Installing a fixed Touchplate for tool changes
The tool change option bCNC is a great option to use on any CNC setup. GRBL does not support a tool change and any M06 code will generate an error. The reason is the variety of equipment that GRBL can run on and no minimum requirements. They are focused on the controller and code, not the equipment attached to it. bCNC will intercept M06 and run a Tool Change Macro to adjust your Z zero or use the tool offset to maintain an accurate depth of cut.
- A Touchplate - either purchased on eBay or make your own.
- Limit Switches - Your CNC must be able to Home. The Tool Change Macro uses Machine Coordinates (MPos). For information on setting up GRBL Homing refer to https://github.com/gnea/grbl/wiki/Set-up-the-Homing-Cycle
Your touchplate can be installed anywhere on your CNC workspace. My suggestion is to install it on front and right side. That way it is not interfering with where you are placing your work. My touchplate is recessed into my spoil board and the wires are hidden and protected. I simply cut the hole with my CNC.
Once the Touchplate is installed, connect the wires to the probe port on your GRBL control board.
Important!!! - Attach the plate to the probe port and the clip to ground on your controller.
The clip may not be necessary. Spindles are grounded through their wiring, but a ground wire may be needed between the spindle controller ground and the negative DC output of the power supply. You can also ground a router by running a ground wire from the router case to the negative DC output of the power supply you are using. If you are unsure, please have a qualified electrician install it for you.
Some routers/spindles isolate the rotor from the casing which would make the bit not grounded. PLEASE test your motor and setup (bit to ground) with a meter, if your bit is not grounded, a ground clip is required for safe operation.
The setting to change is in the .bCNC configuration file. Your config file is located at $HOME/.bCNC. This overrides the bCNC.ini file. This file can be changed using any text editor or can be accessed in bCNC - CAM tab - config - User File.
The settings we are changing are in the [Probe] section
All settings are based on machine coordinates (After homing) and mm.
- toolchange X, Y, Z are the coordinates of where you want to change the tool.
(Usually front and center)
- toolprobe X, Y are the centered coordinates of the fixed/installed touch plate.
- toolprobe Z is the starting position of probing.
( Formula: [Negative #] Travel distance of Z0 (Home)[no bit installed] to the touchplate minus the length of your longest bit)
- tooldistance is the length of travel before you get a soft limit error.
(Formula: The length of your longest bit plus a couple of mm)
After you make a change - You must restart bCNC. The .bCNC file is only read during startup.
Be careful testing - you don't want to drive a bit through your touchplate. Start with a smaller toolprobe Z and increase if needed
TIP: - If your tool is to close to the touchplate when starting the probing - subtract from toolprobe Z and add the same to tooldistance.
toolprobe Z + tooldistance should not exceed GRBLs max travel distance for Z and should be a little longer than the travel distance of Z0 (Home) to the touchplate.
- Always run calibrate after every zeroing of Z. This is a necessary step!
This captures the difference in height between the new Z0 and the touchplate. - Don't forget to clip your ground clip (if needed) - you will punch holes in the touchplate.
- If your motor is properly grounded - you can change the pause setting to 'Only before probing'
This starts running gcode as soon as the probing is done. - It's possible to change a tool after gcode completes and the start of the next one if using WCS (not TLO). You do not have to zero Z again on the same material.
Dean Moe - 3/20/2020
