Post edit help?

[yanzeek]

Just started a new job. First time with Surfcam. 2003
Now where is the Pst file that I have to edit, because the "Old man" wants circle done in simple two lines, so the program will be short, easy to transfer, cuz we dont have and DNC setup to transfer, still doing old fashion way.
I Guess I have to change ByQuad value to "N". But where is that file??
Surfcam is a bit straight forward, doent let you do a lot of things, or maybe I havent gone that far (its 4 days I am using it).
Oh Yeah! How do I disable "infinite look ahead" in Surf?
Anyway first thing is to know how do I get to the pst file, open it in what?

There are tons of pst file in Mpost? folder, and I have to edit fanuc pst. In one directory there are 3 exe files one for wire, mill and lathe, and when I post the program, one of these files execute and ask me bunch questions like for which machine? program number? and work offset.

If anyone can help me, plz reply. I am on a weeks trail and its going to be over. And employers dont like new guys doning mistakes and look clueless. Though its ok for someone who's been working there for long time.

[JimW]

The Surfcam.pst file is a file that Surfcam uses to direct the file your posting to the post. The actual post that your wanting to change is called postform.m and it is located in the PostLib folder. But as always make a backup copy before changing, an inadvertent change to either of these files can be a real headache.

[ltmquik]

You need to open the PostForm.m file and find the post file name that you intend to edit. Depending on the number of posts you have added to SurfCAM there could be alot. I found that the newest posts are loaded at the end of the PostForm.m file. Look for the titles "name [the post name that appears in SurfCAM]". These are basically the same as the files in the POSTLIB, MPOST folder. You have to change the PostFrom.m file as SurfCAM does not even look at the .M3 files.

I made a backup of the PostForm.m file and then deleted all the posts that we do not regularly use from the PostForm.m file. This makes it alot easier to edit the posts when you need to.

[yanzeek]

Thanks guys, it really helped me. Found that post file and edit that, most of the thing is as I want except one thing.

1stToolChange # First tool change
G0 x0.0 y0.0
T[Tool] M6 (0 e[ToolDiam] f[corner]
Comments
G0 X[H] Y[V] # "G90 G[Work]" Taken out
G43 H[Lcomp] Z[D] M03 M08 S[Speed]
End

In here I am getting tool dia and corner rad in this format.
( Tool dia: 1 C Rad: .2
But it is missin a ) to close it
In The bigening of Post processor I have ( 00
But there is no entry about )
I put a line ) 00 and edit that line to T[Tool] M6 (0 e[ToolDiam] f[corner])
but it didnt work got error, any idea how can I get a ) to close it?

[ltmquik]

We should know what the controller is you are trying to fix. Some controllers don't need closed comment lines.

[yanzeek]

They are fanuc, haas and fadal. As I have been told by the superviser, he want them to be closed, even if the controller dont need it.
Any suggestion what is suppose to be fixed in it?

I am posting the post file here, it has all my edit too that I did yesterday.

name FANUC

% 00
! 00
/ 00
O >4
N >4
G 2
X ->3.>4
x 1.1 X
Y ->3.>4
y 1.1 Y
Z ->3.>4
z 1.1 Z
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
S >4
M >2
( 00
d >3.>4
e >3.>4
f >3.>4

SbackDoor SupressHeader

ModalLetters X Y Z F R # List of letters that are modal (Added R in modal -26/1/2007-)

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

Sequence#s N 1 1 1 # Char, freq, incr & start
First#? N # 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 R # 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? N # Y or N 'Break arcs at quadrants (changed from 'Y' to'N")

UppercaseComments? Y # Y or N 'Require uppercase comments

Drill # Drilling canned/manual cycle
G81 Z[D] R[Vclear] F[FRate]
end cancel
# (Line "G[RetPlane] X[H] Y[V]" Taken out
# (From all Canned Cycles -26/1/2007-)
CSink
G82 Z[D] R[Vclear] F[FRate] P[Dwell]
end cancel

Peck # Pecking canned/manual cycle
G83 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 Z[D] P[Dwell] R[VClear] F[FRate]
else
G84 Z[D] R[Vclear] F[FRate]
Endif
end cancel

LTap # Left handed tapping cycle
G74 Z[D] R[Vclear] F[FRate] Q[VBite]
end cancel

Ream # Reaming canned/manual cycle
G85 Z[D] R[Vclear] F[FRate]
end cancel

Bore # Boring canned/manual cycle
G86 Z[D] R[Vclear] F[FRate]
end cancel

Back # Back boring canned/manual cycle
G87 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
%0
!0 O[Program#]
G17 G20 G40 G49 G54 G80 G90 G98
End

