[Claude Boudreau]

I am using the Mach3 (with no tool changer) post processor, with ver.23 on my home made cnc router.
Everything seem to work ok except for an (unspecified failure error on line 2) message . My line 2 reads N02 G53 Z0. From what I was able to find out its to cancel work offsets. Is this a Mach 3 setting causing this error?

I can still run my files by pressing start again.

[dertsap]

g53 is relative to machine zero position , try adding a g0 or g1 to your line
take a look in the mach controller at the g code list , it has a brief description

[Geof]

G49 is the cancel length offset code and G40 is the cancel diameter offset; G53 is the command to use the machine coordinate system. Some of these may not be recognised by your system.

[dertsap]

mach will recognize it , but won't run it without a rapid or feed command , i doubt the necessity of it on a 3 axis machine and it could probably be deleted , my preference is to code it in as my safe zone for fixture clearance when rotating an axis or clearance for tool changes etc

[rwestbr]

Hi, I have mach 3 as well with no tool changer running a X2 converted bench top mill. I use home switches on all 3 axis, G53 Z0 makes my mill go to Z0 in the machine cords which is where the home switch is located (Z0), if you dont have home switches I think you should not use G53 in your post processor.It is called before a manual tool change in my post.

Hope this makes sense and helps....

Robert

[Claude Boudreau]

Hi, I have mach 3 as well with no tool changer running a X2 converted bench top mill. I use home switches on all 3 axis, G53 Z0 makes my mill go to Z0 in the machine cords which is where the home switch is located (Z0), if you dont have home switches I think you should not use G53 in your post processor.It is called before a manual tool change in my post.

Hope this makes sense and helps....

Robert

I seem to have a similar setup,but my z0 is on top of my stock.
The first line of code is a line full of G-command given before the actual job , the second with g53 is a continuation of the first line I think...
I will check on my shop computer tomorrow but I dont think g53 was anywhere else...

[Geof]

.....The first line of code is a line full of G-command given before the actual job , the second with g53 is a continuation of the first line I think....

This makes sense; the second line is not exactly a continuation of the first but has the same purpose, it is a safety line.

The line full of G-codes has things like G20 (or G21) to set inch (or metric) dimensioning, G80 to cancel canned cycles, G49, G40 to cancel all offsets, etc. This is your safety line that makes sure the machine is not going to do somrething you did not expect. The G53 Z0. is telling the machine to take the Z axis back to machine zero; i.e. getting it out of the way of the table moving. It sounds like there was not any G00 in the first line; as dertsap says G53 G00 Z0. should work and it should work with the G00 on the first line.

[rwestbr]

I seem to have a similar setup,but my z0 is on top of my stock.
The first line of code is a line full of G-command given before the actual job , the second with g53 is a continuation of the first line I think...
I will check on my shop computer tomorrow but I dont think g53 was anywhere else...

Its not a part of the first line but can be used to send the machine to any position in the actual machine coordinates (Mach uses 2 different coordinate systems) you or your post specify after the G53, for instance here is my code just before a manual tool change (the G53 Z0 takes my Z to machine coordinates Z 0, which is at the top of the Z travel,then the M06 pauses the machine, I then change the tool and re zero the Z off the part and continue the job.

N5594 G53 Z0. (sends Z to 0 Machine cords before my tool change)

(JOB 1 POCKET)
(FEATURE POCKET)

N5595 T2 M06 (.0312) (ENDMILL ROUGH) (M06 pauses the machine)
N5596 M05
N5597 G90 G54 X4.413 Y1.5388
N5598 G43 H2 Z.1 M08

G53 (Will take any axis to the actual machine cords for the specified axis)for instance at the end of the program you could use G53 Z0 X0 Y0, Basically its sending ZXY to their home positions in actual machine coordinates, the Z0 off the part is the 0 used by the part program (work offset or the cad programs Z0).

IE-I have home switches so before I run my program I hit the reference all home button by the DRO in Mach3,It then runs all 3 axis to their home switches and automatically 0's them out in the machine coordinates, from there I jog to my part and set the top of my part for 0 with the button beside the Z DRO and I also 0 out the X and Y axises on the part (thats the X Y Z 0 in BOBCAD).

Does this make sense?

Robert

[Claude Boudreau]

Its not a part of the first line but can be used to send the machine to any position in the actual machine coordinates (Mach uses 2 different coordinate systems) you or your post specify after the G53, for instance here is my code just before a manual tool change (the G53 Z0 takes my Z to machine coordinates Z 0, which is at the top of the Z travel,then the M06 pauses the machine, I then change the tool and re zero the Z off the part and continue the job.

N5594 G53 Z0. (sends Z to 0 Machine cords before my tool change)

(JOB 1 POCKET)
(FEATURE POCKET)

N5595 T2 M06 (.0312) (ENDMILL ROUGH) (M06 pauses the machine)
N5596 M05
N5597 G90 G54 X4.413 Y1.5388
N5598 G43 H2 Z.1 M08

G53 (Will take any axis to the actual machine cords for the specified axis)for instance at the end of the program you could use G53 Z0 X0 Y0, Basically its sending ZXY to their home positions in actual machine coordinates, the Z0 off the part is the 0 used by the part program (work offset or the cad programs Z0).

IE-I have home switches so before I run my program I hit the reference all home button by the DRO in Mach3,It then runs all 3 axis to their home switches and automatically 0's them out in the machine coordinates, from there I jog to my part and set the top of my part for 0 with the button beside the Z DRO and I also 0 out the X and Y axises on the part (thats the X Y Z 0 in BOBCAD).

Does this make sense?

Robert

I ve check my program today and you are right, my code is using g53 in a similar fashion.
I cant explain it but my error message disapeared after running the file a second time...computer glitch is the easy culprit...thanks everyone