[minifig-phil]

I just got a 2001 Fadal that I'm trying to learn how to use and am having some problems trying to get my program to run
I'm in Format 2 and have set my tool lengths to the table and work offset is Z+4.364 (set from table) in E1 (G54)
It runs OK until it gets to the 1st tool change then it goes past the CS Z Position right to the limit.
What am I doing Wrong?
Program was created in MasterCam X3 with Fadal Format_2 4x Mill pst

%
N1 O0007(T)
N2 G20
N3 G0G17G40G80G90
( 1/2 EM TOOL - 1 DIA. OFF. - 51 LEN. - 1 DIA - .5 )
N4 T1M6
N5 G0G90S2600M3E1X4.0672Y-1.85
N6 H1Z2.
N7 Z.1
...
N9 X-.35
N10 G0Z2.
N11 M5
N12 G90H0Z0. ------ Here Z goes up past Tool change height to hit software limit
N13 M1
( TOOL - 2 DIA. OFF. - 52 LEN. - 2 DIA - .25 )
N14 T2M6
N15 G0G90S5000M3E1X.4651Y-.9229
N16 H2Z2.
N17 Z.1
N18 G1Z-.028F12.
...
N20 X3.2494Y-1.7111R.0193
N21 X3.2301Y-1.7303R.0193
N22 G0Z2.
N23 M5
N24 G90H0Z0.
N25 E0X0Y0
N26 M30
%
%

[slowtwitch]

I would change your G90H0Z0 to something like this G28 G91 Z0.

[ianagos]

Do you have a negative length tool offset?

[minifig-phil]

Yes tool offset is negitive.

[ianagos]

Did you try adding a g28 g91 z0?

This is a bit of one of my programs

N10 G90 G94 G17
N15 G20
N20 G28 G91 Z0.

(FACE3)
N25 M9
N30 T3 M6
N35 S4000 M3
N40 G4 P45
N45 M8
N50 G90 G0 E5 X4.92 Y-1.

[Techman]

You just need to combine your xyz into one line.
G0G90X1.Y0E1Z3.H1
The z value in your fixture offset exceeds the plus value above the z cold start limit. Even though you didn’t command the z axis in your first xy line the controller thinks it has to move the z by the fixture offset amount to maintain z zero. I use both tool lengths and a z value in my fixture offset all the time. Hope this helps!

[ianagos]

You just need to combine your xyz into one line.
G0G90X1.Y0E1Z3.H1
The z value in your fixture offset exceeds the plus value above the z cold start limit. Even though you didn’t command the z axis in your first xy line the controller thinks it has to move the z by the fixture offset amount to maintain z zero. I use both tool lengths and a z value in my fixture offset all the time. Hope this helps!

That should work too. The g91 will also solve it and he could just throw that in to the code vs trying to change a bunch of stuff.

[Techman]

Whoops! Just re-read the original post. He will have a crash on line 5 and line 12. Line 5will hit the limit because of his z offset value. Line 12 will hit it again because the fixture offset is still active. I changed my master cam post to put out combined xyz moves on the first rapid line and an M1 immediately after every tool change. No wrecks and works every time.

[warrenb]

The Tx M6 command will bring the z up regardless of offsets. Why put in the extra codes with "G90H0Z0."

[minifig-phil]

I tried g28 g91 z0 and it worked
will try just a Tx M6

Just annoying that i have to edit posts.
Is there a way to modify the post in Mastercam so I don't have to edit each .nc file?