1stToolChange # First tool change
G0 x0.0 y0.0
T[Tool] M6 (0 e[ToolDiam] f[corner]
Comments
G0 X[H] Y[V] # "G90 G[Work]" Taken out
G43 H[Lcomp] Z[D] M03 M08 S[Speed]
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
G28 G49 Z0.0 M19
M1
T[Tool] M6 (0 e[ToolDiam] f[corner]
Comments
G0 X[H] Y[V] # ("G0 G[Work] X[H] Y[V]" Taken Out -26/1/2007-)
G43 Z[D] H[Lcomp] M03 M08 S[Speed]
End

EndCode # End of the program
M9
G28 G49 Z0.0 M19
G28 Y0.0
M30
%0
End

replace "d" with "Rad: " # (Brought down to short name -26/1/2007-)
replace "e" with "T DIA: "
replace "f" with "C RAD:"

[JimW]

You need the ) 00 after the ( 00

Then try changing this line

T[Tool] M6 (0 e[ToolDiam] f[corner])

to this

T[Tool] M6 (0 e[ToolDiam] f[corner] )0

[yanzeek]

I think I did that but did'nt write the line )0 instead just ).
And shorten it to just ) 0 in the first part of post this way I had to just write (T[Tool] M6 (0 e[ToolDiam] f[corner]) without 0 after it. Will try exctly as you saying and see the result.
Thanks for the help, really appreciated.

[yanzeek]

Originally Posted by JimW You need the ) 00 after the ( 00 Then try changing this line T[Tool] M6 (0 e[ToolDiam] f[corner]) to this T[Tool] M6 (0 e[ToolDiam] f[corner] )0

Now the result I got was ( ) Tool Dia: 1 Rad: 0
Any idea why?
What is the language these Posts are written in? Any web site link? so I can learn, I have done Oracle in the past so I know the concept.

[yanzeek]

Thanks a lot guys for help. Lost my job anyway. The boss was looking for some kind of his right hand and I am not close to his pinki. I know I am not stupid or geek, but it gets tough when I have to work with ppl stuck in 80's and use DOS virsion cnc software.
I solved the issues they had with surfcam, in the mean time I was editing the NC files in note pad (like everyone there), and now the programs are posting flawless, ready to run on machine. Maybe my job is done fixing the bugs they had which I dont think was a big deal.
Now I am back to looking for job..

[CADGUY7]

I'm sure this should be a new thread but, I'll darned if I cant find the link to start one....

I have two post templates fanuc dam 0t.L and fanuc dam 10t.L
This is how it looks in the post.ini file:

[LPOST]
Format C:\SURFCAM\POSTLIB\fanuc dam 0t.L
AutoOpen? Yes

Format C:\SURFCAM\POSTLIB\fanuc dam 10t.L
AutoOpen? Yes

When I open the NC Operations manager the two templates are listed. But only the second template is selected regardless of which I select in the Operations manager... its got to just be a matter of syntax. Can anyone point out my error(s)?... Thank you for the help.

Here is the lathe section of surfcam.pst.

BeginPost Lathe Default:1
PostItem Fanuc D.A.M. 0T
Status Fanuc D.A.M. 0T
ChDir "C:\SURFCAM\Velocity3\MPOST"
Delete "%p%N.TAP"
Command "C:\SURFCAM\Velocity3\MPOST\LPOSTWIN" "%p%N"

PostItem Fanuc D.A.M. 10T
Status Fanuc D.A.M. 10T
ChDir "C:\SURFCAM\Velocity3\MPOST"
Delete "%p%N.TAP"
Command "C:\SURFCAM\Velocity3\MPOST\LPOSTWIN" "%p%N"
EndPost


Oh, I am using PostHaste.
Thanks again

[NICK REESE]

Cadguy7,

Try changing this line in the first item:

Command "C:\SURFCAM\Velocity3\MPOST\LPOSTWIN" "%p%N"

to:

Command "C:\SURFCAM\Velocity3\MPOST\LPOSTWIN" "%p%N" 01

and the same line in the second item to:

Command "C:\SURFCAM\Velocity3\MPOST\LPOSTWIN" "%p%N" 02


good luck,

nick.

P.S. I forgot to say, the 01 and 02 should reflect the position of each post in the postform.l file.