Please Help! - How to use G19 with G12.1 in Mazak Turn Milling Mode

[afrancoc]

Hi!,

I'm working with a Mazak Mill Turn, and although I've worked a lot with G codes I'm new to the Mill turning codes for Mazak.

So, I'm trying to get my postprocessor to work properly but I don't understand the way my machine does the plane interpolation on milling mode.

When I use G17 everything goes great thats because I'm in front of the piece and I don't need to change planes, I start in C0.0. the only thing weird here is that I need to put the speed twice for it to work, once before the G12.1 and a second one after, here is an example:


N1870 G53
(HTA-11A FRESA 0.625)
N1880 G98
N1890 G00 T1100 M08
N1900 G50 S3000
N1910 M202
N1920 M200
N1930 M212
N1940 G97 S1800 M203
N1950 G10 P11 X0.0 Z0.0
N1960 G98 G00 C0.0
N1970 G50 C0.0
N1980 G12.1
N1990 G17
N2000 G00 T1111
N2010 G97 S1800 M203
( )
( )
N2020 G00 X0.456 Y-0.11
N2030 G00 Z0.533
...
N2140 G00 Z2.325
N2150 G13.1
N2160 G28 U0.0 W0.0 T1100 M09 M205
N2170 M202

No idea but this is working if you know a different way to do it I would appreciate it.


But this is my real problem, now I need to make a milling in G19 at C90.0 and 270.0, but everywhere I read you need to be in C0.0 to enter milling mode, I tried it on the machine and no luck the machine didn't moved in Z and it did weird moves in X.... its a really simple machining but I can't make the machine do it... please help!!!!

This is the code:

N5670 G53
(HTA-12B FRESA 6 GRADOS)
N5680 G98
N5690 G00 T1200 M08
N5700 G50 S3000
N5710 M202
N5720 M200
N5730 M212
N5740 G97 S1900 M203
N5750 G10 P12 X0.0 Z0.0
N5760 G98 G00 C90.0
N5770 G50 C0.0
N5780 G12.1
N5790 G19
N5800 G00 T1212
N5810 G97 S1900 M203
( )
( )
N5820 G00 X1.85 Y-1.57
N5830 G00 Z2.1545
N5850 G00 X0.94
N5860 G01 Y1.57
N5880 G00 X1.85
N5900 G40
N5910 G13.1
N5920 G18
N5930 M212
N5940 G98 G00 C270.0
N5950 G50 C0.0
N5960 G97 S1900 M203
N5970 G12.1
N5980 G19
N5990 G00 X1.85 Y-1.57 Z2.1545
N6010 G00 X0.94
N6020 G01 Y1.57
N6040 G00 X1.85
N6050 G13.1
N6060 G28 U0.0 W0.0 T1200 M09 M205
N6070 M202



Thanks!!!

[psychomill]

You can't change planes in G12.1 mode. You need to command your planes before it.

not sure why your spindle needs to be commanded twice....

[afrancoc]

Hi,

Thats what the manual says and that's the problem, I'm changing planes before entering the G12.1 but it doesn't work, not with G19, my piece doesn't move in Z as if a different plane is selected.

I don't know if there should be a different way to change planes than G00 C90.0, if there is, then that probably is my problem but I don't know it.

Thanks!!!

[froggy]

You must designed the plane for G12.1 mode with name of virtual axis
G17 UH
I don't exactly understand what you want to do in G12 mode in G19 plane but try to select
G19 ZH (just before activate G12.1 for me..)

If your mill is vertical mode, you need to use cylindrical interpolation G07 ..

[jimiscnc]

G12.1 applies only to a cutter axis parallel to the machine Z axis. (AKA face drilling) It is software that can translate the C axis motion combined with X axis motion to result in a linear path. To explain another way - it will establish a "virtual" X-Y coordinate system on the face of a part, with part program zero the center of spindle rotation. This coordinate systems corresponds to the C axis degree coordinate system like this:

C0.0 degrees is the X plus direction vector, C90.0 degrees corresponds to the Y plus axis direction vector (except I'm pretty sure you must use letter address "C" instead of Y in this mode only.) It is more funky because I think you still have to program X as diameter units and C (virtual Y) is in radius units. A 1.0" square, starting at C0.0 in the middle of the flat, with program zero being the center of the square, would be:
X1.0 C0
X1.0 C.5
X-1.0 C.5
X-1.0 C-.5
X1.0 C-.5
X1.0 C0.0

So, with an axial milling cut, you can program it just like a round part in a vertical machining center, with program zero being the center of your stationary chuck, after the G12.1 info is in your program. You need to position C0.0 before invoking G12.1, because G12.1 turns whatever the C position is at the time G12.1 is programmed into C0.0 (virtual Y0.0 in G12.1) The above paragraph helps if you are overlaying C degree positioning with G12.1 polar (motion) interpolation.

If your cutter axis is 90 degrees to the machine Z axis, (aka cross drilling) then you want to contour in the Y-Z plane. THIS CAN ONLY BE DONE if you have a full blown real linear Y axis! All Integrex types do, and some Mazak mill-turns also offer REAL Y axis capability.

If you do not have a real Y axis, then a radial (cross) contour milled feature would require another set up, probably a machining center. If your life depended on doing it on the Mazak mill-turn, you could semi finish the turned blank, and mill fixture jaws to grip the part with the axis 90 degrees from the turned axis of the part and use the polar G12.1 capability. Coming in from the side of the part this time.

an explanation I like is to think of a roller lifter in a car engine following the camshaft. think of the cutter as the roller and the cam profile as your workpiece. This up down motion of the lifter is the linear X axis, and the cam rotation is the rotary C axis. The cam profile could be any combination of arcs and straight lines, just like the X-Y on a typical VMC, but using one rotary and one liner axis to get the result, as opposed to the easy to understand two linear axis of the VMC.

The G12.1 is software to afford really easy programming and take more advantage of the axes already there (C and X). Without it, you would have to perform what I would call "interpolation by part program", which means that you have a to calculate a bucket load of X-C polar coordinates that would approximate your milled profile. But, you'd need to calc. a lot of coordinates before you achieved fluid interpolation like motion. (and too many could result in "information bind", which I don't think is very common these days due to the processing speed of modern cnc's)

-jim

PS - I just remembered something - NEVER EVER EVER us a G0 while in G12.1! It will create weird problems. use a high feed rate instead.
Also, the hardest task for G12.1 is simply a straight line on the face that goes from X plus to X minus and crosses the centerline. It will reverse "instantly" when it hits centerline, as it doesn't ever cross over into the real X minus of the machine. (Mazak don't do X minus travel typically) this makes older machines trip out their servos. modern Mazaks, for perhaps the last 5 years, actually fixed this and put in deceleration and microsecond dwells to make the reversal of the C axis and X less severe and more fluid. But you still will get reversal error marks on the side walls.

[Integrexman]

afrancoc

What control is this Matrix? What type of machine is it? If you use G122.1 X can be radial.

G00 C0.0
G17UH
G12.1
G122.1

You can search G12.1 here and find several posts.
integrexmachinist.com community built on miniBB - Search - G12.1