Software chain to create this work for the Shapeoko 2
CorelDraw - VCarve Pro – Notepad++ - GRBL Controller – Arduino GRBL 0.8c
- Create art work i.e. Coreldraw, Adobe Illustrator or Inkscape
- Save as DXF
- Open in Cambam or VCarve etc.
- Ensure the settings limit the G-code to 4 decimal places – Very important! Otherwise the Arduino will not be able to process the code, circles become stars and the CNC will behave unpredictably. I did not have to set this in VCarve.
- In VCarve, setup your cutting jobs, profiling, pocketing etc. This job had three tools, a 6mm End Mill, 2mm End Mill & r1 Ball Nose.
- Save each set of jobs according to your tool. You only really want to set your jobs so you use each tool once. I used the post processor set to Anderson(mm) (*.nc) in VCarve
- GRBL 0.8c does not support all of the commands in this file and I have not yet found one that will run through cleanly from VCarve, yet. So edit each job file .nc and at the bottom will be:-
You need to remove G28G…. To M30 to make the file look like this
G0 Z1.000 - Ensure you include this as not to leave any tooling marks on the work.
This will stop the CNC miss behaving at the end of the job and withdraw the tool from the work to the clearance height. In this case 1mm above the work. Which will allow you to use GRBL Controller to move back to the reference point as required. This is a small inconvenience but makes everything reliable. It is all about price/performance!
- Open the edited .nc file in the GRBl Controller, Version 3.6.1 in this case.
- Ensure the correct tool is inserted, I name my files with a Job no., identifiable name and tool required. i.e.:-
1. Initial Clearance 6mm End Mill.nc
2. Word Clearance 2mm End Mill.nc
3. Final Word Job r1 Ball Nose.nc
Make sure you move back to the x0,y0,z0 position, do NOT unplug the stepper motor drivers, this keeps enough pressure to allow the tool to be changed without losing the correct reference point. Lift the Z – Axis up and change the tool, find the new correct Z-Axis zero point reference height using a piece of paper slide test between the tool and the chosen reference point. i.e. known block on the waste board or known height on the work in a location that is away from the final work, or if the work is tight on size in a place that will be removed during cutting to avoid any marks on the final work. You will have a new z location, record it! Make sure you move back to x0, y0, z New position.
Once there click ‘Zero Position’ on the GRBL Controller Screen.
- Check you are about to run the correct job with the correct tool at the correct x0, y0, z0.
- Ensure all the rails and runners are clear of any debris ALL THE TIME.
- Start the work.
- Monitor the job, Ensure the rails and runners are clear of any debris at ALL TIMES! Do not knock the rails or runners when keeping them clean!
A. I have drawn a BIG RED circle on some sticky paper and put it on my CNC laptop over the Z Axis down button on GRBL Controller. Making you think twice before pressing it and ruining the work by accident moving the Z-Axis down instead of the Y-Axis forward!!
B. Keep the rails clean, or have work ruined when the axis’s jump!! X, Y & Z in that order, I have designed and built X guard covers which reduces most of the debris reaching the rails but not all.
C. Use a reliable starting reference point to create your 0,0,0. I have made my own waist board with several reference points to work from. Working to 0.01 mm accuracy. The stepper step size (if I remember correctly TBC when I get back to some CNC’ing) is around 0.0025mm so you want to be at least twice that step size in any work.
D. Upgrade to GRBL 0.9c required for my kit.
E. GRBL 0.9c PWM motor control upgrade to be created.
F. Limit Switch’s upgrade,
G. Reference Point upgrade (limit Switches and some form of Z-Axis as used per industrial CNC’s)