G-code telling machine to return to "Home" position instead of zero point

[cms9094]

Hey guys,

This might be an easy fix, but I exported G-code yesterday using Fusion 360 CAM, and the G-code works just fine. However, after the cut is finished, the machine is returning to it's "home" position (Ref All Home - Mach3) instead of the zero/zero point that I specified in Mach3.

Basically, in Mach3 you can have a custom zero/zero point anywhere on the surface. The tool path that I programed yesterday exported the G-code just fine, but why is it telling the machine to return to "home" instead of my custom zero/zero point?

Is there an easy fix for this?

By the way, I'm using a CNC router. 

[Steinwerks]

Sounds like a post issue. What's the last move in your program? Paste the last few lines if you can.

[cms9094]

G1 X4.5 Z-0.2062
G2 X4.5625 Y-0.5 Z-0.2063 R0.0625
G1 Y-2.5 Z-0.21
Y-4.5 F12.
G2 X4.5 Y-4.5625 R0.0625
G1 X0.5
G2 X0.4375 Y-4.5 R0.0625
G1 Y-0.5
G2 X0.5 Y-0.4375 R0.0625
G1 X4.5
G2 X4.5625 Y-0.5 R0.0625
G1 Y-2.5
G0 Z0.6

M9
G28 G91 Z0.
G28 X0. Y0.
M30

It's using G28, which apparently tells the machine to return to it's reference point. But, isn't the reference point zero/zero and not "home"?

[Laurens-3DTechDraw]

So what do you want? G53? G29?

[Steinwerks]

Semus wrote:
It's using G28, which apparently tells the machine to return to it's reference point. But, isn't the reference point zero/zero and not "home"?

You could try a few hand modifications, replace G28 with G53X0Y0. It's not Mach3, but on the Fadal at work we use G53 for Z0 and the home position before the M2/M30. Both our machines have to start at the reference position when they are turned on for the day, but both have G53 "home" positions for reaching the table from the doors.

Try changing it by hand and re-running your program.

[Steinwerks]

Oh, and a good description of how G28 works. I would have to think that G53 is supported by Mach3.

https://www.cncci.com/resources/tips/how%20g28%20works.htm

[cms9094]

I'll try G53 and see if that works.

[Steinwerks]

Any news here? This should be the last three lines for the test (although you could replace the third with G53 Z0):

G28 G91 Z0;
G53 X0 Y0;
M30;

[tacticalkeychains]

If using Mach 3, look up my Tormach post on the forum, I've cleaned up many of those issues with it. Not able to attach it here right now.

[cadtekk]

I use G54 in Mach3 for toolchanges and home at the end of a run. This is written in my HSM post, and always goes to Z0 first.

N2821 (--- END OF PROGRAM ---)
N2820 G1 Z3.000 F30
N2822 M9 (Coolant Off)
N2823 M5 (Spindle Off)
N2824 G0 G53 Z0 (Machine Coord's)
N2825 G0 G53 X0 Y0 (Machine Coord's)
N2826 G54 (Work Coord's)
N2827 G49 (Cancel Tool Length Offset)
N2828 M30 (All Motors Stop, Rewind)
%

[daniel_lyall]

G28 machine zero

G30 work zero

that's how they work in M3

[atackchris]

I have been asking the exact same thing in the post processor side of the forum

http://camforum.autodesk.com/index.php?topic=6103.0

But what worked for me was getting rid of everything after the m9 - m30 like the example below and it just returns to the corner of your part. Instead of back to machine zero.

M9
G0 X0. Y0.
M30

Chris

[shaka3zulu4]

Hi,

I have a similar issue (somewhat).  when I start a new job on my cnc, after specifying the origin (and the machine would start cutting normally), it goes home and indicates that the job is complete without cutting anything.  this has happened previously and I would simply re-create the file and the gcode and everything would work.  I have tried re-creating the file and generating the gcode several times but always the same results.  I have attached both the fusion and the gcode file.  any idea what I am doing wrong?

[shaka3zulu4]

problem solved!  related to how WCS was setup.