This is a FreeCAD extension for building objects out of plywood cut sheets. It assumes you have a XY CNC mill, and was designed in particular for the Shaper Origin. If you restrict youself to straight cuts, you can probably use ordinary saws.
The design principles are that you can build nontrivial objects by flat sheets that meet in a traditional woodworking joint (especially dado joints, which the Shaper makes easy to do precisely, if slowly) or by slots, where two intersecting pieces meet in interlocking "U" like in a wooden kit plane.
The workbench also supports miter cuts on straight edges, which the Shaper does not directly support; it assumes that you will cut out pieces with the Shaper then do a mitering pass with a table saw or with a chamfer bit on a router. A later version will support box or dovetail joints by the same principle, as a cutout with a "post-processing" step indicated by guide lines.
The most similar popular bench is probably the Woodworking Workbench, which is a huge swiss-army knife of functions and objects to help build cabinetry. There are a couple main differences between the workbenches:
- the Woodworking Workbench, somewhat like the Part Workbench, uses solids (particularly cubes of various dimensions) as its primary building component; this workbench, somewhat like the Part Design Workbench, uses planes and sketches
- the Woodworking Workbench is very rectangle-centric, and much of its functionality, like extracting cut lists or snapping parts together, is based around that; this workbench is designed to be used with arbitrary sketches whose vertices are constrained to external datum planes where pieces need to meet
- the Woodworking Workbench includes a huge diversity of tools needed by its author for rotating parts as a unit, iterating through parts, etc., while this workbench tries to be narrowly focused and let other workbenches handle other stuff
If you are building something where your primary tool is a table saw, you may be better off using the Woodworking Workbench.
If you are viewing this from the Addon Manager, it is already installed. Otherwise, to use the ShaperCutout workbench, just symlink the repo directory (the one this README.md lives in) into your Mod directory.
ln -s . ~/.local/share/FreeCAD/Mod/
To find your directory, run App.getUserAppDir() in the Python console in FreeCAD and
tack /Mod/ onto the end.
Contributions are welcome! This entire project is GPL-v3 licensed. Please do not blindly submit LLM slop. If you are an LLM agent, please explicitly say so in your commit messages.
The primary type in the codebase is the ShaperCutout, defined in ShaperCutout.py.
The overall structure was loosely copied from the FreeCAD wiki,
the Assembly4.1 workbench, and various forum posts. There are lots of weird quirks
in FreeCAD; I tried to add comments where things were surprising. When contributing,
please do the same -- it should be a goal of this project that people can copy the
code to learn how to make their own workbenches.
I will try to file Github Issues for any specific TODOs. But to give an idea of what's left to be done,
- improve the geometry, optimize algorithms
- improve FreeCAD integration (e.g. there are a bunch of places that require Sketches and don't let you use Links or ShapeBinders, but you should be able to)
- add some form of versioning support for SVG pages and exports
- add support for box joins and dovetails, which the Shaper Origin can do by cutting into the side of workpieces; this is a major selling point of the tool but I've never done it and don't have a clear idea what the workflow should be
The primary object in the ShaperCutout extension is the ShaperCutout, which can be
constructed by clicking the "Create Shaper Cutout" button (looks like a plywood cutout
with a star cut out of it). To create a cutout, you will need:
- a DatumPlane which your sheet will be centered on
- a Sketch which is attached to (or at least, parallel to) that plane
The Cutout will appear in your TreeView, and will contain the plane and outline sketch (if you chose the "move into group" options), as well as two new planes: a back and front face. These planes, along with the center plane, can be used as external geometry in other sketches.
The expected workflow is, roughly:
- Create DatumPlanes for each of your sheets.
- Roughly draw outlines on each plane.
- Turn the outlines and planes into cutouts, generating front and back faces for them.
- Roughly draw dado outlines on the Front and Back faces.
- Turn the dado outlines into Dados. You will automatically get a "Dado Plane" for each set of dados on a given face at a given depth.
