths in the drawing.
If you have other purposes for Combine or Move Face, that's fine with me. I am not describing all situations, but only what I encounter. If your weldment cut length is a multiple of what it should be, this is a workaround and potential source of the error. This is a little awkward for me because earlier this year I had suggested Combine as a good workaround for a different issue, which coincidentally was in an earlier revision of the exact same model I am detailing now for fabrication, where the conditions have altered to that the previous issue no longer applies.