What's new
What's new

please help with radius program

ohiomachiner

Plastic
Joined
Jan 10, 2020
Could anyone please help me. I need to program a .141 radius into the face of a part on a haas st10. No Y axis or live tooling. Im using a .125 wide full radius groove insert in a holder that points directly into the face of the part.Im not using tool nose comp or anything fancy. Just line for line programming. I don't have much lathe programming experience. Just have to make 6 parts from 316ss. I know the inside dia of the radius starts at x.185 and out from there I guess .282 to make the .141 rad. Please help me! Any help would be much appreciated. Ive never generated a radius like that.
 
You're probably gunna have to put up a sketch of what you're doing so folks can have a look see. When cutting on the face depending on the depth and diameter you're cutting the radial clearance on top and bottom of the insert is more of a factor than anything. This is a top notch style insert?

Brent
 
Ive never generated a radius like that.

G01 X(startpoint) z(startpoint)
G02 X(endpoint of rad) Z(endpoint of rad) R0.141

The G02 code is a clockwise radius. If you want your tool path to be counterclockwise, use G03 instead. You have to use a little common sense to figure your start and end points. Just make sure the distance between the start z and end z are 0.141. The actual distance between the two x’s should be 0.141 too, but the value would be double if your X axis is diametrical.

If your tool is 1/8” wide you could do it in two passes G02 and G03 and have the passes meet in the middle. It could be done a few different ways. If the radius is critical you need to be using rad comp.
 
If you touch your Tool off on the inside of X. Start at
G0X.177; (.185-.016)
G1 Z0;
G2 X.209 Z0. R.016; (.177+.032)
G1 Z..

This probably won't throw an Alarm, but it also won't generate ideal results. Hopefully you get the most basic principle.

R
 
If you touch your Tool off on the inside of X. Start at
G0X.177; (.185-.016)
G1 Z0;
G2 X.209 Z0. R.016; (.177+.032)
G1 Z..

This probably won't throw an Alarm, but it also won't generate ideal results. Hopefully you get the most basic principle.

R

Hello Rob,
Belated best wishes for the New Year.

Maybe I'm not seeing the OP's part feature as I should, but how do you get the R0.016 Radius. I'm assuming a concave feature of 0.141rad. With a 0.125 wide, full radius tool, the R would be 0.141 - 0.125/2 = 0.0785.

With the tool set as a Type 2 tool (typical boring bar setup) and a 0.141 radius face groove having a small diameter of X0.185, I get the following. The finish pass shows the true positions of the tool.

Regards,

Bill

141rad1.JPG

(0.0625 RADIUS FACE GROOVING TOOL)
(ROUGH CUTS START HERE)
G00 X0.5920 Z0.1250
G01 Z-0.1310
G04 X0.1
G01 Z0.0100
(SEMI FINISH CUT STARTS HERE)
G01 X0.7290
G01 X0.7290 Z-0.0625
G03 X0.4550 I-0.0685 K0.0000 (or G03 X0.4550 R0.0685)
G01 Z0.0100
(FINISH CUT STARTS HERE)
G01 X0.7490
G01 Z-0.0625
G03 X0.4350 I-0.0785 K0.0000 (or G03 X0.4350 R0.0785)
G01 Z0.1250
 
Hello Rob,
Belated best wishes for the New Year.

Maybe I'm not seeing the OP's part feature as I should, but how do you get the R0.016 Radius. I'm assuming a concave feature of 0.141rad. With a 0.125 wide, full radius tool, the R would be 0.141 - 0.125/2 = 0.0785.


Bill, I'd been waiting a long time for this. I thought you were wrong, but I was mistaken. :)

R

.141 is a radius not a diameter.
 








 
Back
Top