Steps
- Save fin geometry from OpenRocket as PDF.
- File → Print/Export PDF → Only check "Fin Templates" → Save as PDF
- Import PDF into Inkscape.
- Select the fin, and use the keybind CTRL+SHIFT+G to ungroup the fin from the ruler scale part.
- Delete the ruler scale part.
- Verify that the fin is correctly sized.
- Inkscape allows you to measure the outer rectangular perimeter of a part by clicking on it, use this to verify.
- Moving the fin shape nearer to the bottom left of the page will help you later.
- You can also just resize the page to your fin shape by selecting the fin shape and going to "Edit → Resize Page to Selection".
- Save fin as DXF.
- Open FlatCAM.
- Import fin into FlatCAM
- File → Import → DXF as Gerber Object
- Double click on file in tree navigator on left hand side.
- Set tool diameter to the diameter of your end mill (units are mm).
- NOTE: Default units in FlatCAM are mm.
- Click "Generate Isolation Geometry".
- You will see an isolation geometry path follow both the outside and inside of the fin. We only need the outside, so we will need to delete the inside line.
- Navigate to the project tab, right click on the geometry object, and click "edit".
- Select and delete the inner line.
- Now is also a good time to make sure that the fin is positioned close to the origin, you can use the move tool on the right hand side to do this.
- The fin should be just above and to the right of the origin (NOT intersecting the x or y axis).
- If you adjusted the fin location in the Inkscape file earlier this should be fine.
- CTRL+S to save the geometry object.
- Double click on your geometry object.
- Set "Cut Z" to the thickness of your material plus 0.03".
- Make sure to convert this number to mm before you put it into FlatCAM.
- The extra thickness is to account for tolerances of the material and any errors in z levelling.
- Set feedrate and multi depth passes as necessary.
- Feedrates of 90 to 120 mm/min with a depth per pass of 1mm works well for fiberglass.
- Click "Generate CNCJob object".
- Ensure that the path looks good, then click "Save CNC Code".
- Connect to PCB Mill via USB and open up UGS (Universal Gcode Sender).
- Set port, set baud rate to 115200, set firmware to GRBL, and click "Open".
- PCB mill will open in an alarm state, click the "$X" button to release is from this state.
- Attach material to bed of PCB mill, install end mill.
- Various methods to attach material.
- Best known method is blue tape on bottom of material, blue tape on top of PCB mill bed, superglue between. Strong hold and easy removal/cleanup.
- Move end mill to proper X and Y location, Set zeroes by clicking "Reset X Axis" and "Reset Y Axis" respectfully.
- Set z zero position.
- Best known method is to do the "paper trick". Google this if you are unfamiliar.
- The "Reset Z Axis" button will reset it.
- Enter your gcode into UGS using the "Browse" button.
- Activate the spindle by turning the knob on the PCB mill.
- Run your gcode using "Send".
- It is useful to set your z zero to a set position above the material and running your gcode first, to ensure everything runs as expected before you start cutting material.
- Success!
- You will need to vacuum up all that dust after the part has run. The PCB mill has a vacuum built in. Toggle the foot pedal attached to the left of the machine to turn it on/off.