clear pocket milling w/right angle head

Disclaimer: I am an automotive machinist, not a real machinist so cut me some slack! I have a 4 axis VM20 Milltronics that I do block work on. I have to machine a diameter on the rear of a block to accept a crank seal adapter. It's too tall to stand on it's nose and mill in XY so I am using a 90 degree head in the spindle, with block mainline indicated on the X axis. Machining will be done with the tool coming in from the right. I have no programming software, I do programs manually in G code. I utilize the canned programs that came in the machine, interpolation, rigid tapping, peck drilling etc. I made a program to get the tool to interpolate a full circle in YZ using G19/G03 but I really need to use a 1/2" end mill and machine it as though I'm clearing a pocket, including depth moves in X-. In my mind I'm thinking that I just need to change my G17 program to G19 and enter my own step over values, depth of cut increments, etc. Can this be done manually? Thanks.

Once you get your step-over path figured out, just copy and paste your code in G91 with X- steps for the depth.

Rstewart said:

Once you get your step-over path figured out, just copy and paste your code in G91 with X- steps for the depth.

Click to expand...

If you do that ^ make sure you have a G90 at end of program (or where appropriate) to change back to absolute values.

If I’m not missing something, why not use a boring bar on your 90 deg head?
I do this on my rottler all the time.
I have done it on my vmc when my Rottler is busy.
I would find a older version of bobcad or something like it you can get post processors to fit your machine easy , would make life a lot easier and open up your options for custom parts.


Sent from my iPhone using Tapatalk

Thanks for the replies so far. I'm still in the fog so maybe this will help. The first is my generic G17 program, the values are from the last time I used it. The second is the one I made experimenting with interpolating in the YZ plane. Can anyone make some chicken soup out of this chicken shit??
My angle head has ER20 collets so I cannot use my boring tooling, plus this needs to be milled for other reasons.



O0002 (CLEAR POCKET XY ZERO)
M0 (ZERO T13 TO PART)
M0 (PROGRAM STARTS NOW)

G20 G90
N1 G17 G70 G50
M06 T13
M03 S3000
G40 G80 M9 G0
M6
(Conversational File Centurion VII CNC 7.7369p C.F.)
G20 G90
N1 G17 G70 G50
T13
G40 G80 M9 G0
M6
S500 M3
D13 G43 H13
N2 G0 X0.0 Y0.0
G99 F10
P140 = .010
P141 = -.030
P143 = .010
P145 = 10
P144 = -.010
N3 P150 =.425
P522 = 0
P153 = 0
P154 = 0
P155 = .350
G24 V[P144] P199=0 G40 G3
N4 M5
M9
G0 G53 Z[-P262]

----------------------------

O0001 (Y/Z INTERPOLATE)
M0 (PROGRAM STARTS NOW)
G01 G53 G49 G90 Z0.0 F500
G90 G53 X-30.0 Y0.0
M06 T13
G19 G43 G54 G90 G20 G40 G80
M03 S2000
G01 G90 X0.00 Y0.00 F500
Z0.00
G02 Y-1.000 Z0.000 J-.500 K0.00 F15
G02 Y1.000 Z0.000 J.500 K0.00 F15
M28
M05



OK,problem solved. The machine will not clear pocket on anything other than XY using it's conversational program so I just made some moves in progressively larger diameters using G19, then moved in X- after each cycle to reach final depth. Yes, gotta watch those G90/G91 inputs, nothing will get you in trouble faster than getting those wrong!