Using G12.1 Milling Mode on a Mazak Integrex

[mattclubb]

Has anyone done milling with G12.1 and the planar G-codes G17 and G19?

I'm trying to run the following code to machine a curved slot on a face with G-codes setup as T32 compatible:

------------------------
T3535.0
G97 S3000 M203
G12.1
G17
G0 Z50. S3000 M8
G98 X37.276 Y53.248
G1 Z5. F250.
X0. Y65.
Z-2.
G2 X65. Y0. R65.
G3 X0. Y65. R65.
G0 Z50.
------------------------

When I upload this onto the machine the program runs but in Toolpath the Y value never leaves Y0.0

If I take the G12.1 out it works but obviously all my X values are radial amounts not diametral.

Does anyone have sample G12.1 milling code that works?
I would be great help.

Thanks very much in advance.

[M-man]

I guess that you should use C(H) instead of Y when you cut in G12.1 mode.. and usually Rapid movements arent allowed during interpolation...
T3535.0
G97 S3000 M203
G0 Z50.C0 S3000 M8
G12.1
G98 X37.276 C53.248
G1 Z5. F10000.
X0. C65.
Z-2.F250
G2 X65. C0. R65.
G3 X0. C65. R65.
G1 Z50.F10000
G13.1



Mabe this should work...

[mattclubb]

Well I tried that and no luck :-(

I've also tried putting the Plane G-code G17 before the G12.1 but that made no difference either.

Mazak say that parameters must be set
P16 Bit 3 to 0
P6 Bit 2 to 1
P10 Bit 3 to 1

But I've checked these and they're all correct too.

Anyone else used this mode before?

[erwin]

Y Axis should not move when you use G12.1

You program X and Y (X is radial, not diametral), machining is done by moving X and C Axis

Try

T3535.0
M201 (Milling Mode)
G97 S3000 M203
G0 C0 (move C-axis to 0 before changing to G12.1)
G12.1
G17
G0 Z50. S3000 M8
G98 X37.276 Y53.248
G1 Z5. F250.
X0. Y65.
Z-2.
G2 X65. Y0. R65.
G3 X0. Y65. R65.
G0 Z50.
G13.1
G0...move Tool away

be careful and dont machine through X0 Y0 because feed of C-Axis will become infinite

[Integrexman]

I am trying to get G12.1 to run on Head1 of a Matrix controled Integrex.
We are geting alarm 1802 "ILLEGAL STARTUP CONDITION G12.1". We have the option number 38 "CYLINDER." It is the only option that sounds like the cylindrical interpolation option on the MT-Pro control.

Here is a sample program that runs on the MT-Pro control. You have to have cylindrical interpolation option on the machine and parameter P16 bit3 to 1.

O00009999()
M1
G109L1
M302
M200
T001001
S5000M203
G53.5
G17 G40
G00C0.0(C needs to be at 0.0 before G12.1)
G12.1
G122.1(so X can be radial)
G00X1.0Z0.0
G01X0.0C1.0F100.
X-1.0C0.0
X0.0C-1.0
X1.0C0.0
G13.1
G28U0W0
M30

What do we need to change to make it run on the Matrix?

[M-man]

Home the c-axis before the interpolation cycle.. Just a thought.

[Integrexman]

We figured it out, there needed to be a G17UH (UH=XC) before the G12.1

O5
(XCZ-G12.1 Matrix)
G109L1
M901
M200
(TOOL 3/8BULL)
T031T032M6
G53.3
G97 G98 S10000 M203 M8
G00 C0.0
G17UH
G12.1
G122.1(put X in radial)
G00 Z0.1875
G00 X-1.0239 C-0.5354
G00 Z0.0281
G01 Z-0.1006 F20.
.
.
G00 X-0.2253 C1.0238 Z0.1875
(Full machining time: 3.08min.)
G13.1
G28 U0. M205 M9 M154
M30

[newguy81]

Just a question, But why would you spend all that time on a simple face slot in G-code that Mazatrol would do very easy. Or am I missing something in the process?

Joe

[Integrexman]

This was just a program to test G12.1 the part we are making had a very complex profile not programable in Mazatrol.

http://integrexmachinist.com/