Fanuc tool offset behavior

cdmurphy · Dec 11, 2009

Hello all,
I'm trying to find out if there is any way to change the tool offset behavior of a Fanuc 10M based milling machine. As it is now, every time I command a G43 Hxx, the head instantly moves to correct the position by the offset amount. As you can imagine, this significantly increases the pucker factor when working on this machine. It doesn't matter if I'm in G90 or G91, or whether I also give it a Z value. What I want is for the offset amount to simply shift the coordinate position, or wait until a z move is commanded. I've looked all over the parameter manual for this control, and I can't find anything that seems to address this. There are two parameters, LGT and LWT, #60000 bit 2 and 3 that seem apparently address this, but the manual says they are only for the 10T/11T/12T series of lathe controls. I've tried setting them anyway, but they didn't have any apparent effect.

Anyone know what I'm missing? or is this just not possible on this vintage of control?

Thanks,

Cameron

Heinz R. Putz · Dec 11, 2009

Hello Cameron:
Here is a simple program that should work on any machine with the 10M control.
01000
G90 G80 G40
T1 M6
G54 G0 X1.0 Y1.0S800 M3
G43 H1 Z1.0
G81 X1.0 Y1.0 R.1 Z-.5 F10.0 M8
G80
G91 G28 Z0
G28 X0 Y0
M30

Its one of the programs I have as an example on my website, all the steps ar explained. There are more, take a look.
This program has worked on every 10M I have trained shops on for the last many years.
www.doccnc.com
Heinz.

Dan from Oakland · Dec 11, 2009

Cameron- I think it is just a parameter change, but I'm not near my manuals right now.
Do you have the control manual for a 10 M with the parameter info? I'll take a look and see what I can dig up. Someone else may chime in here with the solution- lots of 10Ms out there. Are you programming a Z position in your g43 line as above? I would try that 1st as Heinz suggested.
Dan

dicer · Dec 11, 2009

This may work too. I have not tried it. The reason it takes off is the GO commands rapid. If you have a rapid override then you can slow it down.
Anytime you call a feed rate you can of course slow it down with the feed rate dial, well that is if it has one, the stinking buttons like HAAS is way to slow.

O1324
G91G28Z0
T2M6
G90G0G54
X0.0Y0.0
S1000M3
G1G43H2Z2.0F20.0 <<<<<< G1 and Feed ???? Maybe
AND ON AND ON

Also it kinda does not make sense to command an H compensation shift before any Z is commanded.
Why? Because of the various values used. Some cases the shift is a plus value, and that would want to
jam the upper limit switch. If its a minus value then it wants to of course move down. That sort of thing may cause more problems, the way it works is just fine.

cdmurphy · Dec 11, 2009

Heinz, thanks for the help, the program works just fine. The problem is that when I do the G43 command, either with or without a Z parameter, the spindle goes to Zxx + Tool Length if I have a Z value defined, or just Z0.0 + tool length if I don't. This isn't so much of a problem, it's when my CAM program thows in a G49 to cancel the offset, that it tries to put the tool through the table. I'm having to retract to at least the tool length to avoid touble, but on some of the longest tools this is difficult. From reading other posts on the subject, it sounds as though on many machines the g43 / g49 commands don't actually result in movement, simply a shifting of coordinates by the tool length. I'm hoping it's possible to make my machine behave similarly.

Thanks,

Cameron

rainman · Dec 11, 2009

I dont know the answer to your question, but you are correct in stating that on a Fanuc (10M, anyway) any time you command G43 Hxx and a Z move the tool length offset realized at the machine will be added, not simply changed. Haas does not do this. It does what you wish, it simply alters the tool length, but does not add to it. G49 cancel (or I believe G28 Zxx also) is the only way(s) to cancel the current offset. I fully understand what your concern is, because Ive seen more than one operator crash a machine by invoking a G43 with one already active.

beege · Dec 11, 2009

My parameter book has param. # 6000, bit #7 (first one on the left):

Tool offset is applied:
0: Even in a block containing no movement command
1: Only in a block containing a movement command

Not sure this is the parameter you need to change, but maybe?

cdmurphy · Dec 11, 2009

Beege, I just tried #6000, bit 7. Unfortunately it doesn't seem to make any difference. From what I can tell from that area of the parameter manual, it looks like what I want is only available on the lathe controls, not for milling. :-( I've played around some more, and I think I will be fine as long as I specify a Z value along with every G49 something like G49Z19.0 will cause it to go to a safe Z value rather than dive for the table.

gw · Dec 11, 2009

Would this work?

O2020
start up code, etc.
G0 G43 Z.1 H1
yada
yada
yada
G0 G43 Z0.0 H0 (to send Z to home position)

This is what I used to use on an old 6M.

GW

jbexplorer · Dec 11, 2009

gw said:
Would this work?

O2020
start up code, etc.
G0 G43 Z.1 H1
yada
yada
yada
G0 G43 Z0.0 H0 (to send Z to home position)

This is what I used to use on an old 6M.

GW

No

G0 G49 Z0.0 H0 (to send Z to home position)

Needshave · Dec 11, 2009

I have always sent the Z to a position when turning on and off the H offset.
example

G00 G90 G43 H1 Z1.

G00 G49 G53 Z0.

Lenebm · Oct 19, 2021

beege said:
My parameter book has param. # 6000, bit #7 (first one on the left):

Tool offset is applied:
0: Even in a block containing no movement command
1: Only in a block containing a movement command

Not sure this is the parameter you need to change, but maybe?

I need to find this parameter for a Fanuc 16TB lathe. I've been through the parameter manual several times and I'm not able to locate it. Anyone remember which one it is, please? On other lathes with Fanuc control I have been able to find it, but not for Fanuc 16TB

Lenebm · Oct 19, 2021

Lenebm said:
I need to find this parameter for a Fanuc 16TB lathe. I've been through the parameter manual several times and I'm not able to locate it. Anyone remember which one it is, please? On other lathes with Fanuc control I have been able to find it, but not for Fanuc 16TB

Sometimes all you need to do is ask for help.

Just after posting this question I did find the paramter. It is the PRM 5002 #6 in case anyone else is having the same issue. I also changed the PRM 5003 #2 to ensure no kollision while running a G28 ref point return in same block as cancelling offset.

Search

Largest Manufacturing Technology Community on the Web

Search

Fanuc tool offset behavior

cdmurphy

Aluminum

Heinz R. Putz

Stainless

Dan from Oakland

Titanium

dicer

Cast Iron

cdmurphy

Aluminum

rainman

Cast Iron

beege

Stainless

cdmurphy

Aluminum

gw

Plastic

jbexplorer

Aluminum

Needshave

Aluminum

Lenebm

Plastic

Lenebm

Plastic

Similar threads