I use FreeCAD for…well nowadays pretty much all of my personal CAD needs, including woodworking. For woodworking projects, my workflow is:

• Open the Spreadsheet workbench and start listing out measurements. I start with things like the dimensions of stock and features of that nature in one column, important project overall dimensions in the second column, then calculated or derived component dimensions in the third column. I use a macro called EasyAlias which lets you put a label in a spreadsheet column to the left of the values, highlight those labels, click one button, and it applies that string as an alias to all the cells to their right. Why that isn’t a built-in feature I don’t know, but it speeds things up dramatically.

• Switch to the Part Design workbench, create a Body, give that body a name (something like Side or Shelf or Base, not being spectacularly creative here) and then sketch-and-pad this part into existence. There’s another macro from the addon manager I use here, Dimension From Spreadsheet, that makes this a much less tedious process.

• I often put these in a Part (The equivalent of a Fusion360 “Component”; an abstract group of other things in the tree to keep them together, mostly so that I can disappear all of the parametric Bodies at once.)

• Open the A2Plus workbench (from the Addon Manager). A2Plus is a very simple workbench; it’s not really good for designing machines with moving parts, but aligning faces and edges etc. together works pretty well; it lets you glue the parts of a bookcase together. I’ll import a bottom, back, middle or other “major” fixed Body into the workbench, which creates another object in the tree. These objects I often put in another Part again so I can toggle their visibility all at once. Make this first object “fixed” in space, there’s a value in the Data window for this. I’ll bring in another part, and join it, usually in a “this edge is coincident with this edge; this face is parallel to this face” kind of way, to the first part, and so on until the project is assembled.

• If I need to add or adjust features on the models, I can do that by switching back to the Part Design workbench, then you Refresh the file, and then switch back to the A2Plus workbench which has its own refresh button which updates the A2PLus objects to match the Bodies they are based on. Beware the topology problem; if you create additional faces, the mates may break.

• I don’t always draw both “sides”, sometimes I’ll use the Mirror Body function found in the Part workbench if I feel I need to make sure something fits, sometimes I just don’t bother.

• Using the tape measure tool in the Part Design workbench I’ll verify certain dimensions to make sure everything is working out okay. I’ve also used that tool to very quickly make overall drawings if need be.

• I’ll print out the Spreadsheet, which I find is a useful reference especially when milling and cutting stock to size.

• Using the TechDraw workbench, I’ll create drawings of more complicated parts. In my recent end table project, I didn’t bother doing drawings for the tabletops or the aprons, which were very simple symmetrical parts. The legs on the other hand feature dados, tapers and mortises, so I did dimensional drawings of those.

At this point I’m ready to go to the shop and start butchering some tree meat.

It would be rather nice if there was a woodworking workbench in FreeCAD that let you work with boards and create features like miters, dados etc. in those terms, plus creating things like cut lists and calculating board feet etc. I know there are payware CAD packages that do that. I’m not skilled enough with Python to know where to start though.