Changing G-Code Axis' ?

[cubby]

Fellers, I know I ask a lot of dumb questions. But I learned long ago that if you don't ask the dumb question
you will make DUMB Mistakes.
I have G-Code for a project that has the material to be cut laying sideways on the table.
X= 20 inches
Y= 16 inches.
My home made machine won't cut this like that.
But I can cut Opposite that with X= 16 and Y= 20
Is there anyway to change the G-Code for the size and direction of my machine?
I sure appreciate your Expertise.
Thank You,
cubs

Similar Threads:

• Need Help!- Error code when changing parameters in N C Studios - PLEASE HELP!!!!
• G code for changing axis angle
• Changing post g-code for helical arcs
• Need Help!- How to rotate G-code in the G-code (to simulate 4th and 5th axis) or axis indexing?
• Changing g-code in beginning

[Jim Dawson]

I would rotate the part 90° in the CAM program, then repost the G-code

[cubby]

Thanks Jim,, Not sure if the Cam information is here. Will look. All I have see thus far is the Tap files.

cubs

[Jim Dawson]

OH, you don't have the original drawing to work with? What CAM program do you normally use?

[cubby]

Jim the Only Cam I have is what came with Mach3 called Lazy Cam.
But I looked and See CRV Files. I am downloading Corel Graphics to open them.
They are probably the Cam Files for Vectric Carve.
What Cam software do you use?

cubs

[Jim Dawson]

I normally use Fusion 360 now, but I used to use CamBam for everything. I still use CamBam for quick jobs, very simple to use. CamBam does have a function that will save a .tap tool path to a dxf file. But that is the tool path rather than the drawing so the tool offsets would already be applied, a bit complicated to derive a rotated tool path from that. If you want to attach your .tap file, I'll see what I can do with it. Change the .tap extension to .txt to attach to a post.

It would be possible to exchange your X and Y axis using the ports & pins in your Mach3 config screen, but this might require recalibrating the axes.

[ger21]

You can use G68 to rotate the coordinate system 90°.

[Jim Dawson]

You can use G68 to rotate the coordinate system 90°.

Thank you Gerry, I learned something new today.

[109jb]

G68 is dependent on whether your control system supports it. In LinuxCNC the equivelant would be G10 L2 P1 R90 would rotate the G54 (P1) coordinate system by 90 degrees. P0 would be the currently active work coordinate system.

Other controllers may not support any rotation at all and there are ways around this.

You could go to your machine settings and change which pins control X and Y temporarily, or even save that config so you can go back and forth easily.

I wrote a visual basic program once to do this for a particularly long program I didn't have the CAD/CAM for. As I recall, t replaced X with Y, and Y with X but then also had to change the sign on all the "new" y moves or the part was mirrored. That was a long time ago but that's what I remember.

[mactec54]

You can use G68 to rotate the coordinate system 90°.

G68 by itself is not going to do much, you have to tell it what you want it to do, also some controls won't support a G68

G68 X0 Y0 R90 ( this is the minimum that you will have to use X---- Y---- are your starting point )


G69G80 (At the end of your program you need to add this line to cancel it )


G68 is also incremental moves your program will have to match this G91

[ger21]

G68 X0 Y0 R90 ( this is the minimum that you will have to use X---- Y---- are your starting point )

He's using Mach3, where it's :
G68 A0 B0 R90

G69G80 (At the end of your program you need to add this line to cancel it )

All you need is G69 in Mach3.

G68 is also incremental moves your program will have to match this G91

Not according to the Mach3 manual.

[mactec54]

He's using Mach3, where it's :
G68 A0 B0 R90



All you need is G69 in Mach3.



Not according to the Mach3 manual.

With Mach3 anything is possible

A0 is normally used for 4th axes rotation

In Mach4 they have changed it to work the correct way using X and Y