Objects are moved to the zero position of the machine?

[Roelli]

Hi there.

I have a small problem with the zero point of the machine.
When saving a drawing from vcarve with the Datron PP everything seems to be fine.
But when using the G-Code PP the text will be moved to the zero position of the machine, but I don't want it to be moved!

While its working with the Datron PP I guess its a problem with the G-Code PP?

There is a pdf with sceenshots attached to this posting.

What can I do?

Thanks!

Roelli.

[ssflyer]

If the Datron PP works fine, why do you want to use the G-Code PP?

[Roelli]

If the Datron PP works fine, why do you want to use the G-Code PP?

Because the Datron PP does only work on my Datron Machine.

But I have another Machine, which doesn't work with the Datron PP. This machine works fine with the G-Code PP, but it doesn't makes sense to me that the drawing is not at the same position on the machine as it is in vcarve.
If I want to make a hole in the middle of a 500x500mm panel the hole is at the bottom left corner instead with this PP. Does this make sense?

I just want to have the vectors at the same position as they are in the vcarve software. (just like with the Datron PP, which I just tried to figure out what the problem is... the problem IS the PP).

Cheers,
Roelli.

[ssflyer]

Hi Roelli,

There should be nothing in the G-Code PP that moves your work. I'd suspect a settting in the CNC control software that is moving it to the 0,0 location.

[Roelli]

Hi Roelli,

There should be nothing in the G-Code PP that moves your work. I'd suspect a settting in the CNC control software that is moving it to the 0,0 location.

I had the same idea. But with the Datron PP the objects don't move to the XY 0,0 position. So I thought it is a problem with the PP. What do you think?

Thanks,
Roelli.

[Leo]

What I would do is output the code for the datron machine using the datron PP

Whatever goes to the other machine would use the proper PP for that machine.

IF there is a problem with scrolling through the long list of pp's - just go to the folder with all the pp's and move them ALL out except the two you need. Don't delete them - just move them to a different folder. Then - you will only have the 2 you need to pick from.

[Adrian]

Look at the co-ordinates of the code produced by the two PP's. They should be the same so if the co-ordinates of the initial plunge into the material are not the same then you know it's the PP at fault.

I'm with Ron though. I seriously doubt it's an issue with the PP. It's going to be a controller setup issue.

[zeeway]

Do you have x/y offsets set (by accident) in your machine control software?

Angie

[Roelli]

Hi guys. Thanks for your time. Iam not good in reading G-code. So here are the outputs of the two PP:

I tried to remove "G00 Z30" and "G00 X0.000 Y0.000" which looks to me like the first move to zero, but the object is still moved to the zero position.

Here's a video:
https://www.youtube.com/watch?v=BrKg9JEFVmE&hd=1

Here is the Datron pp output: (which works)

%
:1248
N20G91G28X0Y0Z0
N30G40G17G80G49
N40T4M6
N50G90G54
N60G43Z20.000H1
N70G0X0.000Y0.000S60000M3
N80G0X26.938Y11.421Z0.600
N90G1Z-0.875F2400.0
N100G1X82.189
N110Y25.908
N120X26.938
N130Y11.421
N140G1Z-1.750
N150G1X82.189
N160Y25.908
N170X26.938
N180Y11.421
N190G1Z-2.625
N200G1X82.189
N210Y25.908
N220X26.938
N230Y11.421
N240G1Z-3.500
N250G1X82.189
N260Y25.908
N270X26.938
N280Y11.421
N290G0Z0.600
N300G28G91Z0
N310G49H0
N320G28X0Y0
N330M30

And here's the G-Code pp (which moved the object to the zero point of the machine mistakenly)

G00 G17 G53
G40 G50 G71
T4 M06 S60000 M03
G00 Z30
G00 X0.000 Y0.000
M08
M09
G0X26.938Y11.421Z0.600
M08
G1Z-0.875F2400.0
M08
G1X82.189
M08
Y25.908
M08
X26.938
M08
Y11.421
M08
G1Z-1.750
M08
G1X82.189
M08
Y25.908
M08
X26.938
M08
Y11.421
M08
G1Z-2.625
M08
G1X82.189
M08
Y25.908
M08
X26.938
M08
Y11.421
M08
G1Z-3.500
M08
G1X82.189
M08
Y25.908
M08
X26.938
M08
Y11.421
M09
G0Z0.600
G0Z20.000
M09
G0X0.000Y0.000
M30

Thanks!

Roelli.

[Roelli]

What I would do is output the code for the datron machine using the datron PP
Whatever goes to the other machine would use the proper PP for that machine.

Yeah... thats what iam doing at the moment.
I moved the not-used PPs to another folder. Just leaving the Datron, HPGL and GCODE PP in the original folder.

Do you have x/y offsets set (by accident) in your machine control software?

I can't see any adjustments for any offset in the machine sofware.
But other than that iam always using G-CODE (DIN ISO). If one PP works fine I think the problem can't be the machine software? Or am I wrong?

Look at the co-ordinates of the code produced by the two PP's. They should be the same so if the co-ordinates of the initial plunge into the material are not the same then you know it's the PP at fault.

I posted the PP output in the previous posting. But Iam not good in reading G-CODE in general. So I don't know what I have to look for.

I'm with Ron though. I seriously doubt it's an issue with the PP. It's going to be a controller setup issue.

Hmm. I think I have to ask the company who writes the machine control software now.

Thanks,
Roelli.

[PaulRowntree]

I can only give a comment based on the main gcode provided ... there is no translation there, the two files refer to the same X,Y,Z positions.

I haven't looked at the details of the top header sections yet.

I am not sure if the two machines have defined different coordinate offsets, which I believe would not show up in the specific GCode files. I don't know why this would change either (cosmic rays?), but the files look the same to me.
Cheers!

[Leo]

Those two G-Code files are certainly different.

The first one actives the work coordinate system G54

The second one does not.

That could be an issue. I am not stating that it IS - I am just saying it could be.

It depends on how you go about setting up the work coordinate system in the machine. It also depends on how the particular machine registers the work coordinate. Many machines can handle G54-G59 as work coordinate systems. Generally, G54 is default.

Work coordinates are a system that offsets the work coordinate system from the machine coordinate system. You could have G54 for one position - then have G55 for an entirely different position. All you need to do to activate any system is to have G54 - or G55 or so on in the gcode program.

I am a manufacturing engineer with decades of experience. I have worked in 7 companies in my career. I have also worked with several Cad, CAM systems and with many many different machines, of various shapes, colors and sizes.

It is NOT at all uncommon to have the SAME part run in different, and similar CNC machines - but the programs will be different. It would be customary to have a single CAD file and run that through different posts to go to the respective machines. Right now, I have 2 Citizen L20 Swiss turn lathes. They "look" the same - but the programs are different.

If you have two different machines - then two different posts would be normal, common and expected.

[Roelli]

Sorry guys and thanks for your help.

You were right, it was a problem with the machine software. The software developer fixed it.
It was just confusing to me because one PP moved the objects, the other not. But if its different because of G54, like Leo said, it could make sense. Now it works.

Thanks to all!

Roelli.