Maho MH 800E (CNC 432 Phillips)

[kotten1]

Hi.

We have an old Maho MH 800E with CNC 432 Phillips.

Now to the problem.

Howe do I run the machine to machine zero point? (What is the G-code for it?)
I wont to have that G-codes at the end of the program.

Regards/
Kotten1 Sweden

[Konrad]

Are you just setting up this machine?
Are you trying to run machine home?
If you want to go to Z0, Y0 X0 at the end of program, then it would look like this..

G0 X0 Y0 Z0 M30 but... Y3" or so for tool clearance would be better and move ram Z 4" away.

Konrad

[kotten1]

Hi.
We have this machine at my work.
I working at SNA-europe
Snap-on in USA owns us.

If I run the machine in G0 X0 Y0 Z0 M30, it would be the same point that I have in G53?

I would like to run the machine to the ref point.
The same position you run the machine to than you start it up.

Regars/
Kotten1 Sweden

[sneebot]

I think G52 is the reference point zero. So if you are 'in' G53. You need to have a call G52 and then go to zero

G52
G0 X0 Y0 Z0 M30

You should be able look at all saved reference points from the programming menu.

[Paul Deady]

You should try the following,
G51 Cancels the Reset Axis Position (or G52)
G53 Cancels Stored Work Coords (G54 - G59)

Therefore if you are usinfg G54 to G59 in your Prog
G53 X0. Y0. Z0.

If you have found Prog Zero Point & Reset the Axis use G51

[kotten1]

Here is a small program to my machine.

After block N210 G0 Y100 M5.
Should it be like this? N220 G52 X0 Y0 Z0 M30

%PM
N9001
N10G18
N20G51
N30G54
N40M5
N50T19M6
N60S2400M03
N70
N80G0X-60.Z10.Y100.M03
N90G0X-60.Z10.Y3.M03
N100G1Y0.F400.
N110G1X60.Y-.9474F960.
N120G1Z-60.Y-1.5
N130G1X-60.Y-2.4474
N140G1Z10.Y-3.
N150G1X60.
N160G1Z-60.
N170G1X-60.
N180G1Z10.
N190G1Y3.F1000.
N200G0X-60.Z10.Y100.M03
N210G0 Y100 M5
N220M30
N230

Regards/
Kotten1 Sweden

[Paul Deady]

Hello Kotten1,
N20 you have re set or canceled the Automatic Shift Value of Zero Datum Shift G52
N30 you are using the Stored Zero Datum Shift 1 G54

Therefore to cancel G54 use G53, Be aware that this will now change to the machine co ord positions. M/C ref pt and zero point are not the same values. On a 600 M/C my refrence point is at X =560.6, Y =390.6, z =390.6.
To check your positions in MDI (MDA) type G51 Enter Cycle Start, G53 Enter Cycle Start
Then go to manual mode, Menu #2 / Refrence point search. The values after refrence search will be on the screen
Therefore for a 600 M/C I would use
N220 G53 X590.6 Y390.6 Z390.6
N230 M30

This would send the machine back to refrence point at the end of the prog.
Hope this helps
Regards
Paul Deady