Difference between G68 & G68.2

[BBIGOTON]

Does anyone know what the difference between G68 and G68.2 is?

 

I love these, they're cool.

 

I would like to thank you all for the great advice y'all provide.

[Guest CNC Apps Guy 1]

G68 is Coordinate System Rotation/3D Coordinate Conversion ON.

 

G68.2 is Tilted Work Plane.

 

If you have a FANUC Series 30i/300i/300is manual B-63944EN-2/03 it's on page 172. It's fairly involved to explain. Better off seeing the illustrations.

 

HTH.

[Guest]

quote:

---

Does anyone know what the difference between G68 and G68.2 is?

---

.2

[MMT-USA]

Put simply - Advanced 3+2 programming function that enables a feature based coordinate system shift through multiple table rotations.

 

Comparable functions;

 

- Heidenhain CYCLE19 / PLANE SPATIAL

- Siemens CYCLE800

[Steve@Cimco]

Cimco Edit Pro supports backplot of G68.2 code now. Need some feedback on it if you want to give it a go. Need to make sure we have our Euler angles correct. If you download the latest version and set the backplot control to Fanuc milling and load C:CIMCOCIMCOEdit5SamplesFanuc MillG68.2 cube.nc There is also an STL file of the finished part in the same directory that you can load using Backplot- load STL. We had a couple of reports of STL files looking too big in the backplot window when Windows is set to US region that I hope to get fixed soon. We are also starting to support G43.4/5, Macro B (not system variables) and suprograms.

[Reko]

THREAD HIJACK!!!

 

Hi,

 

Rather than start a new thread, I thought I'd use this one and add to the topic...

 

I have a Fanuc 31i A5 controller and a head-head configuration on a gantry mill.

 

Can I use tilted work plane, G68.2 with an aggregate head (90 degree) for 4-axis work or is TWP only for use with full 5-axis work using both B and C axis?

 

I normally use G18 & G19, but my question is, would G68 or G68.2 work... and would it be better?

 

Any advice is much appreciated.

[crazy^millman]

Reko, that is a very loaded question. There is a lot to consider there. You have it working for 4th axis work. How did you go about setting it up on the machine? How do you have it defined and posting out of Mastercam? When going to 5 axis and the tool is 90 degrees to the normal position care in my opinion would have to be taken since where are the vectors being defined from? Is it being posted with the tool normal or using the aggregate head? You have already gotten to a good place doing 4th axis the care and work you took doing that would be double if going to 5 axis work with a 90 degree head. Comes down to how comfortable you are with the code, the machine doing what you expect and have you given yourself enough fail safes to make sure it is going to do what you are expecting. Years ago we had 5 axis check pins for the operators, but it was good sanity check for the programmer on new programs. We ran it through some basic moves on the aluminum pins. If everything was set correct then they would go from there. Might do the same thing make dummy part to test it on or make sure you have enough clearance to take tests cuts in the air to prove out what you are attempting. Like anything nothing like going all out, but doing it safely and trying to make sure you have done everything you can to not have a crash or scrap part.

[Reko]

Reko, that is a very loaded question.

 

Here is a better question, and I think I know the answer... should I just stick with G18 and G19 and do the 4th axis work using planes?

[crazy^millman]

Yes you know the answer and yes if not expect to run into problems and errors.

[Reko]

Okay, good.

 

Now... next question... what is the preferred method to post to a gantry mill with true 5-axis and a nutating head... spacial or eulean angles?

[robk]

On our 5 axis head-table machines (Integrex e-1060 thru e-1850) my preferred method of programming a RAH is to use G68.

G18 or 19 will work only if you are not tilting your head, but once you do any rotating then you need a way to track the tool.

Here is a code sample from Matrix control (fanuc should be very similar).

 

 

N8 T100.6 M06

#3901 = #4114

M00

(RAH OPERATION)

(MAKE SURE CORRECT TOOL IS IN THE HOLDER)

(MAKE SURE TLO AS WELL AS STICKOUTS ARE SET CORRECTLY)

()

M00

M00

(RAH OPERATION)

(MAKE SURE CORRECT TOOL IS IN THE HOLDER)

(MAKE SURE TLO AS WELL AS STICKOUTS ARE SET CORRECTLY)

M00

G20 G69 G80 G40 G49 G17 G90 G94 G98

G10.9 X0 (SET RAD MODE)

G91 G28 Z0

G91 G28 X0 Y0

G90

()

()

( Tool Name : ENDMILL_1.0_DIA_.197_CR)

()

(N8_FIN_POCKET_1)

()

()

G91 G28 Z0.0

G19

M107 (B AXIS CLAMP)

M210 (C AXIS CLAMP)

M200 (C AXIS CONNECTION)

G90 G00 G53 B-8.

