Has anyone had any experience generating a Surfcam postprocessor file for a CNC mill? I currently have SurfCAM 2003 and am trying to set up a postprocessor for a Sherline 2000 CNC running Mach3Mill.

I've been playing around with the SPOST option file generator, but I'm not even sure what it does exactly.


Thanks,

Neil

I would try working with the MPost. It's easier to configure, you should be able to find a stock post you can modify. The manual has pretty much all the info you need. All the files are in plain text, so you can edit them in a simple text editor. You should have on hand the specs for your machine w/regards for what it wants for input. --ch

Yes, Mpost is easier.
Find a file name POSTFORM.M .
Back it up before you make any changes.
This is where you can make changes.
If you write a specific question we can help you.
There is a lot of information in the end of the surfcam help file.

Thanks, I'm off to play with Mpost.

Hey Neil

Any luck with a post for Mach3?

I've been playing with the Mpost too
Let me know where you got to

Steve

Well I have the start code right and the end code
But getting a G00 or G01 in all the lines seems to be tougher to do
I don't need to change the G02 or G03 they seem right (I'm playing with the Fanuc 10 post)

Any ideas?

Steve

In the line that starts with "ModalGs", you will see some numbers. If you want G0 and G1 to be output on every line, remove the 0 and 1 from that line. "Modal" means active until canceled or changed, and therefore the output is only given at that point. If something is not modal, it will be output on every line where it is called for. --ch

thanks bud

I'll try that

that got it
Not sure if thats what Mach3 needs yet; but I know turbocnc needs it
I run both

actually I think Mach uses just g1 and g0
So changing that should be just 1 numeral instead of 2
I know that one
I'll make 2 posts
1 for Mach3 1 for turbocnc

Turbocnc post is just about done; but then it's really quite simple
Mach 3 is getting there; need to play with it a bit more; but I have most of it done already
Way simpler than Mastercam to change posts

Hey Neil

Any luck with a post for Mach3?

I've been playing with the Mpost too
Let me know where you got to

Steve


I did get it working with Mach3, I'll attach it here tomorrow.

Thanks

I'd like to see it

again thanks
Steve

I found the Z was only giving positive moves in the post for Turbo; it started at the bottom of the cut and worked up (wow)
So I guess I need to add the - sign to the numerals rule
I thought of this while I was shaving this morning; I'll have to try it once I get a chance

Hey Neil

Any luck with a post for Mach3?

I've been playing with the Mpost too
Let me know where you got to

Steve


Here's my mach3 post. It has worked pretty good for me.

(rename it to Mach3Mill.m3 and insert into C:\surfcam\PostLib\mpost .. Then use the Post Menu Wizard utility under Start/Programs/Surfcam xx/Surfcam Tools to add the post)

Hi Neil

Thanks
I'll shoot it into Surfcam tonight

Actually both mine and yours work about the same
mine is a but smaller; with less stuff in the start code but the results are the exact same as far as running Mach3

Here is mine

name Mach 3

% 00
/ 00
O >4
G 1
N >4
$ 00
^ 00
& 00
* 00
X ->3.>4
Y ->3.>4
Z ->3.>4
A ->3.>4
I ->3.>4
J ->3.>4
K ->3.>4
Q ->3>4
R ->3.>4
P >40
F >3.1
H >2
D >2
T >2
M >2
S >4

SbackDoor SupressHeader

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

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

Sequence#s G 0 1 1 # Char, freq, incr & start
First#? Y # Y or N 'Output 1st sequence no.
Last#? N # 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 61 62 63 64 # Flood, Off, Mist and Thru Spindle M codes
DComp 41 42 40 # Left, Right & Cancel m codes
LComp 43 49 # On & Off codes

Feed G01 # Linear move
Rapid G00 # Rapid positioning word
ArcPlane G 17 18 19 # G19, G18, G17 Arc Plane selection
ReturnPlane 98 99 # G98 G99 Return Plane selection
Cw G2 # Circular move clockwise
Ccw G3 # Circular move counter clockwise

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

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

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

UppercaseComments? Y # Y or N 'Require uppercase comments

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

CSink
G82 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate] P[Dwell]
end cancel

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

Tap # Tapping canned/manual cycle
if [Rigid] > 0
G93 G93 to lock Z to spindle rotation.
G84 G[RetPlane] X[H] Y[V] Z[D] P[Dwell] R[VClear] F[FRate]
else
G84 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
Endif
end cancel

LTap # Left handed tapping cycle
G74 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate] Q[VBite]
end cancel

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

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

Back # Back boring canned/manual cycle
G87 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
end cancel

Cancel # Cancel a canned/manual cycle
G80
if [Rigid] > 0
G94 Unlock Z if w/ rigid tap.
endif
End

StartCode # Start of the program
G90 G80 G49
End

1stToolChange # First tool change
T[Tool] M6
M[Direct] S[Speed]
G0 G[Work] X[H] Y[V]
G43 Z[D] H[Lcomp]
M[Cool]
End

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

Outfeed # Disable cutter comp
G1 G40 X[H] Y[V]
end

ToolChange # Secondary tool changes
M9
G49 Z0 M5
T[Tool] M6
M[Direct] S[Speed]
G0 X[H] Y[V]
G43 Z[D] H[Lcomp]
M[Cool]
End

EndCode # End of the program
M5
M30
End

Replace "$" With "()"
Replace "^" With "()"
Replace "&" With "("
Replace "*" With ")"

I dont use the same method of adding a post
you put
(rename it to Mach3Mill.m3 and insert into C:\surfcam\PostLib\mpost .. Then use the Post Menu Wizard utility under Start/Programs/Surfcam xx/Surfcam Tools to add the post)
I just edit one of the existing posts that I do not need; then rename it in the Surfcam pst file; so it shows as what I want in the dialog box when it's time to post
I'm still tweeking the Turbocnc post; not quite there yet

Thanks Neil

oops; edit
all the spaces it needs have been dropped by posting it here; if someone needs it i'll repost as an attachment; but Neil's is just about the same