One of my use cases for my Shapeoko is adding keyhole slots to an irregular shape sign I make. I have a jig that fits the contour of the signs which has a rectangular bottom left corner for zeroing. The work process is;
1.) Align the keyhole jig with the carved grid on my waste board and secure it.
2.) Place one of my signs to be cut into the jigs and secure it.
3.) Run the keyhole cut program from carbide motion.
The machine will then;
1.) Ask for a bit.
2.) Measure the bit (BitSetter).
3.) Ask for the required speed and power
4.) Do the cut
My question is: Is there a way to circumvent the measuring step of the machine after the first time? By far the most time consuming portion of this workflow is waiting for the machine to prompt for and measure the bit each time. Since there are no bit changes, these steps seem to only be adding time.
I thought I remembered discussion of a change to carbide motion regarding production runs like this somewhere on the forum but I cannot find it.
I was wondering this, but haven’t tested it (Just wanted to get through those jobs with a known good process). I suppose if the last tool offset measured is preserved when this setting is turned off that would work. Can anyone confirm if this is true?
Yes, I have had my bitsetter disabled for a couple months now. I just haven’t had any production jobs with toolchanges in a single file. The bitsetter isn’t even mounted to the machine as it gets in the way of larger jobs & surfacing the spoilboard.
If you are only using 1 tool, then you don’t need the bitsetter. You set your Z zero with the same tool you are cutting with, so no tool offset is required. You just have to reset Z zero when you change tools.
This actually did not occur to me. To make sure I understand the machine/software;
Without a bit setter and no tool change the Z-zero you set is also incorporating the tool offset and therefore there is no reason to ever use the bit setter when jobs only use 1 tool.
Or am I still understanding this incorrectly since the bit setter always measures the tool at the beginning of a job? Maybe when there are no tool changes, but the BitSetter is still enabled, is just not accounted for in software?
Gotcha, so the machine zero is the amount the axis have moved from the limit switches relative to a point specified by the user and offsets are displacements from said zero?
When the bitsetter is enabled, CM will ask you to insert a tool when you initialize, and it will measure it.
It assumes this is the tool you will use to set your Z zero. (whether it’s the first tool you plan to use, or a probe / dowel).
Then it also asks for a toolchange & does a measurement everything it sees an M6 (Toolchange) in the G-code.
If you used your first tool to set the Z zero, then it will measure it twice. Once at initialization, and once at the first M6.
When the bitsetter is disabled, it will not ask you for a toolchange when you initialize. It assumes you will insert a tool and use it to set Z zero, and subsequently cut with the same tool.
If you are disabling the bitsetter, you should output every toolpath to it’s own separate file. And if you use Advanced V-Carve, you should split the file into separate paths. (GcodeSplit - Split gcode files by toolpath)
One caveat: When you disable the bitsetter, you should re-initialize the machine, and/or Clear All Offsets.
Once disabled, Z zero will just be wherever you set it.
Well, the X & Y workpiece zero that you set are “offsets” from the machine zero.
But otherwise on these machines, no. Other offsets might be cutter compensation, transition & rotation offsets, et.al. which GRBL doesn’t support. So there is no reason to be concerned with them.
The easiest way without disabling BitSetter and having to re-enable it and worry about your Z-height being off is to leave it enabled, but pull out the Tool Change command from your program (assuming you have it in gcode format, and not in a Carbide Create file).
Look for M6 T??? in the first couple lines of your program, the ??? corresponds to your tool number. It may also be reversed as T???M6 sometimes. Anyway, remove that it it will never go to the BitSetter. You just need to make sure you have the right tool installed when you initialize the machine. I do this pretty often for simple programs, and especially if I’m making small changes to the programs (ex. trying to run it again to make a pocket slightly bigger). And I’ve also done this to production programs we run on the HDM in the shop. Really the best way to do it IMO.
If you initialize with the BitSetter on and turn it off you need to reinitialize. If you dont it messes with the internal coordinates and for me it produces an air job. So uncheck the BitSetter and power cycle the Shapeoko and you are all set.