C-Axis orientation problem

We have a HAAS SL-20 with full C-axis,live tooling et. al.
I'm trying to program a part that has 3 holes in the face
on a 1.75 dia. B/C. One hole at M19 R0, and one hole 77
degrees either side.This worked fine. The problem is that
there is a flat 180 opposite of hole 0.I used the G77
flatting cycle with I180. The flat comes out somwhere
around 90 degrees from hole 0.
This is my first attempt at something like this.So far we
have only used this machine for bolt circles on the face
and around the OD of parts.
What am I doing wrong?

Ford

Ford,

With a C axis use M154 C0., C77. C283. to position holes to mill flat use G112 instead off G77 you will have much more control over the feed rate: Also remember that C0. is at 3 O'clock.

T909 (1/2 ENDMILL)
G54 G98
M133 P2000 (engage live tooling)
M154 (engage C axis)
M08
G00 X0.475 Z0.1
X0.
G112 (Cartesian to polar on)
G01 X-0.65 Y0.8 F250. (Move off part)
G01 Z-0.485 (Go to Z depth)
G01 Y0.75 F10. (Left to right feed)

etc
etc

Andrew

Cool!!

Makes more sense now,I really appreciate it. I guess I thought that it all came
from a common reference, sucks being self taught.

Got Ammo now, thank you

Ford

yeah dont think of spindle orientation as anything that YOU can use..... io tried to indicate the live tooling on my hass with that and was having issues till the tech told me forget it....it isnt very accurate. Basically he told me spindle orientation is for threading type stuff.

if you want precise location and orientation, you have to use C-axis via M154 with a programed degree orientation. Dont forget the feed rate for any C axis rotation.

my program to check the runnout on my live tooling went like this

G98
G01 Z-4. F10.
M154
G00 C0.
G98
G01 Z-5. F10.
M133 P500
G04 P5
Z-5.
G00 C180.
G01 Z-5.
G04 P5
G00 Z-4.
M155
M99

i HAD TO USE A MIRROR TO LOOK AT THE INDICATOR UPSIDE DOWN THAT IS WHY I REPEATED THE PROGRAM OVER AND OVER.
ok caps are off now. ha ha

good luck

bob

Thanks guys. I wrote all of this down. astorck, you got me going
on this and I appreciate it. I'm the only "real" G-code programmer
here(finger cam). We also have a regular SL-20 and a VF-3 with
fourth axis, all running on my programs, all the other CNC's are old
Hurcos.

We got bought out by a very large co. and have a CAM system
coming. As I was fighting this problem on monday a brand new
Mazak Integrex was being skated into the shop. I think I'm going to
roll my box over to the manual lathe dept. and lay low.

Thanks again, Ford

I have use spindle orientation with very good success.


You do have to lock it, or even a small drill will over power it, but it does orient accurately.

MAKR.....when I just used spindle orientation and spindle lock rotation 180 degrees in between measurements...the live tooling I was using showed to be .029" TIR

but when i subsequently went to using M154 and C0 and C180...the TIR dropped to .006" TIR

you know when the indicator starts to rotate with the spindle it ramps up pretty fast.

so I THOUGHT I was rotation 180...but I am sure it wasnt..............

dont know how far it was off.....

the tip comes from the tech trying to troubleshoot my live tooling woes.

bob

It may sound redundant, but I've had issues where I thought the C axis on my Haas and my Mazak wouldn't position properly or consistently.

I made a mark aligned with the part and a chuck jaw and found the part was creeping under heavy cuts making it appear to be a psotitioning issue, when it was in reality a clamping or holding the part issue.

Just something to check so you don't feel silly later on.

Stu