I am using Surfcam 2004 and when I post drilling and tapping cycles it produces a z move on the first line of the hole pattern. I didnt have a Format 2 post with rigid tapping so I reworked the Format 1 with RT and everything is works except the extra z. It doesnt affect the drill cycles only the tap cycle. if I dont manyall take it out the machine will alarm out. Can anyone help with how to fix the Pst file so that it wont produce this extra z.

The post looks like this.

M6 T3 ( Tool Radius 0.095 Diam 0.19 Corner Rad. 0
G0 G90 S200 M3 E1 X-4.5669 Y-0.2475
H3 M8 Z1.
G84.1 G98 S200 R0.1 Z-0.5571 X-4.5669 Y-0.2475 F8.3334
Y-0.8775 Z-0.5571 (This is the z I am talking about.)
X-0.472
Y-0.2475
G80


My post file looks like this.
name FadaL 2 Rigid Tapping

% 00
! 00
/ 00
O >4
N >4
g >2.1 G
G >2
S >4
H >2
D >2
M >2
T >2
R ->3.>4
r +->3.>4
z ->3.>4 Z
E >2
X ->3.>4
Y ->3.>4
Z ->3.>4
I ->3.>4
J ->3.>4
K ->3.>4
F >4.>4
Q ->3.>4
P >4
L >4
( 00
d >3.>4
e >3.>4
f >3.>4
* 00 ""

ModalLetters X Y Z F R # List of letters that are modal

ModalGs 0 1 2 3 73 74 76 80 81 82 83 84 84.1 85 # List of g codes that are modal

Sequence#s N 0 1 1 # Char, freq, incr & start
First#? Y # Y or N 'Output 1st sequence no.
Last#? Y # Y or N 'Output last sequence no.

HCode X # X or X U 'Horizontal char.
VCode Y # Y or Y V 'Vertical char.
Dcode Z # Depth char.
FeedCode F # Feed rate char.

Comment ( ) # Begin End comment char.

Spindle 3 4 5 # Cw, ccw & stop m codes
Coolant 8 9 7 # On, Off & Mist m codes
DComp 41 42 40 # Left, Right & Cancel m codes
LComp 43 49 # On & Off codes

Feed G1 # Linear move
Rapid G0 # Rapid positioning word
Cw G2 # Circular move clockwise
Ccw G3 # Circular move counter clockwise

Inc/Abs G 91 90 # Inc & Abs char. & values

CtrCode I J # I J or R or I J K L
Helical? Y
Spaces? Y # Y or N 'Spaces between words

Incremental? N # Y or N 'Inc or abs output
CtrIncremental? Y # Y or N 'Inc or abs I & J
ByQuadrants? N # Y or N 'Break arcs at quadrants

UppercaseComments? Y # Y or N 'Require uppercase comments

WorkDefault 1 # Work offset register default

Drill # Drilling canned/manual cycle
G81 G98 R[Vclear] z[D] F[FRate] X[H] Y[V]
end cancel

Peck # Pecking canned/manual cycle
G83 G98 R[Vclear] z[D] F[FRate] Q[VBite] X[H] Y[V]
end cancel

Tap # Tapping canned/manual cycle
g84.1 G98 R[Vclear] z[D] X[H] Y[V] F[Frate] S[Speed]
end cancel

LTap # Left handed tapping cycle
G74 G98 R[Vclear] z[D] F[Frate] Q[VBite] X[H] Y[V]
end cancel

Ream # Reaming canned/manual cycle
G85 G98 R[Vclear] z[D] F[FRate] X[H] Y[V]
end cancel

Bore # Boring canned/manual cycle
G86 G98 R[Vclear] z[D] F[FRate] X[H] Y[V]
end cancel

Back # Back boring canned/manual cycle
G76 G98 R[Vclear] z[D] F[FRate] Q[Sclear] X[H] Y[V]
end cancel

Cancel # Cancel a canned/manual cycle
G80
end

StartCode # Start of the program
%0
O[Program#]
End

1stToolChange # First tool change
M6 T[Tool] (0 d[ToolRad] e[ToolDiam] f[corner]
G0 G90 S[Speed] M[Direct] X[H] Y[V] E[Work]
H[Lcomp] M[Cool] Z[D] D[DComp]
End

Infeed # Enable cutter comp
G1 G[Side] X[H] Y[V] F[FRate]
end

Outfeed # Disable cutter comp
G40 X[H] Y[V]
Z[D]
end

ToolChange # Secondary tool changes
M5 M9
G0 G49 G90 Z0
M6 T[Tool] (0 d[ToolRad] e[ToolDiam] f[corner]
G0 G90 S[Speed] M[Direct] X[H] Y[V] E[Work]
H[Lcomp] M[Cool] Z[D] D[DComp]
End

EndCode # End of the program
M5 M9
G0 G49 G90 Z0
E0 X0 Y0
M6 T[Tool1]
M2
%0
End

replace "d" with "Tool Radius "
replace "e" with "Diam "
replace "f" with "Corner Rad. "

I've always had to add the spindle speed on that and every line on my tap cycle in format two but maybe that's because I left the Z in the first line.

M6 T3 ( Tool Radius 0.095 Diam 0.19 Corner Rad. 0
G0 G90 S200 M3 E1 X-4.5669 Y-0.2475
H3 M8 Z1.
G84.1 G98 S200 R0.1 Z-0.5571 X-4.5669 Y-0.2475 F8.3334
Y-0.8775 Z-0.5571 S200
X-0.472 S200
Y-0.2475 S200
G80

Sometimes you have to have the Z there if the hole depth is changing. I always wish I new what made the post put that Z out so I could use it to make it put the speed on every line.

If you just remove the z on the first line it will work. When I hand code at the machine I only have the z in the g84.1 line only then just add my positions and it works fine. The extra z doesnt bother dirll cycles but it does on the tap cycle.

Does any body have any Idea how to resolve this problem?

I corrected this in my post by removing the "z ->3.>4 Z" line, and changing all the lowercase "z" in the drill cycles to uppercase.

In your post "Z" is listed as modal and "z" is not.

The problem will be corrected only if you move (FADAL ONLY) the entire drilling section to the very bottom of the post.

add little z to the post line
ModalLetters X Y Z F R # List of letters that are modal
> ModalLetters X Y Z z F R # List of letters that are modal

I corrected this in my post by removing the "z ->3.>4 Z" line, and changing all the lowercase "z" in the drill cycles to uppercase.


Thanks for the help it worked like a champ.