Machsupport Forum
Mach Discussion => General Mach Discussion => Topic started by: sinkyster on July 13, 2011, 05:03:05 PM
-
Hi all,
I can't seem to find anything on XY rotation for a CNC Plasma Cutter.
I know other controller software can do it, so MACH3 should also be able to do it! When we load a plate on our bed it is not always 100% parallel to the X or Y axis. I want to use a laser (with an offset to the torch tip) to calculate the amount of degrees that the plate is rotated. I figured it to be something like this:
1. Move torch to corner of plate (which should become X0, Y0)
2. Laser shines on the corner and operator press button to say this is the 0,0 coordinate
3. Operator moves torch along the X axis towards the next corner (which might be at an angle of say 5°)
4. Bring laser to exact corner and operator press the button again to tel the machine the current coordinate. (ex X1000, Y20)
5. Now (somehow??) it should know the plate is not parallel to the side and rotate the XY plane by 5°
After the job is cut it should take the XY axis back to normal state.
My research only told me that it might be the G68 code, but I have no idea how to use it! This would save a lot of time in CNC Plasma Cutting!
Any help would be appreciated!
-
Mach does NOT have that function as a normal feature.
Depending on what Z home method you use the G68 MAY or MAY NOT work.
With the G28.1 style Z home(TOM) it will NOT work
With the G31 style Zhome(TOM) it WILL work
(;-) TP
-
uh-oh! I have it on G28.1 at the moment... I wanted to change it to G31 a while ago but didn't have time to sort it out. I understand that you use G31 if you have a Z Limit/Home switch at the top of the Z axis, and another for plate sensing... Correct?
I'll try and figure it out using the G31...and then I'll ask you again! :)
Thnx Terry!
-
You just set your ZhomeTOM switch to be a probe. Then substitute the G31 for the G28.1. Your backoff setting may change a few thou so you may need to reset that value. That will get you running and you will have to change your post to reflect the change .
G68 is really great to have with plasma.
(;-) TP
-
OK. I have changed the machine and PP to use G31, and it works...
Now for the G68... can you please help me to use it?
BTW - why doesn't G68 work with G28.1?
C
-
When Art set up the G68 in Mach he assumed that you should NOT be able to home the machine while in a rotated position ,and he assumed correct for the X and Y axis. But homing the Z would have no effect on the rotated axis, I tried to get it fixed BUT it did not happen(;-) It would be BETTER IF you could use the G28.1 for the Z as it gives you the dual function of home and limit from the same setup. AND allow you to use a probe funtion if needed.
IF you had a seperate Probe feature you could do an auto sheet setup where the probe touched off on the edges of either the X or Y axis and rotated the program to fit the sheet.
Just a thought, (;-) TP
-
To use the G68 function is fairly simple the easy way is to move into position at the point you want to PIVOT the program at(normally at X0Y0) . Then figure out the rotation angle you need.
Then apply the rotation angle from the MDI screen.
NOW THE REALLY WEIRD PART. The machine will cut in the rotated plane BUT it will not JOG in the rotated plain. It jogs in the original machine coord plane.
This also was Art's choice I tried to get it changed as well, no luck. It could have been an option to go either way. It makes it very strange when you have to jog away from a lost arc to clean or change consumables.
But for the most part it IS what it IS and does work. You just have to understand the QUIRKS
(;-) TP
-
It seems rather simple - it makes sense. But how do you implement it in Mach3? Should I run a macro to calculate the angle or how should I do it?
C
-
You can do it a bunch of different ways just depends on what YOU want. It can be done from a macro or a lot of people use a large protractor to get the angle off the table. Some use best guess(;-) to make it fit.
(;-) TP
-
OK. Say I get the angle, how/Where do I put the angle into the software? How do I use the G68 code?
-
IF you have the angle just go to the MDI page and input the angle into the LOCAL SYSTEM ROTATED dro. That will automatically rotate the system for you. IF You first go to the rotation point and then mach will rotated it aound that point .
To undue the rotation just input ZERO into the DRO.
Gcode wise you use the G68 code. You can rotate the system around the current point G68 R45 OR you can rotate the system from a KNOWN point G68 X1 Y1 R45.
(;-) TP