Z-Axis Moving Wrong Way While Running G28, Leadwell VMC with Fanuc OM

[Sage Brush]

Hi All,

I have looked and looked for a thread discussing this. If you know of one I'd be glad to read it.

Machine: Leadwell MCV-OP
Type: VMC, 3-Axis
Year: 1996
Control: Fanuc OM-F

I have been running this old machining center for about a month now and noticed something scary. If I use a POSITIVE tool length off-set and run the following block in a program, the tool moves DOWN the length of the off-set, then rapids up to home.

G91 G28 Z0;

I thought at first it was moving to the mid point for G28. But it is being called in incremental mode and the downward motion is equal to the length of the tool off-set. Up to now I've been using NEGATIVE length off-sets and I see the same thing only the tool moves UP the length of the off-set, then rapids home. I'm worried I will have a crash if I'm not real careful. Is this normal for Fanuc? Maybe a parameter could change this behavior? I would like to have the above G-code only move the tool up.

I had the idea of inserting a rapid up move in front of the G28 block to compensate for the downward motion, but that seems like painting over the problem.

By the way, I am setting all my tools off of a block on the table. Tool 1 is just a reference tool (no cutting edges) that has a length off-set of 0.0". Up till now it was the longest so all other tools had a negative length off-set.

 

[Vancbiker]

You could plug in a G49 to cancel the tool offset.

 

[sinha]

Are you cancelling length offset before G28?

 

[dandrummerman21]

Are you doing this in MDI?

Does it do the same if you have it in a program?

I doubt this is the cause, but what is the contents of parameter 3?

 

[Sage Brush]

You could plug in a G49 to cancel the tool offset.

I thought G28 cancelled the offset. Maybe I missed something?

Are you cancelling length offset before G28?

No, just cutting with the tool, rapid up a little and calling G91 G28... At any rate, I will give that a try.

Are you doing this in MDI?

Does it do the same if you have it in a program?

I doubt this is the cause, but what is the contents of parameter 3?

Its when running a program.
I will check parameter 3 this afternoon.

Thanks for the replies!

 

[dandrummerman21]

I run several 0 machines here, all of which are Leadwell verticals of the same era, and none of them require cancelling the offset with g49 before sending it home with G28G91Z0M19

Only other thing I can guess, are you SURE you had a G91 in there and not G90? with a G90 in there, it would send the tool tip to Z0 before going up to home.

 

[sinha]

No, just cutting with the tool, rapid up a little and calling G91 G28... At any rate, I will give that a try.

It is ok. Length offset need not be cancelled. Should have gone to home position directly.

Also try G91 G53 Z0.
Edit: Read G90 instead of G91

 

[sinha]

Only other thing I can guess, are you SURE you had a G91 in there and not G90?

Do verify.

 

[Sage Brush]

Ok. Ran a test program with a tool length offset of 1.0".

%
O0013
(Tool Offset Cancel Test)
(BEGIN PREAMBLE)
G17 G54 G40 G49 G80 G90
G20
(MACHINE UNITS: IN/MIN)
G54
(7-32IN_ENDMILL_3FLU001)
M5
(TOOL CHANGE)
G91 G28 Z0
G90
M6 T7
G00
G43 H7 Z3.6900
M3 S3000
(BEGIN OPERATION: PROFILE)
X1.5799 Y1.5799
G1 X1.5799 Y1.5799 Z3.1500 F6.0000
G2 X0.1452 Y-2.2296 I-1.5799 J-1.5799 F10.0000
G0 Z3.6900
(BEGIN POSTAMBLE)
M05
G49 (Tool Offset Cancel)
G91 G28 Z0 (HOME Z)
G91 G28 X0 Y0 (PARK TABLE)
G17 G54 G90 G80 G40
M30
%

Still the exact same behavior. Tool moves down 1.0" during G49, then rapids up to home.

I checked parameter 3: 00000001

 

[angelw]

Also try G91 G53 Z0.

A Fanuc control ignores G53 completely when specified in G91 Mode; it only has affect in G90 Mode.

@ Sage Bush
It doesn't answer your question as to why the machine is behaving in the manner it is, but the workaround would be to use G90 G53 Z0.0 instead of G91 G28 Z0.0

Regards,

Bill

 

[dandrummerman21]

So you had G49 in there before? Does it happen without G49?

 

[angelw]

Still the exact same behavior. Tool moves down 1.0" during G49, then rapids up to home.

Well, the behavior is different to how you first described it if it's moving during the G49 command. There is a parameter that affects how G49 is applied, either the Tool Length Offset is canceled and physical movement occurs, or reference to Tool Length Offsets is set to Zero and no axis movement occurs.

Regards,

Bill

 

[Sage Brush]

So you had G49 in there before? Does it happen without G49?

When I first saw this problem the program did not have G49 before the G28 Block.

Well, the behavior is different to how you first described it if it's moving during the G49 command. There is a parameter that affects how G49 is applied, either the Tool Length Offset is canceled and physical movement occurs, or reference to Tool Length Offsets is set to Zero and no axis movement occurs.

Regards,

Bill

Your right. It is a bit different. Actually, I see the exact same stuff happening using G43 to call an offset. Calling a negative offset just after a tool change would send the Z UP and over travel. Issuing a rapid down in the same block fixed that. But like you said the issue really seems to be how the offset is applied or cancelled and not with G28 working wrong.

 

[angelw]

I see the exact same stuff happening using G43 to call an offset. Calling a negative offset just after a tool change would send the Z UP and over travel. Issuing a rapid down in the same block fixed that.

That behavior is rather typical and it's almost universal practice to call G43 in the first Z movement Block. One machine of a client when G49 is executed will cancel the Tool Offset with a physical Z movement, but G91 G28 Z0.0 will move the axis seemingly directly to the Z Reference Return position irrespective of whether G49 is executed prior or not. I say seemingly, because with the G91 G28 Z0.0 command, the move to the Reference Return position is via the Intermediate position Zero distance away from the current position.

Regards,

Bill

 

[Sage Brush]

Ok. Edited the above program so the last few blocks were:

M05;
G90 G53 Z0;
G91 G28 X0 Y0;
G17 G54 G90 G80 G40;
M30;

Works well. No downward movement even with length offset at 1.0".

I looked in my manual for the parameter to set G49 behavior. I must have missed it. I'll have another look later on.

 

[TKassoc]

Check parameter 5006.6=1 which prevents rapid down on a G49

 

[Sage Brush]

Check parameter 5006.6=1 which prevents rapid down on a G49

Thanks for the suggestion, but I seem to only have 3139 jumping to 6140. No 5000 parameters.

 

[Sage Brush]

I don't know if this is related but, if I run the above program and stop in the middle (Feed Hold, Reset) and run the program again, the tool will move DOWN 1.0", then rapid up to home for the tool change (G91 G28 Z0). This is even after the preamble block containing a G49. I saw something in the manual about a setting which would not cancel an offset when a issuing a control reset command. Back to the manual...

 

[Sage Brush]

Could this be part of the problem?

Parameter 24.6 CLCL
1: The local coordinate system is canceled by automatic reference point return.
0: Not canceled.

On my machine this bit is 0.

 

[sinha]

A Fanuc control ignores G53 completely when specified in G91 Mode; it only has affect in G90 Mode.

That was a typo. I meant G90 only.