C axis clarification?

[Eric S.]

Hello all

 

I have been programming and setting up our HAAS mills for quite some time and now have started to get into some programming for our Lathes with live tooling (we have 2 Pumas and a Mori). I have done some searching for my problems that I have been having with using cutter comp. As far as I can tell from my programming so far and what I have read is you can not use cutter compensation when milling with the C axis using G117. With G112 the only way to get it to work is to draw in the lead in and out so the cutter starts and stops at C0? I find this VERY STRANGE?!?! Is this correct? Are all multi-axis lathes like this? This is not a big deal for simple parts but when things get more complex and tolerances get tighter I can see this being a huge pain in the a$$. It just does not seem right to me that this is just the way it is and if I want to change the size I have to re-post the job. Any explanation to why this is or advice in this subject would be greatly appreciated.

 

Eric

 

p.s Still using MC9.1

[MCFELIX]

eric you can use cutter compesation in polar interpolation G112 i dont know about G117

[Eric S.]

I have only been able to get it to work if the toolpath starts and ends at C0. If not the tool end up making some really oddball moves in all axis.

[crazy^millman]

Eric if you read what it says in the post you must start and end the C axis toolpath at C0 with mastercam. If the machine has a Y axis then you can use mill toolpaths just need to kee pthe Amount of Y axis movement in mind when programming with it.

 

HTH

[Eric S.]

Thanks for the input..our machine do not have a Y axis, but machines that do have a Y axis can use cutter comp with no problems? Guess the boss should have spent the bucks on a good machine. I'm just surprised that it has to be done this way. I would have thought the machine would have been "smart" enough to figure out the cutter comp.

[David Colin]

I'm programming a 5-axis lathe Mazak IntegrexIII and polar interpolation (G12.1) is working perfectly with control compensation. Even if the machine is Y-axis equiped I prefer polar interpolation to avoid out of range with Y-axis (-80mm/+80mm).

 

With polar interpolation the main rule is to reset C-axis to C0 in lathe mode (G13.1 with Mazak) prior to start every contour machining.

 

In mastercam, I draw my toolpath on standard right view. Toolpaths can start anywhere.

[lowboy]

Depends where the post picks up the polar with the comp. My post I can use the lead in and lead out function without constructing any geometry.

[4xxx4]

I'll be working my hardinge T-42 post in the short future and I'll be sure to have a few questions like these as well. I can start anywhere when I program by hand but I'll have to try a few different scenario's to figure out MCX2 and how to make it do it correctly. I think I'll do a file with some cross holes at 0 and an end slot @90 degrees. This should pick up most of the problems.

I understand the problem pretty well and should have some idea where to go when I dive into it.

[Eric S.]

So this is a post issue and not just the way the machines work? I'll have to give some manual programming a try and see if I get the same problems.

 

Thanks

[David Colin]

 

Here is an example working with our Mazak Integrex 200 III. It might helps...

 

quote:

---

( OUTIL - 1 OFFSET - 1 )

( SECO DIA40 )

N10 G17 G53

N20 G28 U0.

N30 G28 V0. W0.

N40 M200

N50 T0101.00

N60 M211

N70 M203 G97 S5570

N80 M212

N90 G0 C0.

(RESET C-AXIS TO C0)

 

N100 M210

N110 M153

N120 G0 Z60.

N130 X156.331 Y0.

(INITIAL POSITION DIAMETER-X)

(Y0. IF MACHINE IS Y-AXIS EQUIPED)

 

N140 G12.1

(POLAR INTERP. CYCLE START GCODE)

 

N150 M211

N160 X44. Y64.605

(START OF CONTOUR TOOLPATH - MCAM RIGHT SIDE VIEW)

(NB: RADIUS-X POST OUTPUT)

(Y-AXIS IS CONSIDERED VIRTUAL)

(THIS POSITION IS = X156.331 IN PREVIOUS LATHE MODE - CONTROLLER CALCULATES C-AXIS MOTION)

 

(MACHINE WILL NOW CALCULATE AND MOVE C-AXIS & X-AXIS TO MATCH TOOLPATH)

N170 Z-49.8

N180 G98 G1 G41 X23. F2674.

N190 Y18.398

N200 X25.463 Y13.879

N210 G2 X29. Y0. I-25.463 J-13.879

N220 X0. Y-29. I-29.

N230 G1 G40 Y-50.

N240 G13.1

(POLAR INTERP. CYCLE END GCODE)

 

N250 G0 X100. Z60. C-90.

(AFTER INTERP. AXISES ARE ALREADY AT X100. C-90)

(SO THIS OUTPUT IS ONLY MAKING A Z-MOTION...)

 

N260 M154

N270 G28 U0. V0.

N280 G28 W0.

N290 M205

N300 T0101.00

N310 M30

---

[Santa Fe]

We have a Mori ZL200 lathe with live tooling and I'm having the same problem when I do contour with cutter compensation on the face of part. The lead in is fine (short line and an arc to prevent marks) and is also inside G112 which is fine but lead out (same short arc and a line) posts after G113 on a polar move with deg/min (instead of interpolation move with in/min).

I asked out MC post writer and he told me to draw the lead in and lead out as I want it and chain the whole thing this will allow MC to cancel the cuttern comp before G113. Also told me that using arcs for lead in and out is a bad practice and it is not recomended.

 

What's funny is that when I manually edit the lead out to be a regular arc interpolation in/min move before the G113 it works fine.

 

I'm sure there should be a better way to go than drawing the path for the lead in and out or to manually edit the program to make it work.

 

Here is a sample of what the post does when I post this toolpath with a short line and arc for lead in and lead out at midpoint in a closed contour:

 

N8(MS-UT 1/8 FLAT EM ROUGH POCKET)

G53 X0.

G53 Z-10.

G0 T0606 ( 1/8 FLAT ENDMILL)

G0 G54 Z.25

X0.

C90.

M08

G97 S4000 M13

Z.1

G28 H0

G50 C0

G98

G112

G1 X0. C0. F10.

Z-.055

X-.51 F15.

X-.5254 C-.0077

X-.5208 C-.01

X.5208

C.0088

X-.5208

C-.01

X-.655 C-.0725

X.655

C.0725

X-.655

C-.0725

X.675 C-.0825

C.0825

X-.675

C-.0825

X.675

Z.045

Z.25

(MS-UT 1/8 FLAT EM FINISH INSIDE CONTOUR OF POCKET)

X.605 C-.02 F100.

Z.1

Z-.055

G41 X.645 F12.

G3 X.685 C0. R.02

G1 C.0875

X-.685

C-.0875

X.685

C0.

C.05

G113 <===here cancels interpolation before time

G3 X.66 C1452.246 R.02 F1671.34 <===here lead out

G1 G40 X.621 C1453.029 F469.71 <===here lead out

G0 Z.25

M09

M05

G28 U0.

G28 W0.

M01

[David Colin]

Why don't you edit your post to output G113 code after the lead-out (after G40 block)?

 

Your lead-in should be correct even if there is weird Z-moves before G41. Your post break lead-in, for my own i prefer standard lead-in with G3 codes.