G54.1 P1

C19.3881

G90 G54.1 P1 X18.0654 Y-.7088 B-8.

M19

G97 S2030 M3

G43 X18.0654 Y-.7088 Z25.0 H#3020

G46 X18.0654 D#3020

G68 X0 Y0 Z0 I0 J1 K0 R-8.

Z-5.5958

M08

G0 X28.0654

X34.0654

G93 G1 X34.1239 Y-.6441 F279.234

X34.1766 Y-.5746 Z-5.5957 F279.234

X34.2231 Y-.5008 Z-5.5956 F279.234

X34.2629 Y-.4232 F279.234

X34.2958 Y-.3424 Z-5.5955 F279.234

X34.3216 Y-.259 Z-5.5954 F279.234

X34.3399 Y-.1737 F279.234

X34.3508 Y-.0872 Z-5.5953 F279.234

X34.3541 Y0.0 Z-5.5952 F279.234

C20.0646 F59.291

C20.7411 F59.291

C21.4176 F59.291

C22.0941 F59.291

C22.7706 F59.291

C23.447 F59.291

C23.6162 F237.161

C23.7007 F474.322

C23.743 F948.645

C23.7536 F3794.578

G94 X33.7885 Y-.5657 F24.36

G0 X29.7885

()

X30.0654 Y.7088 C19.8044

Z-5.5958 X34.0654

G93 G1 X34.1239 Y.6441 F279.234

X34.1766 Y.5746 Z-5.5957 F279.234

X34.2231 Y.5008 Z-5.5956 F279.234

.

.

.

[crazy^millman]

Now... next question... what is the preferred method to post to a gantry mill with true 5-axis and a nutating head... spacial or eulean angles?

 

 

To be honest you just lost me there. I got by what the post gives me and which one of those the post is using I could not tell you. Care to explain what the difference is?

[Reko]

On our 5 axis head-table machines (Integrex e-1060 thru e-1850) my preferred method of programming a RAH is to use G68.

G18 or 19 will work only if you are not tilting your head, but once you do any rotating then you need a way to track the tool.

Here is a code sample from Matrix control (fanuc should be very similar).

 

G68 X0 Y0 Z0 I0 J1 K0 R-8.

 

 

Hi Rob, thanks for the response.

 

The G68 is cool and I think I will end up going that way. I got that output from the first version of the post I recieved from my dealer, except it was a double line like this:

 

N160 G68 X0. Y0. Z0. I0. J0. K1. R90.

N170 G68 X0. Y0. Z0. I1. J0. K0. R90.

 

I'll look up what the difference is between the two, but if you can explain the IJK on your G68 line, that'd be cool.

[robk]

IJK represent whichever axis you are rotating about.

This is copied from my manual;

 

 

Programming format

G68 Xx0 Zz0 Yy0 Ii Jj Kk Rr ; ........... Program coordinate system rotation ON

G69 ; ........... Program coordinate system rotation OFF

Xx0 Zz0 Yy0 : Coordinates of the center of rotation

Specify in absolute dimensions the translation of the workpiece origin.

i, j, k : Designation of rotational axis (1: valid, 0: invalid)

I : X-axis

J : Y-axis

K : Z-axis

r : Angle and direction of rotation on the rotational axis

A positive value of angle refers to the left turn when seen from the positive

side of the rotational axis.

[Reko]

To be honest you just lost me there. I got by what the post gives me and which one of those the post is using I could not tell you. Care to explain what the difference is?

 

I wasn't understanding what/why the difference was, but I am getting a better understanding of it.

 

I think I need to go with the Euler angles... here is the response I got from my dealer, which makes more sense the more I read it.

 

"Regarding the changes to the angles output for the nutating head, we have used the spatial angles as shown in the sample file but would like to confirm that this is how the machine physically runs. Since the B-axis is rotating about an axis that is 45 degrees between the X and Z, rotating the B-axis will form a cone rather than a standard arc. Please let me know if these angles work out correctly or if you need physical angles output."

 

So, when I posted the question yesterday, I was still trying to understand... the way that reads, it looks like it is not a choice, but a necessity for the machine I have.

[Reko]

Thanks Rob.