[ranchak]

I have an OT-C control, I have been trying to do a chamfer on the back side of the part. This would be when the tool is traveling in Z- and then moves X+. My machine using the two line G01 move using the K and I words. My problem is I can not get my machine to execute a chamfer on the rear of the part. I was hoping that someone could post the exact g code that their machine runs. I have googled and can not seem to find an example of this. I have tried everything that I can think of, but still no luck. I know that the "I" needs to be -. Any help would be appreciated.

[fordav11]

If you mean on the edge of an under-cut or groove/shoulder the auto-chamfering using I/K only works with a movement that conforms to a single X or Z straight direction AFTER the chamfer. So if you are boring and want a chamfer at the back of the bore going larger your tool movement after the chamfer must be X+ to a larger diameter. Of course with a boring bar that movement is impossible. Or on an OD the movement after the chamfer must be to a smaller X. If you are not using a square grooving tool to do the chamfer that X- straight in movement is impossible too because the tool will rub. You really don't need that B.S. Use G1 X Z; A chamfer is 45 degrees so movement in Z for chamfer is half of X travel distance for chamfer (on diameter).
(example for boring)
G0 X2.2 Z0.1
G1 Z0
X2.0 Z-0.1
Z-2.0
X2.2 Z-2.1
X1.8
G0 Z1.0
etc

if this is not what you want provide more info.....

[ranchak]

fordav11 that's not what I meant. Here is a picture of the part that I am trying to do. I have tried writing the g code as a simple X,Z move and have the move be a 45' cut, but this leaves a slightly rough edge. Using K,I leaves a much nicer finish.

Lines 530-550 are cutting a small .015 chamfer on the .750 diameter of the part as the tools moves from X+ to Z-. I then need to cut the .020 chamfer that is a move from Z- into X-, this is line 560 and 570. This machine will execute this move, but it will not execute line 580, which is just the beginning of turning down the part to the .625" diameter.

[angelw]

fordav11 that's not what I meant. Here is a picture of the part that I am trying to do. I have tried writing the g code as a simple X,Z move and have the move be a 45' cut, but this leaves a slightly rough edge. Using K,I leaves a much nicer finish.

It makes no sense that using I and K for cutting a chamfer will give a better finish than programming in X,Z. The I,K format just invokes a routine within the software that calculates the destination point, the move to that point, whether the control or you does the calculation, is still a linear interpolation move.

Lines 530-550 are cutting a small .015 chamfer on the .750 diameter of the part as the tools moves from X+ to Z-. I then need to cut the .020 chamfer that is a move from Z- into X-, this is line 560 and 570. This machine will execute this move, but it will not execute line 580, which is just the beginning of turning down the part to the .625" diameter.

In your code below
1. you can't cut a chamfer to N560 G01 Z-0.51248 I-0.020 F0.005 when block N550 already has the tool at the Z destination of the chamfer.

2. N560 G01 Z-0.51248 I-0.020 F0.005 describes a 0.020 chamfer, but N570 G01 X0.729 F0.005 is only a 0.10 radial move from the X start point. Accordingly, this X move is in the wrong direction following an I minus chamfer.

Unless you're using TNR compensation at the control, the TNR of the tool needs to be accommodated in your I,K value.

Depending on what the X position of the tool is before the N530 block (it needs to be less than X0.719), deleting the N550 block, and making the N570 move to an X coordinate less than X0.709 will make your code function. Whether it cuts the correct size chamfer is another matter. This will depend on whether TRN comp is being used.

As Ford states in his reply, cut with the BS and just program the chamfer in X and Z.

Regards,

Bill

N530 G01 Z-0.250 F0.005
N540 G01 X0.749 K-0.015 F0.005
N550 G01 Z-0.51248
N560 G01 Z-0.51248 I-0.020 F0.005
N570 G01 X0.729 F0.005
N580 G01 Z-0.685 F0.005

[fordav11]

actually the info I gave you is *exactly* what you want. I just applied it to a bore rather than an OD. But it's the same thing.
In this case do not use I/K for chamfers.
sometimes a machine can give a rougher finish when moving XZ together. you can fix that by putting a slower feedrate on the chamfer line.
the drawing is too incomplete to create a complete program so I can't write you a working example. the chamfers at the back should be done with a grooving tool or something similar. or at the very least with a 35 degrees turning tool.

[ranchak]

Thanks for pointing out that I did not allow enough room for the X move, I changed it to X0.709 and the program worked.

It makes no sense that using I and K for cutting a chamfer will give a better finish than programming in X,Z. The I,K format just invokes a routine within the software that calculates the destination point, the move to that point, whether the control or you does the calculation, is still a linear interpolation move.



In your code below
1. you can't cut a chamfer to N560 G01 Z-0.51248 I-0.020 F0.005 when block N550 already has the tool at the Z destination of the chamfer.

2. N560 G01 Z-0.51248 I-0.020 F0.005 describes a 0.020 chamfer, but N570 G01 X0.729 F0.005 is only a 0.10 radial move from the X start point. Accordingly, this X move is in the wrong direction following an I minus chamfer.

Unless you're using TNR compensation at the control, the TNR of the tool needs to be accommodated in your I,K value.

Depending on what the X position of the tool is before the N530 block (it needs to be less than X0.719), deleting the N550 block, and making the N570 move to an X coordinate less than X0.709 will make your code function. Whether it cuts the correct size chamfer is another matter. This will depend on whether TRN comp is being used.

As Ford states in his reply, cut with the BS and just program the chamfer in X and Z.

Regards,

Bill

N530 G01 Z-0.250 F0.005
N540 G01 X0.749 K-0.015 F0.005
N550 G01 Z-0.51248
N560 G01 Z-0.51248 I-0.020 F0.005
N570 G01 X0.729 F0.005
N580 G01 Z-0.685 F0.005

[ranchak]

I did try using a slower feedrate, but it still gave a ragged edge, thanks again

in this case do not use I/K for chamfers.
sometimes a machine can give a rougher finish when moving XZ together. you can fix that by putting a slower feedrate on the chamfer line.
the drawing is too incomplete to create a complete program so I can't write you a working example. the chamfers at the back should be done with a grooving tool or something similar. or at the very least with a 35 degrees turning tool.

[angelw]

I did try using a slower feedrate, but it still gave a ragged edge, thanks again

Post a listing of your program using X and Z. The I and K Chamfer format will calculate the correct start and finish point of the chamfer based on those addresses. You may not be calculating the X,Z coordinates correctly. As stated in my previous Post, the chamfer move is still the same type of linear interpolation whether via X,Z or using I,K format.

If you do Post your X,Z chamfer program, specify if TNR comp is being used, and if not, the TNR of the tool being used.

Regards,

Bill