Programs from Fusion, VCarve and other CAM programs change the tool with M6 (usually together with T2, T3 …). Grbl does not know M6 and would reject the line with error 20. myCNC takes M6 out while sending and stops at that point. What happens then is chosen per machine under Settings → Machine → Tool change (M6).
Four modes
- Guided (default): The machine finishes all lines before the change, switches the spindle off, moves Z all the way up and to the change position. An assistant names the new tool, then measures its length and continues milling.
- Stop only: Spindle off, Z up, then the job waits. You change the bit, set Z yourself (for example with Probe Z in the control window; jogging and macro buttons are available during the change) and press Continue in the job display.
- Ignore: M6 is removed and everything runs with the first bit. Only useful if every change means the same tool.
- Pass through (only with grblHAL that reports tool change): M6 goes unchanged to the controller. It stops by itself (state “Tool”), the job display shows Tool change at the controller, and Continue sends cycle start. How the tool is changed and measured is set in the controller (grblHAL
$341and following). This mode only appears when the connected controller reports “TC” or “ATC” in$I; on another controller the app guides the change.
A change at the very start of the program (before the first move in X or Y, such as T1 M6 in the header of a Fusion file) does not stop: you insert this tool in the milling assistant as usual. The notes in the milling assistant name it, together with all later changes.
In the assistant
- Move out: The app waits until the machine is at rest, switches the spindle off (with a manual spindle it reminds you) and moves Z all the way up, then to the change position.
- Insert bit: The window shows number, name and diameter of the new tool as far as the file names them in comments (tool table from Fusion, VCarve or myCNC). The Z buttons give you more room.
- Measure length: automatically with the fixed length sensor or with the touch plate on the workpiece.
- Continue: Z stays at a safe height, the app restores the program state (units, distance mode, motion mode, feed), starts the spindle as before the change including spin-up time and continues from the line after the change.
Later only closes the window; the job waits, and Tool change … in the job display opens it again. Cancel job ends the job; you can pick it up again with Resume from line.
Fixed length sensor
A length sensor (tool setter, BitSetter) is fixed on the table. Choose Fixed tool length sensor under tool change, home the machine, move the bit a few millimetres above the centre of the sensor and press Save here. The search distance down limits the measuring move.
At the first change the app measures the old tool as reference, after inserting the new one. It applies the length difference to the Z zero; the already milled workpiece is not probed again. The reference holds until you set Z by hand. Measuring uses G38.3: if the sensor finds no contact there is no alarm and the job keeps waiting.
Tool table
Under Settings → Machine → Tool table myCNC keeps the tools of each machine with T number, name, diameter and the length measured at the length sensor, with the date. The length is the machine Z at which the tool touches the sensor; the difference between two tools is their length difference. Every measurement at the sensor (including the reference measurement of the old tool) enters the length; name and diameter come from the file. You can add, edit and remove rows or take over the tools of the file with From the loaded program.
If the lengths of the old and the new tool are both in the table at a change, the app sets Z zero without measuring again: the assistant shows the difference from the table, and after Bit is inserted it continues right away. This only applies if the tool has not been re-clamped since it was measured (fixed tool holder, quick change). If the bit sits at a different depth in the collet, tick Measure at the sensor anyway. If you save the sensor at a different place, the app clears the measured lengths.
Touch plate on the workpiece
Without a sensor you probe Z again with the touch plate, as described under Probing Z. Surface is at Z is the height of the spot where the plate lies: 0 if Z0 is on top of the material; with Z0 at the bottom, the material thickness. If the plate lies on an already milled face, enter its height. Continue without measuring is only right if Z already fits the new tool.
Change position
Without your own setting the app changes at the park position, without a park position in place with Z all the way up. Save change position here stores the current position (after homing) in the machine profile, for example front centre where you can reach the collet easily.
Own projects with several bits
If a project has several bits, myCNC computes one program per bit. In the Mill window, All bits in one program combines them into one job: a tool table at the top and T<n> M6 before every further bit. This is not available for large workpieces in sections or several workpieces; there it stays one program per bit.
Resume and interruption
When you resume from a line, the dialog names the tool that must be inserted from that line. If a change lies between the chosen line and the next move, resuming starts after the change. Later changes stop as usual. If a job breaks off during a change (page reloaded, connection lost), the dialog Milling job interrupted points it out: check which bit is inserted and measure Z again.