Hi guys. I can’t get on with the touchprobe, and a lot of my work is using a 25mm bowl and tray bit. I often have several pieces on the go on the bench at any one time- at different stages. I manually jog machine to corner of my work and zero X&Y to start. If I don’t move across to work on another piece then I change bits and just reset Z and away I go. however if I move to another workpiece, or I lose connection between controller and laptop I have lost the Stored X,Y Zero positions. my question is? How do I record the (grid coordinate??) zero position of the work I’m on, so if/when I have to come back to it and do a bit change, I can guarantee I am starting from exactly same spot. at the moment I jog machine reset it manually if need be, but there is more room for human error like this. I’ve looked to see if I can find a reference when I have hit zero, but no luck. Any thoughts ? thanks
G28.1 will store a position (it's relative to the home position in your machine co-ordinates system) and G28 will move to the position you stored. Be aware that the controller will not know about any obstructions that might be in the way. An alternative approach is to use a different workplace coordinates system for each job. Grbl has 6 workplace co-ordinates systems. What cad-cam software are you using? Most with allow you to set a workplace coordinates system when you create a toolpath/g-code file. Alex. PS, you should not lose a workplace coordinates system zero if you lose contact between PC and controller, but it is a point referenced from the home position so re-homing should re-establish the workplace zero. What controller do you have?
no, you don't since the controller stores the offsets from home, so where ever you 'setZero' after homing will be remembered. This does mean you MUST home every time the controller powers cycles or resets. there are several ways. way 1 hover your mouse over the X Y and Z boxes in CONTROL and the machine coordinate will display in a hint, write that down (when at x0 Y0 z0 of course) and you can get back to that exact offset using G53 moves (raise Z first) then G53 G0 Xxxx Yyyy where xxx and yyy are the numbers you wrote down from the hint boxes That should put the tool over the 0,0 point and now you can jog the Z down till you get to the surface of the work OR to the indicated coordinate. DO NOT use a G53 move to position Z, since you have changed bits you will certainly have a different tool length every time and will crash. way 2 activate the serial console tab in CONTROL type $# and press enter all the offsets will be displayed and you can write them down. Code: [18:59:46] [ $# ] [G54:0.000,0.000,0.000] <------ offset from home to WCS 1 [18:59:46] [ $# ] [G55:0.000,0.000,0.000] <---- offset from home to WCS 2 [18:59:46] [ $# ] [G56:0.000,0.000,0.000] etc [18:59:46] [ $# ] [G57:0.000,0.000,0.000] etc [18:59:46] [ $# ] [G58:0.000,0.000,0.000] [18:59:46] [ $# ] [G59:0.000,0.000,0.000] [18:59:46] [ $# ] [G28:0.000,0.000,0.000] ignore from here down [18:59:46] [ $# ] [G30:-300.000,-300.000,-10.000] [18:59:46] [ $# ] [G92:0.000,0.000,0.000] [18:59:46] [ $# ] [TLO:0.000] Then, you can use the offsets to return to the recorded positions as in way1 way 3 use the other 5 work coordinate systems to store positions. other 5? yes, when we use the setZero buttons we are using G54, the default WCS, but there are 5 more, G55 through G59. say I have 3 work pieces on the table, left to right I jog to the left hand one and I use probe/paper and setZero for that one. that sets the G54 offsets. with the tool at 0,0,0 I select G55 and 'setZero' now select G54 again Now I move to the 2nd part and setZero,, select G56, and setZero again now select G54 again move to 3rd part, probe, setZero, select G57, setZero. now I have the offsets for the 3 parts saved in the controller under G55 G56 G57 and can go back there and set G54 to those values at any time in the future. NOTE: your Gcode includes G54 to select that WCS, and yes you could change the gcode to use different WCS offsets. You can select a different WCS in the CAM, or just edit the Gcode. but remember to put the WCS in the filename so you dont get it wrong.
thanks David. looking at method 1, as that appears the only one within my skill level. I have managed to get the X,Y location prompt to to show, when hovering with mouse, and I can now adjust back to that position manually by nudging if I need to. But how do I send the machine back to that position using G53, I’ve never used the Gcode box on the screen before? thanks Gareth
So, you have written down the Machine co-ordinates for the position you want to return to. In the g-code box type G53 G0 Z -10 (to raise Z to 10 mm below the limit switch) Then type G53 G0 Xnnn Ynnn (to move X and Y to the positions you wrote down) Then re-set your Z zero (because you have changed a bit and your Z zero will have changed) Alex.
Now more confused than ever. I had success with writing down the X,Y zero then moving back to it manually after going on to work on another piece- worked perfectly- thought I had it cracked. Now this morning I have tried to go back to a work piece, I jogged the bit to what I thought would be roughly my last zero, then with mouse hover over the X,Y on the screen to see how much I need to jog slightly- this is where problems started. My written down previous zero was X45.97 Y-417.72 but although I am now within a few mm of the original zero position ( workpiece not been moved) the readings displayed on the laptop screen are X-526.37 Y-584.25, I don’t understand I thought the readings were a fixed grid? I also tried following your instruction using gcode to move the bit, but I got an error message. I am happy moving the bit manually for the moment, and will revisit the gcode problem when I have resolved this zero problem. This workpiece is to have resin cleaned out of a bowl, so really important I get the zero back to the original zero position. thanks gareth
Did you constantly remember to Home. All coordinate systems are overlayed offsets from the base coordinate system (Machine Coordinates) set by Homing. Homing before setting other coordinates, and thus rehoming when you want to reference previously set coordinates is very important
Can one of you please explain further? I followed David’s instructions and it worked fine in the week. Now the numbers are out and you say I need to home? I can’t find any reference online to setting home. I got a work piece I can’t complete without getting the bit back to the original zero position. If there are steps that haven’t been listed by David or Alex can one of you pkease explain, thankyou.
Try the "Home" button But if you didn't home consistently you can't really reestablish origin reliably so you might have to scrap the piece. Homing is critical and one of the first things one has to do after turning on the machine, but also after any alarm/error/crash/etc.
@David the swarfer's first comment was about the need to home your machine - that sets the reference point that everything else uses. You might be able to rescue your job if there is still a point on your job that allows you to identify where you set the workplace coordinates system zero, but it is essential to home whenever there's a power cycle or an alarm that tells you the home position may have been lost. Alex.