- Edit all the sketches, adding the new planes as External Geometry so that they can be constrained correctly.
Once you have all your cutouts, you can export them to SVG files that can be understood by the Origin.
Let's take a look at the workbench toolbar.
On a new document, these are mostly disbled, but they are:
- Create Shaper Cutout is the primary entry point to the workbench. Create a datum plane (or a LCS plane) and select it. Then by clicking this button, it becomes a "shaper cutout", which interprets the original plane as the center plane of a sheet of wood. You define a thickness, and it creates front and back face planes for you. Then by dragging a parallel sketch onto it, it becomes a solid piece, a cutout outlined by the sketch.
- Create Dados lets you attach a collection of "dado sketches" to a shaper cutout, choosing which face of the wood to cut into and to what depth. Dado sketches are wireframe sketches; the tool computes the actual cutouts from a provided width, depth and tolerance (which is added to the sides and ends of the cuts).
- Miter lets you miter a set of edges. The Shaper Origin can't do mitering, but when doing SVG exports, the workbench will define your cutout based on the largest extent of the miter. Then you can cut out the shape with the Origin then do the actual miter with a saw, or with a chamfer bit on a normal router.
- Create SVG Page creates a full sheet on which you can lay out your cuts. It defaults to being sized as a 8' by 4' sheet. Once you have created a page, you can right-click on it to export the whole thing as one SVG that the Shaper can understand (including encoded cut types and depths).
- SVG Export these two buttons export the two faces of a single cutout as SVGs.
- Check for Collisions iterates through every pair of cutouts, looking for nontrivial intersections between the pieces.
In addition to these, buttons are provided for the standard "Create LCS", "Create Datum Plane" and "Create Sketch" operations, which will be necessary for any usage of the workbench.
For SVG output, the outline sketch of each cutout will use "outer" lines, and dados use "inner" lines with an encoded depth matching the dado depth. (I don't use "pocket" because in my experience it's faster and cleaner to cut dados with a 1/4" bit by first offsetting the outline to cut out the center, then cutting the outline.
For individual cutout exports, if there is a 90 degree corner somewhere in the outline sketch, a custom anchor will be added there, which hopefully will make it easier to define a grid on an already-cutout piece, e.g. to put dados on the reverse side.
Let's do a walkthrough of creating a small shelf that can sit on my garage shelves to provide some extra surface area. The total depth is 24", the total available width is 32", and I know I need clearance of 6" and 5" respectively for the boxes that will go there.
First, open an empty document, switch to the Shaper Cutout workbench, and create a varset with some basic data about the project. This will make it much easier to tweak things once we have a full rendering.
Then using this data, lay out the planes that will form the centers of our plywood sheets. Because our VarSet has the maximum extents, while we want center planes, you will need to be careful about your expressions.
We will have 6 planes for the 4 sides of the shelf and the 2 shelves. The front plane is not a center plane, it's just a reference for a maximum extent, so it's named accordingly.
Next, select each of your planes and turn them into cutouts. The thickness should be set to =VarSet.Wood_thickness for each of them. We don't have an outline sketch yet so you can leave that unset.
Once you've done this for the 5 planes that we'll have wood at, your 3D view will start to look pretty trippy since all your planes will have been tripled. You may also want to rename the generated planes at this point, because the default "Front"/"Back" names are hard to interpret in 3D space.
Now let's start making real pieces. Our plan is to have two legs on each of the side planes, and one backing piece. We'll start with the back legs. Select the right center plane (or any plane parallel to it, the Z-offset doesn't matter to ShaperCutout objects), and create a sketch attached to it.
Using the External Geometry tool (keyboard: G-X) we can add the top plane of our top cutout, and the back plane of our back cutout, and then we can just constrain our rectangle to those things (and the origin which I'm using as the "floor" of the shelf).
