In some cases it’s easier to model assemblies using
multi-bodies in a single part file. But when it gets to the point where you
need to create a BOM drawing, you need to save out the bodies as separate part
files and put them into an assembly. This can become quite tedious and will
definitely require some additional space on your hard drive.
Luckily, there is a short cut to this process. Why not try
using a weldment cut-list instead?
Here are the steps:
1 - Start off with a multibody part. In this case we
have a set of geometric primitives laid out around the origin:
2 - Right-click on any of the tabs on the Command
Manager and activate the weldments tab:
3 - Now switch to weldments tab, and click on the
will activate weldment functionality in your part. All solid bodies will be
treated as cut list items:
Cut-List-Item folders can now be renamed, and each one of
these can now be assigned with material and any custom property of your choice:
4 - Now when you make a drawing from part, you can use all of
these in a cut-list table that will immitate a bill of materials:
on a table cell and use ‘Insert’ option from context menu to add columns to the
on the index cell above the column you want to change and choose a property to
on changing column properties until satisfied. Auto-baloons work just as well
with Cut-Lists as they do with BOMs:
Now this part drawing looks almost indistinguishable from an
assembly drawing, even though no assembly was made.
5 - The table you have created can be saved as a
template in case you need to use a similar setup for another part file/drawing:
Since this is not an assembly, no mechanical
interaction can be simulated with SOLIDWORKS Motion.
- Exploded view functionality is only available in
assemblies, but this can be imitated with ‘Move/Copy Bodies’ and 3D-sketching
explode lines manually.
- No sub-assembly nesting in BOM-like cut-list tables.
SOLIDWORKS Applications Engineer