Problem with G52

[kevinwd1]

I have been using the G52 command without any problems until today when I didn't cancel my offset before executing G52 X0 Y0 command. I didn’t think this would be a problem until I realized my absolute position had changed by the exact amount of the offset .The only way to reset the absolute position was to turn the machine off and back on. I was of the understanding that the command G52 X0Y0 would reset any positional change when using G52 command.
I played around with the programs and whenever I didn't cancel my offset before executing the G52 X0 Y0 my absolute position would incrementally change by the amount of my offset. If I ran the program three times my absolute position would change by three times my offset.
Is there any way to overcome this instead of turning my machine off?
Hope this makes some sort of sense

Thanks Kevin

[angelw]

I have been using the G52 command without any problems until today when I didn't cancel my offset before executing G52 X0 Y0 command. I didn’t think this would be a problem until I realized my absolute position had changed by the exact amount of the offset .The only way to reset the absolute position was to turn the machine off and back on. I was of the understanding that the command G52 X0Y0 would reset any positional change when using G52 command.
I played around with the programs and whenever I didn't cancel my offset before executing the G52 X0 Y0 my absolute position would incrementally change by the amount of my offset. If I ran the program three times my absolute position would change by three times my offset.
Is there any way to overcome this instead of turning my machine off?
Hope this makes some sort of sense

Thanks Kevin

Hi Kevin,
It was my understanding also that G52 X0 Y0 would cancel the Local Coordinate System. However, G52 can be cancelled by Reset if the RLC bit is set to 1. The parameter and bit number is #1202.3 for late model controls. For controls before Series 16, I don't think the RLC bit is available and by default G52 will be canceled by Reset.

Regards,

Bill

[fordav11]

incremental work shifts can be dangerous. you've found out the hard way why almost no one uses G52.
Use G54 to G59 as it's much easier to keep track of where your zero is that way.

Here's some notes from the manual.....

By specifying G52 IP _;, a local coordinate system can be set in all the
workpiece coordinate systems (G54 to G59). The origin of each local
coordinate system is set at the position specified by IP _ in the workpiece
coordinate system.
When a local coordinate system is set, the move commands in absolute
mode (G90), which is subsequently commanded, are the coordinate
values in the local coordinate system. The local coordinate system can
be changed by specifying the G52 command with the zero point of a new
local coordinate system in the workpiece coordinate system.
To cancel the local coordinate system and specify the coordinate value in
the workpiece coordinate system, match the zero point of the local
coordinate system with that of the workpiece coordinate system.

WARNING
1 When an axis returns to the reference point by the manual reference point return function,the
zero point of the local coordinate system of the axis matches that of the work coordinate system.
The same is true when the following command is issued:
G52a0;
a:Axis which returns to the reference point
2 The local coordinate system setting does not change the workpiece and machine coordinate
systems.
3 Whether the local coordinate system is canceled at reset depends on the parameter setting.
The local coordinate system is canceled when either CLR, bit 6 of parameter No.3402 or RLC,
bit 3 of parameter No.1202 is set to 1.
4 If coordinate values are not specified for all axes when setting a workpiece coordinate system
with the G92 command, the local coordinate systems of axes for which coordinate values were
not specified are not cancelled, but remain unchanged.
5 G52 cancels the offset temporarily in cutter compensation.
6 Command a move command immediately after the G52 block in the absolute mode.

[samu]

I use G52 on regular basis and never faces any problem until i mixed it with G68.
If i call G52 when G68 is active, the result seems to be unpredictable and G52 X0 Y0 doesn't reset the offset even if i come back in G69.
Rehome the machine reset offset as it should be.

Do you use G68 with G52 ?

[kevinwd1]

No I don't use G68; I’m not sure what that command does?
I have been using G55 to G59 at the same time as G52 without a problem. Also have been using mirrors at the same time as the G52 command and haven't had a problem so long as I turn them on and off around the same centre position.
The problem seems to occur if I use the G52 X0 Y0 command before I've canceled my offset .I will now start all my programs with these two lines to hopefully overcome this problem.

G91G40G80G28G00Z0.
G52X0Y0

Also does anyone know how to get your X0 Y0 position back when you cancel your mirrors incorrectly? The only way I can do it is if I turn the machine off then on.

[fordav11]

Depending on your Fanuc control....(you don't say what you have?)
G68/G69: Coordinate system rotation/cancel
G68/G69: Three–Dimensional Coordinate Conversion

[kevinwd1]

Unfortunately a lot of commands seem to be options on my control so I don’t have a rotational command. I would also love to have helical interpolation. Also not sure if being able to copy programs within the control is an option, but I unable to do it? We have a similar machine with an earlier control in which we can copy programs within the control but following the same procedure doesn’t work even though the machine instruction manual is the same for both machines.The controller is a MSC-501 on a Mori Seiki milling machine (SV 500)

[fordav11]

MSC-501 is a Fanuc 18i Model A. in your case 18iMA
so your mirror image command would be G50.1/G51.1 right?

The 18i manual says.....

In programmable mirror image mode, G codes related to reference
position return (G27, G28, G29, G30, etc.) and those for changing the
coordinate system (G52 to G59, G92, etc.) must not be specified. If any
of these G codes is necessary, specify it only after canceling the
programmable mirror image mode.

[underthetire]

Helical and g68 are standard on a sv500.

[kevinwd1]

For mirrors I use M73,M74,M75,M76 codes

[fordav11]

hmmm, well either way the manual says not to use a workshift command while in mirror mode.
so cancel mirror, set workshift then go back to mirror mode.

[kevinwd1]

I only use mirrors after work shift command and turn them on and off around the new centre .I only have problems with mirrors when I reset programs before cancelling mirrors. This usually happens when testing a program above the job and out of habit hit reset when cutter starts to move back to machine z zero. This is when I have to turn the machine off and on to get back to my correct X0 Y0 position. This problem occurs also when not using G52 command.