CNC Router 2D and Vinyl Cutter Workflows

Overview#

A CNC router cuts flat sheet parts with a rotating end mill, so the 2D workflow differs from laser, plasma and waterjet in several ways: the cutter has a physical diameter, there is a spindle speed and chip load, the tool must be plunged into the material, parts must be held down while the tool cuts, and inside corners cannot be sharp. In Fusion you use the Manufacture workspace's milling operations (2D Contour, 2D Pocket, 2D Adaptive Clearing, Drill, Engrave, Face and Chamfer; the exact names and grouping vary by release) rather than the Fabrication cutting 2D Profile used for beam or jet processes.

A vinyl cutter or drag-knife plotter works differently again: it is a vector-in, vector-out device. You export artwork and let the cutter's driver handle registration marks, blade offset and pressure. Fusion's role is to design the vector shapes accurately.

This page covers both: how to turn a flat design into a safe, accurate router job (stock, setup, contour, tabs, ramping, dogbones, order of operations, post) and how to prepare shapes for vinyl, stencils and paper craft.

Where to find it#

• Manufacture workspace, Milling tab (3D/2D), 2D panel: 2D Adaptive Clearing, 2D Pocket, 2D Contour, Face, Slot, Bore, Drill (general list; not re-verified against the help in this pass, the 2D milling strategies are outside this section's scope).
• Setup dialog: Operation type Milling, Orientation, WCS origin, Stock.
• Tool library: end mills (flat, ball, V-bit, compression, down-cut/up-cut) with diameter, flutes, RPM and feed parameters.
• Tabs for router: inside the 2D Contour operation, geometry options for tabs with size and height.
• Machine library and post library: choose the post for your controller (GRBL, Mach3, LinuxCNC, Shapeoko/Carbide, ShopBot, others).
• Vinyl side: Design workspace sketches, Export DXF, or SVG import (Insert SVG) with SVG export done in other tools.

Step by step: router profile cut#

1. Design. Prepare a flat sketch or flat faces for each part. Keep all inside corners at least as large as the bit radius, or add dogbones. Allow for the bit diameter in narrow slots: a 3.175 mm (1/8 in) bit can cut slots no narrower than 3.2 mm.
2. Create the setup. Manufacture, Setup, New Setup, Operation Type Milling. Orientation: Z axis perpendicular to the sheet. Origin: the lower left corner of the stock top, which is standard for sheet work (Z zero at the top of the material; the alternative is the spoilboard). Stock: relative size box with the real sheet dimensions and thickness.
3. Select the tool. From the library choose a flat or compression end mill appropriate for the material, e.g. a 3.175 mm 2-flute up-cut for plywood. Set RPM (for example 16,000 to 20,000 on a trim router), feed rate (1,000 to 2,000 mm/min), plunge rate (a third of feed), and check chip load against the manufacturer chart.
4. Add operations.
   • Drill or Bore small holes if needed.
   • 2D Pocket for any internal recesses.
   • 2D Contour for inside contours (holes and slots larger than the bit), with compensation on the inside to leave the hole at nominal size.
   • 2D Contour for the outside contour last.
5. Contour settings (typical):
   • Compensation side: inside for holes, outside for part outlines (the cutter center path is offset by tool radius; Fusion handles the direction when geometry direction is correct).
   • Multiple depths: enable and set the maximum roughing stepdown (usually half to one tool diameter in wood; 1/3 or less in aluminum).
   • Lead-in/lead-out: arc entries in scrap, or ramping into the material to avoid straight plunges.
   • Leave a final skin at the bottom: cut to 0.1 to 0.3 mm above the spoilboard to avoid cutting into the bed, or cut slightly into a sacrificial spoilboard if your bed is designed for it.
   • Tabs: enable tabs to hold parts. Typical tab sizes: width 4 to 6 mm, height 1.5 to 3 mm in 6 mm plywood; fewer tabs for large parts, at least 3 per part and more for heavy.
6. Climb versus conventional. Fusion allows selection. Climb milling gives better finish on most machines; use conventional if the machine is flexible or grabs.
7. Simulate. Use Stock Simulation to see the remaining material and collisions. Look for tabs, lead-in locations, and gaps between parts.
8. Post process to your controller's flavor. Open the code in a text editor, confirm units and spindle commands, and run a dry-run with the spindle off and Z raised.
9. Work holding. Screws in waste areas, double-sided tape, a vacuum table, or tabs plus clamps. Keep clamps and screws away from the toolpath, and create toolpath boundaries to avoid them. Zero Z carefully on the material top using a touch plate.
10. Cut and finish. Remove tabs with a flush-cut saw, sand edges, and test fit.