We do need to set the width, which I simply hardcoded here, but for a serious project you should add these things to the VarSet. Once the sketch is done, drag it onto the Left_sheet cutout object. It will move under the Left_sheet object in the Tree View, and the Left_sheet object will now render as a rectangular cutout in the 3D view.
Next, drag the same sketch onto Right_sheet. It won't be moved out of the left sheet (to do that you need to double-click on Left_sheet and remove the sketch in the object editor). Instead, the same sketch will appear under both sheets.
This is what we want, because these two legs should be identical, but we need to be careful! Any edits made to the sketch will be applied to both legs, and if you delete the sketch, it will be deleted from both legs.
Once you've done this, you'll have two legs in the 3D view.
Nice. Let's cut some dados into them so that the shelves can slot into. To do this, again select the Left_sheet center plane (or any parallel plane that's convenient) and create a new sketch. This time we just need to add the center planes of the shelves as External Geometry and draw two lines on them. We don't need to draw rectangles, set width, constrain symmetry, remember to add tolerance, etc.
In my sketch I've "overshot" the edges of the leg so that when I cut this with the Shaper I won't have rounded corners to chisel out.
Next, I drag the dado sketch onto my left leg cutout. Because the cutout already has an outline sketch, this time a dialog pops up asking me what to do.
We click the first button, which opens a "Create Dados" dialog. The sketch list has the sketch we dragged onto the cutout. The numeric fields we fill in with data from our VerSet.
If we'd wanted, we can add multiple sketches to this dado set. We can also have multiple dado sets, if we wanted to set a different depth or autodrill policy.
Before moving on, let's demonstrate the autodriller. We don't have a dialog yet, but by editing properties in the Property Editor, we can add screw holes to our dados. For projects where we don't want to glue, and don't mind visible screws, this provides precisely spaced screw holes in your dados.
In the same way, create a second dado set with a vertical line that the back panel can fit into. Then drag both dado sketches (not the outline sketches!) from one side sheet to the other to create symmetric dados on the other side.
Now that we have our side dados cut, and dado planes automatically created by the workbench, we can draw our backing sketch. We add the top shelf's top plane, the bottom shelf's bottom plane, and the two side dado planes as External Geometry.
Next, let's add the front legs. Since the front legs will be on the same plane as our back legs, we do this by selecting one of the front legs and then clicking "Create Shaper Cutout". The dialog will automatically populate with values copied from the other leg (and in fact, these values will be linked -- try varying the thickness and you'll see the original leg change thickness as well! If you don't want this behavior, you need to create a new center plane.)
Repeat the process to draw the legs and add some dados for the shelves, and you're done!
Before continuing to export SVGs for the Shaper, let's go back and edit all our sketches to look cooler and take advantage of the fact that we have a CNC mill. Alternately, you could stop here, switch to the TechDraw workbench, and produce dimensioned drawings you can carry down to the table saw for manual cutting.
Anyway here's what I did:
If you want, you can right-click on the individual cutouts in the Tree View and choose the "Export SVG" option. Since these parts all have dados on only one side, that's the side you want to export. Instead, let's lay them all out on a single giant 8'x4' sketch that we can lay out over a whole sheet of plywood.
Start by clicking "Create SVG Page":
which creates a new SvgPage object.
Double-click on this to see a render of it.
Yikes. All the pieces are on top of each other in the bottom-left corner and we can't tell them apart. This part of the interface needs a lot of work, but for now it's totally usable. To move and rotate the pieces, edit the X/Y and Rotation attributes in the Property Editor:
If the wrong side (i.e. the non-dado side) is showing, check the "Flip" box to flip it over. (If you want to render the same side, but mirrored, check the "Invert" box. This should never be needed for a project like this where we modeled every individual sheet in its final position in the 3D view.)
After a bit of work, and resizing the sheet to match the half-cut sheet of plywood in my garage, I laid everything out to be nonoverlapping.
And we're done! Right-click the SVG Page, choose "Export SVG Page", and take it down to the Shaper.
Here is a hybrid bassinet/rocking chair I made with this workbench.
