So like most people I have a XYZ probe to get my zero. Most of the time I use a 1/8th endmill. Lot of the time I cannot probe again if I wanna use a 1/4 endmill. So I was wondering if someone has made a macro to change the zero to go from a 1/8th endmill to 1/4th.
What software? The software I use (Estlcam) has the option to enter the endmill diameter and edge finder thickness. Although most of the time I just zero at the center of my work piece in my CAM software. For some reason I prefer that most of the time.
If my job needs a tool change, I just make separate files for each tool. (Is that what you're getting at?)
I would just make a second macro for 1/4" since there is no way to store and retrieve the tool diameter within OBControl nor GRBL.
Your probe will be setting workplace co-ordinates zero at the centre of the bit - your cam software allows for the radius of the bit when you define the toolpath. You still need to reset Z zero though. Alex.
Alex he means allowing for probing X and Y with the side of the bit. The probe macro has allowance built into it for the bit diameter so when you change bits you have to change the macro else you get the wrong XY point. or you can create a 2nd macro for an alternate size or you can probe with whatever bit you have and then offset X and Y by the difference between the bit the macro expected and the bit you actually used and reset 0,0
Yes, but he's talking about changing the bit without doing a new probe. So he can change the bit without re-setting work X or Y zero. Still got to deal with Z zero though.
Am I missing something here? There's no reason to probe again to change tools, except to do a G38.2-G43.1 tool length probe if you don't pre-set your tools with clamp collars or toolholders. All the diametral compensation is being done in CAM according to your operation parameters, before the machine is even turned on. You have to measure precisely, because grbl doesn't accept cutter comp codes (though maybe some g-code senders can, I don't know). But there's no reason whatsoever for grbl to care in the slightest about what diameter tool it's pushing. It just goes from programmed point to programmed point. The probe to get G54 is a one-time deal. It tells grbl where your stock is, essentially, which has nothing to do with the diameter of the tool it's using. If you offset it, say, left 1/16" to go from 1/8" to 1/4", all your left-hand shoulders would be in line and all your right-hand shoulders would be 1/8" heavy. Think about the center of the tool tip as your moving XYZ point, everything else is just calculated from there. Even if you're electrically probing with the actual tool and not a probe, the probing routine still takes into account the diameter of that tool so that the zero is set down the actual spindle/tool axis. A different tool still has the same zero point in X and Y. If you're concerned about physically moving an axis whilst unscrewing the collet nut during a G53-M0 programmed stop at the front of the machine, in theory you should be able to just do a quick re-home. G54 is an offset of this, so as long as your limit switches are repeatable, you'll be right back in place, I don't think grbl resets G54-59 upon re-homing. If you keep your steppers energized all the time, that wouldn't be a likely concern. Edit: the weirdest thing about grbl is that it accepts T-numbers 0-255, but you can't give it an M06 to actually trigger the change!
I could be wrong, but that was my reading of the original post. When I first made an xyz probe I made different macros for different tool sizes, then realised that bits were rarely the exact size they said they were. Now I use an (accurate) 1/8" brass rod for X, Y probing, change to the bit I'm going to use and probe Z. Alex. PS I believe grbl remembers wcs even after power off so you should be able to switch everything off, change bit, switch on and re-home without losing your wcs settings.
I haven't figured out what probing technology I'm gonna use for a future gantry-style machine, I may just build a Renishaw-style probe... Only needs to be accurate to a thou or two, so DIY is probably fine. But this method makes the most sense to me. It does; all G54-G59 WCS, G28[.1] and G30[.1] coordinates are stored in EEPROM. Should be able to survive a hard power loss, in theory. Would need to re-probe tool length, though, and re-apply any arbitrary G92 offset, because they aren't stored.
Alright well I guess i'm just making it harder then it needs to be. Before I was thinking it shouldn't matter because cylindricity. But then I was thinking the probing macro was setup for 1/8th in endmill.
The only reason to be concerned would be if it didn't do this: ...But even if it didn't and your 0,0 was off, shifted over by 1/2 bit diameter, you'd still want to machine everything after the first operation with the same XY coordinates, or you'll have some severe offset issues. You don't want X1 to be 1/16" off the edge of the stock and X2 to be 1/8" off the edge of the stock! Your CAM is definitely not anticipating that one.
