[donl517]

I'm trying to get my table to come to the front of the machine and center; This works fine but Z is running away and faulting at the top of the head. I've tried:

G53 Z0 M9
G53 X0 Y10. M5

&

G53 Z0 M9
G53 X0 Y10. Z0 M5

Both give me the same result when executing the second line Z+ Axis overtravel.

Any thoughts?

Thanks,
Don

[carbidecraters]

Man I do not like G53!!!
I do this


G0Z0H0
X0Y10.
M30

You can use a H0 instead of G53..G53 is very quirky

[VMC_Jeff]

Try G0 G90 G49 Z0 instead

[carbidecraters]

Here is a hole example for format 2 that I use

O212 (.643 hole, single
M6T3 (.500 DRILL/MILL
M3S2600
G0X0Y0
Z.1H3D3M8
G1Z-.8F25.
G1G41X.3215Y0
G3I-.3215
I-.3215 (TWICE AROUND HOLE)
G40 X0Y0
G0Z.1
M5M9
Z0H0
Y7. (MOVES TABLE NEAR OPERATOR)
M30

It really is as simple as that in format 2

[donl517]

OK, this works:

G0Z0H0
G53X0Y10
M30

(I think not canceling the tool offset must have been causing the problem.)

However, does the machine have to go back to X0 Y0 at the M30(M02) command? Is there a parameter that can be set or do I need to put an M0 in front of the M30?

Thanks,
Don

[donl517]

OK, this works:

G0Z0H0
G53X0Y10
M30

(I think not canceling the tool offset must have been causing the problem.)

However, does the machine have to go back to X0 Y0 at the M30(M02) command? Is there a parameter that can be set or do I need to put an M0 in front of the M30?

Thanks,
Don

Sorry, I forgot I had switched back to format 1 while trying to figure something else out. It works right in format 2.

Thanks,
Don

[carbidecraters]

Why are you calling G53 after homing your Z with H0? Your G53 is not needed. M30 wont make the machine go anywhere and will end the program where the axis is.

G53 mean you are using the machines default (or cold start) co-ordinates so you will basically be going to X0 (middle of the table) and Y10. which will be the end of your y travel if you have a 20inch travel in Y. It is easier to eliminate the G53 and jog the Y to where you want it using your fixture offset or your manually inputed X0Y0 that you probly had for your part. So you jog your Y to lets say 7 or 8 inches and then you add that to the end of your program like you did bu without the G53.

Hope I didnt confuse you

[carbidecraters]

Oops sorry I reread that you wanted the table to center and come to the front. I was trying to help you get it to just come to the front. I believe you have it.

[Derdle]

Here is how I end my programs in Format 2:

First jog the table to the desired location(front and center) then use the SETH(set home) command. You only need to do this once or until you want to change the location.

end of program looks like this:

M6T3(DRILL
M3S1500
GO X0 Y0 E1
Z.1 H3
G73 G98 R0+.01 Z-1. Q.25 F12.
X1.
X2.
G80
G0 Z4. (move the tool to a clearance position)
M5 M9
E0 Y0 X0 (clears offsets and moves to SETH position)
M6T1
M30

The table will move in x and y first, then z, so don't forget the Z clearance move.

The nice thing about this is you can position your home where ever it suits your particular setup.I always back off the Y an 1/8 inch from the axis limit to keep the table from banging against the axis limit.

[machinist_1]

G0G49Z0:
G0G54.1P48X0Y0:
M30:

This is what works with the Fanuc 18i

[Larry83301]

On ALL of our FADAL machines, we just set the home position to table X center and Y max with the table to the front. Worked well for unloading fixtures.

[WJ MARK]

Try this

G28 H0 Z0
E0 Y0