Need help with mill programming!

Hello all,

I’m stuck, I’m trying to machine a profile at an angle on the top surface of a part?

I’ve done this in the past and I cannot for the life of me remember what I did? I remember it was something simple, only a couple of lines of code to do what I needed?

I’ll describe what I’m trying to do the best I can.

I’m starting from the right hand side of the part and cutting a profile in the G18 plane using a 1/4 ball end mill programmed from the center of the ball.

Here’s a picture of the profile;



I programmed an M97 with a loop to machine this profile. I need to be able to shift in X and Y after the profile is cut so I can cut the profile at an angle on the top of the part?

Problem I’m having is, I can get the Y to shift but not in X, now I’m totally lost!

Any one have any ideas how to do this?
I cannot mount the part at angle, I’m machining a pocket between to walls in the part!

I can post the program tomorrow when I get to work!

Any help would be appreciated! I tried calling Gerotech who gave me the info in the past, and they have no idea how to do this now?

Thanks for any help!

Kevin

Hi Kevin,

Let's see what you have for code this far. Post the part of the program you're having trouble with, and we can point you in the right direction. Teach a guy how to fish.

beege said:

Hi Kevin,

Let's see what you have for code this far. Post the part of the program you're having trouble with, and we can point you in the right direction. Teach a guy how to fish.

Click to expand...

Here's the code I have right now.


%
O00165

T17 M06
G00 G90 G18 G54 X0. Y-0.08
S6000 M03
G43 H17 Z1. M08
G00 Z0.1
G01 Z0. F300.
G03 X0.7001 Z-0.4809 R0.75
G01 X0.862
G03 X1.5621 Z0. R0.75
G00 Z1.
M97 P1000 L85
G00 G90 Z1.
M30



N1000
G90 G00 Z0.1
G90 G01 Z0. F300.
G01 Z0.
G03 X0.7001 Z-0.4809 R0.75
G01 X0.862
G03 X1.5621 Z0. R0.75
G00 Z1.
G90 G00 X0.
G91 G00 Y0.005
G91 G00 X0.0006
M99
%

This shifts the start point in Y0.005 before each cut, but the X0.0006 line does nothing, I'm stumped!

Kevin

Your profile needs to be in incremental also. Its programmed to go to those absolute X coords every pass regardless of the X shift amount. That's why Y moves OK but X doesn't.
Also I don't see switch back to G17


O00165

T17 M06
G00 G90 G18 G54 X1.5621 Y-0.08 (position at the end of the profile)
S6000 M03
G43 H17 Z1. M08
G00 Z0.1

M97 P1000 L85
G00 G90 Z1.
M30


N1000
G91 G00 X-1.5621 (shift back to beginning of the profile)
G1 Z-.1
G03 X0.7001 Z-0.4809 R0.75
G01 X0.1619
G03 X.7001 Z.4809 R0.75
G00 Z.1

X.006 Y.005

M99

I don't see a G18 anywhere. A G3 in a G18 plane NEEDS a G18. And don't forget to go back to G17 when you're done.

Booze Daily said:

Your profile needs to be in incremental also. Its programmed to go to those absolute X coords every pass regardless of the X shift amount. That's why Y moves OK but X doesn't.
Also I don't see switch back to G17


O00165

T17 M06
G00 G90 G18 G54 X1.5621 Y-0.08
S6000 M03
G43 H17 Z1. M08
G00 Z0.1

M97 P1000 L85
G00 G90 Z1.
M30


N1000
G91 G00 X-1.5621 (shift back to beginning of the profile)
G1 Z-.1
G03 X0.7001 Z-0.4809 R0.75
G01 X0.1619
G03 X.7001 Z.4809 R0.75
G00 Z.1

X.006 Y.005

M99

Click to expand...

beege said:

I don't see a G18 anywhere. A G3 in a G18 plane NEEDS a G18. And don't forget to go back to G17 when you're done.

Click to expand...

I have G18 in the main program, do I need it in the sub program as well?

Kevin

No you're fine.

O00165

T17 M06
G00 G90 G18 G54 X1.5621 Y-0.08
S6000 M03
G43 H17 Z1. M08
G00 Z0.1

M97 P1000 L85
G00 G90 G17 Z1.
M30

I'm not sure if M30 resets everything back to default so it's good practice to program back to XY plane so your next program doesn't do something goofy.

Here's the updated program and its running fine now!

%
O00166

T18 M06
G00 G90 G18 G54 X1.5621 Y-0.135
S6000 M03
G43 H18 Z1. M08
G00 Z0.1

M97 P1000 L300
G00 G90 Z1.
M30


N1000
G91 G00 X-1.5621 (shift back to beginning of the profile)
G01 Z-0.1 F150.
G03 X0.7001 Z-0.4809 R0.75
G01 X0.1619
G03 X0.7001 Z0.4809 R0.75
G00 Z0.1

X0.0006 Y0.005

M99
%


Thanks everyone for the help!

Kevin