Tricopter Base Plate
This page serves as a tutorial on how to get the MyDIYCNC machine up and running, and cutting a Tricopter base plate out of standard FR4 material.
- 3D/2D CAD Program of Your Choice
- HeeksCNC 0.17.2 Open Source CAD/CAM Program
- LinuxCNC Machine Controller
- Assembled MyDIYCNC (Optional: w/Limit Switches)
- 3/64" 4-Flute End Mill
- Windows PC to run HeeksCNC/Your CAD Program
- Linux PC with Parallel Port to run LinuxCNC
- MDF or similar Spoil Board
- Double Sided Tape
- FR4 or G10, 6x6", 1.6mm thick
Making the Base Plate
I prefer to use Autodesk Inventor Professional 2012. A student version can be obtained for free from Autodesk's website: http://students.autodesk.com/ Step 1 is to create a base sketch. I used the Delrin Tricopter Kit to size and position holes and the structure. Creating and dimensioning sketches is the primary way of creating 3D features in Autodesk Inventor. Once you have created the base sketch, you can extrude the sketch into a 3D plate. I used 2.35mm as the thickness to match the thickness of the original Delrin plastic. Now a 3D shape has been created, features such as fillets can be added to smooth out the edges of the plate. This is done as an improvement of the original design, which had many sharp (90°) corners, which concentrated stress in crashes and led to cracks that destroyed the original base plate. The finished base plate design is shown below.
Here is a timelapse video of the MyDIYCNC machine in action.
Once the base plate is designed, a 2D sketch can be exported by right clicking the face and selecting "Export Face as...". Save the file as "base_plate.dxf".
Creating a Toolpath
Importing a Sketch
Now we can use HeeksCNC to perform the CAM portion of the project. Import "base_plate.dxf". My copy of HeeksCNC did not import the sketch correctly and was missing a hole near the bottom of the plate. This was easily fixed by selecting the adjacent hole under "ENTITIES 0", and copying it. You can then paste the duplicate hole into the sketch by selecting "ENTITIES 0" and selecting "Paste Into". Select the newly duplicated hole and change the X value to 5.5. Now our sketch is properly imported into HeeksCNC.
Setting up Machine Parameters
Now we need to set up HeeksCNC for our machine, in this case the MyDIYCNC. First, remove the unneccesary tools in the Objects window by right clicking them and selecting "Delete Marked Items". Select the remaining tool and modify its parameters to match the end mill you will use.
Next, we need to create the profile milling operation. Do this by selecting the sketch, and going to Machining -> Add New Milling Operation -> Profile... You should see Operations -> Profile added in the Objects window. Now we need to configure the Profile operation to match our machine's feed rates. We need to change "roll radius" to 0 to prevent any unnecessary material being cut. The final depth should be modified to match our material's thickness; in this case 1.6mm. We will select a "step down" height of 0.8mm to cut the material in 2 passes. The horizontal and vertical feed rates need to be greatly reduced to accomodate the spindle of the MyDIYCNC. I am using a horizontal feed rate of 12mm/min and vertical feed of 25mm/min.
Finally, we need to add holding tags to prevent the part from falling out or getting thrown by the bit as it is cut away from the raw material. This can be done under Profile -> Tags -> Add Tag. Create two tags, and position them at the top and bottom of the part by right clicking on the tag and selecting "Pick position". You will also need to change the tag height to 0.3mm. Now we are ready to create the toolpath. This is done by selecting Machining -> Make Python Script, then Machining -> Run Python Script. The toolpath should be created and will show up as green and red lines in the main window. For this sketch, the toolpath generated is on the wrong side of the sketch profile, so we need to change "tool on side" in Profile to "Inside or Right". Now re-run "Make Python Script" and "Run Python Script". The final toolpath should be shown in the window.
Now that we have a toolpath, we can save the GCode so we can run the job in LinuxCNC. Do this by going to Machining -> Save NC File. Name the file "base_plate.ngc". Open the file in notepad and remove the first line, "O123 (Test Program)", as it will cause an error in LinuxCNC.
Running the Job
Now we have the actual machine instructions, which we will load into LinuxCNC and execute. First, set up LinuxCNC using the stepconf file found here: . This will set up the machine parameters and parallel port signals for the MyDIYCNC. Launch LinuxCNC and disable the E-stop via the far left button on the toolbar, then power the machine. If you do not have home/limit switches installed, then home each axis manually by jogging and clicking "Home Axis" at the limits. Otherwise, click "Home All" and the machine will automatically home all axes. Open the toolpath "base_plate.ngc" and verify the coordinates. Next we need to attach the spoil board and base material to the machine via double sided tape. Once attached, jog the machine to the corner of the material, and bring down the drill head until it touches the starting point of the cut. Click "Touch off" for each axis to select this point as the origin for the toolpath. Now we are ready to begin the job. Do so by clicking the play button on the toolbar. The job should complete in approximately 140 minutes.