GettingStartedWithOnshape

Variables

Especially when modeling geometry that has specified dimensions, like the board thicknesses for your laser cut parts, it is extremely helpful to first define variables that you can then reference later throughout the design. If you then need to go through and change dimensions because your board is 6mm instead of 1/4", this will make that fix much much easier for you later.

1. The Variable is on the toolbar as "(x)".
2. Define one constant for thick plates (e.g. 1/4"), and one for thin plates (e.g. 1/8").
3. This should look something like this.

Sketch and Extrude The Base

1. Click "Sketch" and start a sketch on the top plane. Alternatively, Shift-s is the shortcut for starting a sketch.
2. Drag a center-point rectangle (Shortcut: r) from the origin.
3. Dimension it to 18x18".
4. The result should look something like this.
5. Accept the sketch, and then click "Extrude" (Shortcut: Shift-e).
6. For "faces and sketch regions, simply choose the sketch itself from the feature tree.
7. For the depth, type in "#plate_thick" to reference the variable you created earlier.

Sketch and Mirror the Sides

1. Start a sketch on the right face of the base you just extruded, and sketch and dimension the outline of the box.
2. Extrude, again selecting the sketch itself as the object. Make sure that the extrusion mode is set to "new" to create a new part, and not "add," which would merge the new extrusion with the base.
3. You should now have two parts that look like this.
4. Choose "mirror" from the toolbar, and mirror the side plate across the right face, again using the "new" option rather than "add."

Sketch and Extrude The Cross Members

You can extrude multiple disjoint regions as part of a single sketch, and they'll all become parts. So for the cross members, we can do everything as a single sketch to define geometry, and then extrude regions from the same sketch in multiple operations.

1. Make a new sketch on the outside face of one of the side plates.
2. Sketch the vertical and horizontal components using corner rectangles (Shortcut: r).
3. For the two pieces along the angled line, sketch a couple of corner rectangles, and select the bottom horizontal line. This should highlight the constraints for that line. Delete the horizontal constraint, and then add a concident constraint between the top line and the edge of the plate.
4. Add equality constraints to the thickness dimensions of all the rectangles, and then dimension one to be #plate_thick.
5. You should have a sketch that looks like this.
6. Extrude non-intersecting plates across the volume, using the "terminate at face" option to go to the outside face of the other side plate. I did the front, back, top spar, and one of the middle spars in one extrude, and the remaining parts in another to end up with this. You'll have to un-hide the sketch after the first extrude to be able to select different regions from it the second time.

Sketch and Extrude Facing Plates

1. These plates will end up covering the insides of the box. For each, sketch and extrude a plate of thickness #plate_thin.
2. Your box should now look something like this.

Add T-Slot Connections for the Facing Plates

We want the facing plates to be removable so you can get at the insides. One way to do this, though by no means the only, is to use bolted edge connections through the facing plates into the edge plates.

1. Select T-Slot Joint from your custom feature toolbar. Select the edge face of the side plate, and set the joint parameters so you get connections where you want them. It may be helpful to hide the facing plates so you can easily select the edges to add the joints on.
2. Repeat for all four edges.

Laser Joint

1. Select the Laser Joint feature from your custom feature toolbar.
2. Select Automatic mode, then drag-select all of the non-facing parts. Enable adaptive pin sizing, and set the limits appropriately. I've found that for most work in ME218/Lab, the other options aren't necessary, but play around with them to get a feel for it. Leave Allowance disabled here to get a nice fit for your parts.

Kerf Compensation

The lasers on campus cut along the centerline. To get nominal-size parts, we'll offset the geometry a little so that everything lines up.

1. Add a Kerf Compensation feature, select the "By Thickness" mode, and enter one of the plate thicknesses you input earlier. I find that for 1/4"/6mm materials, using a kerf of 0.01" and an allowance of 0.001" works well; keep the same allowance and assume a 0.008" kerf for 1/8"/3mm parts. To be extra precise, cut a test square in your material on your laser and measure the kerf.

Export DXFs

1. Before exporting as DXF, measure your actual stock and if necessary update the thickness variables defined at the top of the document. If you've been using those variables everywhere, this should be a really easy way to compensate for odd material thicknesses and get the joints sized so they almost snap-fit (e.g. I find the 1/4" Duron from PRL is usually not quite 1/4" or 6mm).
2. To export a part, simply right-click a face and choose "Export as DXF/DWG..." and download. Since the laser joint is order dependent, symmetric parts will not necessarily have symmetric joints, so export each part individually.

You now have a bunch of DXFs for each individual part. Now we need to lay these out efficiently so that we can make the most of the material when we cut. This operation is called "nesting."

There's a couple solutions here. The easiest , and first thing to try is to use the Onshape Auto Layout feature, but this only gives good results if all of your parts are reasonably close to rectangular.

To use Auto Layout while avoiding CADing duplicates of parts (which is bad practice), do not apply laser joints in the part studios. Create an assembly, insert and pattern all of your parts, and then from the toolbar click "Create Part Studio in Context" (as of this writing, the right-most icon).

In this new part studio, first create a transform feature, choose "copy in place" as the operation type, and select all your parts. Now add any laser joint feature(s), kerf compensation feature(s), and then finally auto layout feature(s) to arrange the parts for cutting.

You will then need to create a 1:1 Drawing, with views cropped to each cut sheet, and export as PDF/DXF. These PDFs will need to be processed in your laser cutter software to reduce line width so the parts are cut and not rastered.

For more complex shapes, you'll need to use an actual nesting solution. SVGnest is a free, open-source solution, but only accepts SVG files. To use this, you'd need to use something to convert your DXF to SVG and then nest. Deepnest is downloadable, and takes DXF input, but costs $5 per saved output (you can mess around with it without exporting as much as you want). NestLeader has a free trial version and takes DXF input, so that's what I've been using.

1. Run the NestProfessor client.
2. Set up the material to have whatever dimensions your laser cutter can handle.
3. Add each DXF file to the parts list at top. If you're cutting multiple copies of identical geometry, you can also increase the quantity here.
4. Hit "Config" and adjust the spacing settings. Note that in the trial version, Part space will be automatically capped at 0.034.
5. Hit execute, and wait for the run to stop.
6. The resulting dialog will show the number of nested parts at top right; make sure everything worked.
7. Look through the sheets and make sure everything looks reasonable; sometimes there's a bug and a part is nested outside the allowed area. Usually this can be fixed by clicking "all results" and choosing a different solution which doesn't have the issue.
8. Highlight each sheet and then hit "Save Sheet" to save the cut file. Note that this includes the outline of the sheet in the file; you may need to use other software to remove this outline so it is not cut. You can then take this output DXF to the laser cutter.