Z Axis overtravel at end of program

[tmachine]

I just borrowed a '97 4020 CNC HS88 with software updated to a copyright date of 2002. I am new to Fadals and normally run Mitsubishi controls.

It has been running fine for a couple of weeks, but now at the end of the program, the Z Axis goes straight up and over-travels and shuts off the drives. I am using the same post (I think). The machine is in format 1. At start up I enter SETH at the CS position and I am using E1 for my fixture offset.

The code is:

N21660 G0 Z10.
N21670 M5 M9
N21680 G91 H0 Z0.
N21690 E0 X0 Y0
N21700 M2

I tried removing line 21680, but it still does it. The post is the one that came with MasterCam 9.1 SP2.

As a temporary fix, I have been adding an M00 before that line. When the program reaches the STOP, I press Manual and enter HO to send it home.

Confused!

[HuFlungDung]

I don't know Fadals, but
G91 H0 Z0
seems illogical to me. H0 cancels the length offset, and G91 Z0 in an incremental move of zero distance, so I find it hard to imagine what I'd be expecting the control to do.

Is there no G28 command available such as:
G00 G28 G91 Z0
or in the machine coordinate system:
G00 G53 H0 Z0
(perhaps G53 = E0)

[daking]

Try replacing G91 H0 Z0 with G49G0Z0. I think what might be happening is that when you call G91H0Z0 the control ignores it because it means nothing and the when you call E0X0Y0 its actually trying to move to E0X0Y0Z10. which would put you 6" past the hard stop in the Z.

Try this:
N21660 G0 Z10.
N21670 M5 M9
N21680 G49 G0 Z0
N21690 E0 X0 Y0 Z0
N21700 M2

[tmachine]

Thanks for your replies.

I tried changing the G91 to G90 and that works also. Now I have to figure out why my post changed.

[stucaruk]

You're telling the machine to overtravel at the end of the part, causing it to hit the upper limit switch and trip out an E-Stop.

At the end of your part, change your post to this:
G0 Z1.
G0 G80 G90 M5 M9
G53 Z0
X0 Y0 Z0 H0 E0 (actually I move x and y to brng the part to the front door)
M30
%

[JR1050]

Either of the two examples will work.Number two will make it easier to convert your program to run on a Fanuc type control.

M9M5
G0H0Z0
E0Z0X0Y0
M30(OR M2)
%

#2
M9M5
G0G49Z0
E0G28Z0Y0X0
M30
%
Good luck

[CAD/CAM Man]

#2
M9M5
G0G49Z0
E0G28Z0Y0X0
M30
%

Depends on which mode of movement you are set to (G90 or 91). On some older FADALs if you were in G90 mode (absolute) when the control reads a G28, it will return the Z axis to the initial Z zero. (top of the part in most cases) That really is not a big deal, but it can be enough to scare the crap out of you then the tool moves TOWARD the part before it goes home. I have written my posts to output the following at the end of the program:

G0 G80 G90 Z1. M9 (I add the G80 to cancel any canned cycle that I might
have been using)
G91 G28 Z0 M5
G0 G90 X0 Y0 E0 (X and Y values can be eddited to move the table closer to
the operator)
M30


You only see this at the last tool in the program because the "G91 G28 Z0" is written into the macro that is executed for a tool change.

Hope this helps

[billystein]

this line "G91G28Z0M5" is an old fanuc line.
the fadal only needs "Z0H0M5" to perform the same function.
I have never used g91 on any fadal except when using 4th axis conouring with some post processors.