Programming with G68.2 and G43.4 - is this possible?

[Rworthy93]

Hello,

I require some 5 axis simultaneous programming assistance. I am currently using a Fanuc 31i control on an SNK CMV-80S, it has an A axis head and B axis table as it's rotary axes. I wish to use a tilted work plane (G68.2) and rotate the WCS in line with an error I have previously measured and written to a variable. However on the machine we use a G43.4 TCP function and I can't get the 2 commands to work together. I have attempted using a G43 but that doesn't pick the correct tool length. Is it possible to run these commands together without the G43.4 cancelling out the tilted work plane?

Please look at the code below and if anyone can point out my mistake it will be greatly appreciated.

 

G40 G17 G94 G90 G21

G49

G91 G21 Z0

T66109 M06

G90 G54

G68.2 X0. Y353.5 Z0. I0. J0. K#883

G53.1

G43.4  D99 H99

G65<TLCK>M0

M08

M51

S995 M03

G0 X-182.534 Y428.787 A-30. B330.

 

This program will run but it cancels out the G68.2 tilted plane so just runs as nominal part. If I've missed any info please let me know and I'll do what I can to provide it.

 

Thanks all!

 

[Greg Williams]

Yes that sounds correct You cannot run both G68.2 (TWP) and G43.4 (TCP) together but you can have G68.2 and G43 together

[crazy^millman]

2 minutes ago, Greg Williams said:

Yes that sounds correct You cannot run both G68.2 (TWP) and G43.4 (TCP) together but you can have G68.2 and G43 together

Yes sir you called it. G68.2 is the ability to map your coordinates to do 3+2 work and so all the 3 Axis canned cycles and such in that mapped plane. The G43.4 is to do full 5 Axis work. They are 2 totally different things and not meant to work together as they serve to totally different purposes.

[davidfree]

Some kind of problem can also be the rise and that you can make the rectification from the blog of the Epson printer recovery mode that will definitely make you follow about the entire process of the settings and the updates of the printer is to be made and that can solve the coding problem of yours.

[Leon82]

Is the error the location of the workpiece? Because you should be able to indicate and set zero and go. I've done it on our matsuura with a collet block bolted off center.

You can use g54.4 if you have that option. I'm not sure if I used it on a full 5 tool path though.

[Rworthy93]

Thanks guys.

Leon82, yes it is, so I've probed two points and calculated the angle of the error then wish to call upon the #883 where this error is stored. I now want to rotate my datum to suit this angle - I can't do this by the machine axes due to the kinematics and workpiece set-up so need to rotate the datum. If you've got any examples of using G54.4 that would be great.

[Leon82]

[Leon82]

[Leon82]

So you would you want to use the 54. 4 if you have an angle error.

 

With a table table machine. It's possible to try to correct an error that the machine is incapable of rotating to.  You may get over travels or unpredictable machine motion

 

to check if you have the option you can go to your work offset page and use the right soft Arrow key to scroll through past the macro you should see the work setting error button

[jlw™]

In my experience G68.2 accounts for deviation from COR and you can set rotary offsets in G54, etc just like XYZ.  You gotta watch out too as some will let you fire both and then it will just act funny with out alarms.  Mazak, what?  I didn't say that.

[huskermcdoogle]

18 hours ago, jlw™ said:

you can set rotary offsets in G54,

you can set rotary offsets in G54, but you have to be careful of parameter settings as to whether g68.2 and g43.4 will "compensate" for those changes or not.  IIRC there are two ways that it can interpret those differences in the yellow book.

[Leon82]

1 hour ago, huskermcdoogle said:

you can set rotary offsets in G54, but you have to be careful of parameter settings as to whether g68.2 and g43.4 will "compensate" for those changes or not.  IIRC there are two ways that it can interpret those differences in the yellow book.

From what I have experimented with on our AC machines.

C axis offsets are fine.

If a is -90. 5 it stays there at a hundred and eighty degrees also instead of going to 89. 5

 

Using the 54. 4 it will track a axis correctly

 

In the pictures I posted I was making Corrections and in certain orientations it was unable to compensate so I had to remove my correction ,luckily I had enough tolerance to work with

[mike93]

This is what are mazack post puts out if it helps.

G00 G20 G40 G80 G90
G91 G28 Z0.
G28 Y0.
G28 X0.
M46 M43
G28 B0. C0.
N1
G00 G20 G40 G80 G90
T5 M06 ( .375 BALL)
G91 G00 G28 Z0.
G00 G90 G54 G17
B30. C348.
M46 M43
M08
X.5316 Y-.314
S7200 M03
G43.4 H5 X.5316 Y-.314 Z6.
G61.1 P1
G05 P2
Z.6155
X.336 Y-.2725 Z.2691
G94 G01 X.1404 Y-.2309 Z-.0773 F35.
X.1159 Y-.345 C345.8652
--------------------Etc
G05 P0
G64
G49
G91 G28 Z0.
(TOOLPATH - FINISHCTOUR)
(STOCK LEFT ON DRIVE SURFS = .01)
(STOCK LEFT ON CHECK SURFS = .001)
G54 G90
B31.6775 C218.8138
G68.2 X0. Y0. Z0. I308.814 J31.678 K0.
G53.1 P1
M47 M44
X.3391 Y-1.8605 S3333
G43 H5 Z4.
G61.1 P1
G05 P2
Z-1.81
G01 Z-1.84 F3.
-----------------------Etc
G05 P0
G64
Z4.
M09
M05
G69
G91 G28 Z0.

[mike93]

G53.1 P1 ??

This is the only post edit we had to do for are postablety post, we started with no p that is 0, P1 is a b positive solution  p2 is negative, everything has worked perfect sens.

 

[dstryr]

If you are programming at G54 and you have XYZ all set to 1.0 and run a G43.4 your control should adjust your 5 axis simultaneous moves to the correct position based on active work offset