Dogbones and inside corners#

A round bit cannot cut a sharp inside corner. For parts with square tabs sliding into square pockets you have two options:

• Dogbone: a circular relief at each corner, centered on the corner or offset along the diagonal, so the square tab corner clears. The dogbone radius should be at least the tool radius, typically tool radius plus 0.05 to 0.1 mm. It leaves visible circular notches on the cut face, which is acceptable for internal joints.
• T-bone: the relief extends along one side of the pocket. Cleaner looking where one side is visible, but it removes more material along the edge.
• Rounded tabs: fillet the outer corners of the mating tab by at least the tool radius. Works well for slots that are cut with the bit and tabs that are rounded.

Autodesk's help consulted documents no dedicated dogbone sketch command. You draw them manually (a circle at each inside corner, extruded or joined into the cut sketch), generate them by script/add-in (several free dogbone add-ins exist; check the Autodesk App Store, and review before installing), or use a smaller bit with rest machining (2D Pocket with rest machining option) to reduce the corner radius. Verify what your version provides.

Router cutting order and strategy#

1. Drill holes first, so the sheet stays firmly held.
2. Cut pockets and internal contours next.
3. Cut small parts before large ones, and the outside outline of each part last.
4. Use tabs on all through-cut parts until the final pass, particularly small ones.
5. For very small parts add a vacuum, sticky tape or larger tabs. A small free piece caught by the bit can break the tool or fly out.

Vinyl cutters, stencils and paper craft#

1. Design. Draw shapes as closed contours, or open paths for pen-style lines. Use stencil-friendly fonts or add bridges to islands in letters (O, A, B, 8, 0). Fusion text (Sketch, Text) can be extruded or exported from the sketch; convert it to curves where available.
2. Minimum feature size. Standard vinyl blades handle details down to about 1 to 2 mm. Fine text under 6 mm height tends to fail or lift when weeded.
3. Export. Save the sketch as DXF (see the export page) or convert to SVG with an external tool. Most vinyl software (Cricut Design Space, Silhouette Studio, Roland CutStudio, Inkscape plugins) imports SVG more reliably than DXF. Check size after import.
4. Mirror. For heat transfer vinyl, mirror the design horizontally in the cutter software before cutting. For regular adhesive vinyl, do not mirror.
5. Blade offset and corners. A drag knife has a blade offset and rounds sharp corners unless the software applies overcut. Add a tiny corner radius or use the cutter's overcut setting.
6. Registration marks. For print-and-cut jobs the cutter software handles registration marks. Fusion is only the shape source.
7. Weeding and transfer. Mirror, cut, weed, apply transfer tape, then apply.

For plotters with pen holders, sketches exported as DXF or SVG with open paths work well. Use single-line fonts for pen plots, since outline fonts generate double lines.

Options reference#

Tips and pitfalls#

Tip: Cut a fit test on the actual router before cutting the whole sheet. Router tolerances depend on bit wear and machine rigidity as much as on settings.

Tip: Use climb cuts for the final profile pass with a 0.1 to 0.2 mm finishing pass to improve dimensional accuracy.

Warning: A router bit, the spindle and the dust all carry safety risks. Wear eye and ear protection, use dust extraction, never leave the machine unattended, and keep hands clear.

Warning: Do not cut through screws or clamps. Set up a no-cut zone and run the simulation including your hold-downs.

Warning: Tab heights that are too small break free and too tall are hard to cut. Test in your material.

Warning: For vinyl, check the DXF scale and avoid overlapping shapes; overlaps cut twice and tear vinyl.

Practice exercise#

Design a 3 mm plywood coaster set: four 90 mm squares with 5 mm corner radius and a 40 x 3 mm slot in each for a stand. Create a router setup with a 3.175 mm flat end mill. Add a 2D Contour for the slot (inside compensation) and a 2D Contour for each outside (outside compensation, tabs of 5 mm width and 1.5 mm height, at least 3 per part). Simulate and post-process. Expected result: the slot cut first, outlines last, tabs shown in simulation, and G-code you can dry-run. Then make a 3 mm stencil of your initials for the vinyl cutter with bridges and export it as DXF.

Related#

• Finger joints, tabs and slots
• Kerf and tolerances
• Exporting DXF and SVG
• Materials and cutting settings