G41/42 question

[OCNC]

I'm trying to generate a g-code program that zig-zags. In order to keep the tool on the correct side of the cut I need to change the cutter offset at the end of each zig and zag motion. The change from G41 to G42 and back again seems like it might be happening at maximum rapid speed. What speed is used for the cutter compensation move and is there any strategy that applies to making a smooth transition between G41 and G42?
Thanks.

Chris

[jvangelder]

I could be wrong not seeing exactly what your doing, however

You are going to need a lead for each new movement when you enable cutter comp

Is there any reason you cant program the path without cutter comp, just programming it with the tool center?

-Jacob

[OCNC]

Originally Posted by jvangelder I could be wrong not seeing exactly what your doing, however You are going to need a lead for each new movement when you enable cutter comp Is there any reason you cant program the path without cutter comp, just programming it with the tool center? -Jacob

I could do it by changing the centerline path. I just thought that changing the comp would be simpler. I'm new to working with g-code so wasn't sure which way to approach the problem. What's involved in creating a lead for the comp change?

Thanks.

Chris

[sinha_nsit]

You can change G41 to G42, and vice versa, in compensation mode, but I cannot imagine any practical example of this application. Pl let me know where you are using it

[Algirdas]

I agree with Mr jvangelder and Mr. sinha_nsit. Post Your part sketch or picture here. Can't imagine necessity to change compensation direction without retracting the tool away from cutting point

[OCNC]

Originally Posted by sinha_nsit You can change G41 to G42, and vice versa, in compensation mode, but I cannot imagine any practical example of this application. Pl let me know where you are using it

The shape is the top surface of an airfoil. The chord is in the y direction and the camber or thickness is in the z direction. The span is in the x direction. The cutting path then zig-zags back and forth along the x axis (the same distance on each pass) and y/z vary to get the shape. In other words I'm extruding a profile along x. The cutter always needs to be to the same side of the center path line relative to the x-y plane (rather than relative to the path direction) and therefore the compensation has to change depending on whether the motion along x is + or -. Of course the other way to do this is to shift each alternate path line to reflect the change in compensation but this is, at least it seemd so to me, more complex than just telling the cutter to move to the other side of the centerline. Asking the same question in the Artsoft Mach forum it was pointed out to me that I need to turn off compensation with G40 before I change it from G41 to G42 or vice-versa which I wasn't doing. This may have been causing the behavior I was seeing which was a kind of snapping motion and it's the 'snap' of this motion that I'm trying to eliminate. If this is still unclear I'll post a drawing. I'm generating the code using a script in Rhino with a simple profile curve so there really isn't any significant graphic that would enhance the present description. I appreciate the input.

Chris

[angelw]

Originally Posted by OCNC The shape is the top surface of an airfoil. The chord is in the y direction and the camber or thickness is in the z direction. The span is in the x direction. The cutting path then zig-zags back and forth along the x axis (the same distance on each pass) and y/z vary to get the shape. In other words I'm extruding a profile along x. The cutter always needs to be to the same side of the center path line relative to the x-y plane (rather than relative to the path direction) and therefore the compensation has to change depending on whether the motion along x is + or -. Of course the other way to do this is to shift each alternate path line to reflect the change in compensation but this is, at least it seemd so to me, more complex than just telling the cutter to move to the other side of the centerline. Asking the same question in the Artsoft Mach forum it was pointed out to me that I need to turn off compensation with G40 before I change it from G41 to G42 or vice-versa which I wasn't doing. This may have been causing the behavior I was seeing which was a kind of snapping motion and it's the 'snap' of this motion that I'm trying to eliminate. If this is still unclear I'll post a drawing. I'm generating the code using a script in Rhino with a simple profile curve so there really isn't any significant graphic that would enhance the present description. I appreciate the input. Chris

I imagine that you would be using a ball nose cutter or an end mill with a corner radius to generate your shape. If the generated code gives the true position of the cutter, I can't see any reason in using cutter rad comp; you may have to enlighten us with a picture of the workpiece and cutter arrangement.

If for some reason cutter radius comp is required, and given that your cutting is mono directional, after you lift off at the end of the cut you could apply G40 to cancel the comp on the rapid back to the start point and reapply the cutter radius comp on your Y move to engage the next cut.

Regards,

Bill

[sinha_nsit]

I tried to study the manual, but the logic is not very clear.
But it is clear that you can switch offset mode without canceling it.
I do not know if this would help, but try switching offset mode after YZ-motion at the end.

And, as Angelw has said, if you have generated the profile using a CAM software, what is the need for using radius compensation? Just specify the radius of the tool before toolpath generation, and select its reference point. The software would automatically adjust the cutter path.

[Algirdas]

You have one (the best) advice already. Set Your CAM to generate tool center path. You can't change the cutter to another size nor You can't compensate tool tip wear while cutting. The advantage is, that You will get simple and fast program. Depending on Your control specifications (NURBS, Hi-NURBS or Super Hi-NURBS as for Okuma like instance) You can increase or reduce the speed. One more advantage - You can get perfect surface. Each tool stop makes clearly visible dot, so - no stops no dots.
Another way is to use machine tool provided "three dimensional cutter radius compensation". It's is optional for Your machine, suppose.
The third solution is to use spiral approach instead of zig-zag

[Kiwi]

Originally Posted by OCNC .....I'm generating the code using a script in Rhino with a simple profile curve so there really isn't any significant graphic that would enhance the present description. I appreciate the input......

If you can get your script to generate code as per example this should help.
You will need to reverse the offset when cutting the half when the Z is decreasing.

G40 G01 X-10. Y0. Z10
G42 G01 X0. Y10
G01 X200.
G40 G01 X210.
G41 G01 X200. Y20. Z12
G01 X0.
G40 G01 X-10.

[OCNC]

Originally Posted by Kiwi If you can get your script to generate code as per example this should help. You will need to reverse the offset when cutting the half when the Z is decreasing. G40 G01 X-10. Y0. Z10 G42 G01 X0. Y10 G01 X200. G40 G01 X210. G41 G01 X200. Y20. Z12 G01 X0. G40 G01 X-10.

Thanks. I'll give this a try tomorrow. I can easily modify the script to embed the offset in the path and will probably not use the compensation but I would like to implement it just to see how it works and to get a feel for what's involved in using it. Your example will be a good starting point for me.
Thanks again.
Chris

[Kiwi]

Chris. May be better to put the Z move in a separate line.
G40 G01 X210.
G01 Z12. ;<<<<<<<<<<<<<<<<<<<<<<<<<<<
G41 G01 X200. Y20.