Surfcam Post

[RICK B.]

My company is buying an Okuma Lathe (LB3000 EX MYW) with an OSP-P200LA controller. I was wondering if anyone has access to a post for surfcam?
I contacted Surfcam, waiting on a reply back but don't want to reinvent the wheel. I would like to get a post that is close. Thank you, Rick

Similar Threads:

• Surfcam Post Citizen
• Surfcam post?
• Surfcam post for g71

[Anders6612]

Here, you have two good manuals, especially the Posthaste.
An ordinary post is easy to configure:

http://www.cadfamily.com/Download.as...rial&ID=297266

https://engineering.purdue.edu/AAE/A...Processing.pdf

But if you send me a file with prefered toolchange, start and end. Cycles etc, maybe i can help you.

[Jerseycnc]

Just happened to read your thread and I also was in need of a post for a Fagor 8025TG
retrofit on a hardinge-gang tool lathe. As you suggested to the other guy;I downloaded 1st PDF but cant get the 2nd. !st time dealing with a lathe and would rather not hand program. Any thoughts !!
would be appreciated

JC

[Anders6612]

Are you using x- in the machine?
I am not sure about the post, and i have not fixed the cycles.
I might need some sample from you, especially tool change. (position)

Based from: http://www.cms-cnc.com/901-2025.pdf

Postform.l

name Fagor 8025TG (Inch)

% 00
O 5
N >3
G >2
X ->3.>4
Z ->3.>4
D 2
I ->3.>4
K ->3.>4
U ->3.>4
W ->3.>4
P ->3.>4
C ->3.>4 Mult 2
J ->3.>4
A 60 P
Q ->4.>3
q >4 Q
R ->3.>4
S >4
T >2
t >2
i 2
F >3.>6
M >2

ModalLetters X Z F M R P S

ModalGs 0 1 2 3 4 73 76 80 81 82 83 84 85

First#? N
Sequence#s N 1 10 10
Comment ( )

HCode Z
VCode X
FeedCode F

Spindle 3 4 5
Coolant 8 9 8
SpeedType G 97 96
FeedType G 95 94
Dcomp 41 42 40

ByDiameter? Y
RevX? N
CtrIncremental? Y
Inc/Abs G 91 90
Inch/MM 20 21
CtrCode K I

Sbackdoor Supressheader

Feed G<1>
Rapid G<0>
Cw G<3>
Ccw G<2>

Leading0s? Y

UppercaseComments? N

StartCode
%<0> O<Program#>
end

1stToolChange
G92 S<Val1>       # Max rpm at G96
G90 G<FeedType> G<SpeedType> S<Speed> T<Tool> t<Tool> M<Direct>
G<0> X<V>
Z<H>
End

Linecode
G<1> X<V> Z<H> F<FRate> M<Cool>
end

Infeed
G<1> G<Side> X<V> Z<H> F<FRate> M<Cool>
end

Outfeed
G<1> G40 C<V> J<H>  # C and J non modal for X and Z
end

ToolChange
i1         # 1 inch safety position and cooling off
M1
G92 S<Val1>       # Max rpm at G96
G90 G<FeedType> G<SpeedType> S<Speed> T<Tool> t<Tool> M<Direct>
G<0> X<V> 
Z<H>
End

EndCode
i2            # 1 inch safety position, spindle and cooling off
M30
End

Drill
G<74> R<Depth>
G<74> Z<Depth> F<FRate>
end

Tap
G<84> Z<H> F<FRate>
end cancel

Ream
G<85> Z<H> F<FRate>
end cancel

Bore
G<74> R<0>
G<74> Z<H> R<SClear> F<FRate>
end

AutoThread
G<76> A<TParams> Q<VBite> R<0>
G<76> X<V> Z<H> R<StartAng> P<Depth> q<Peck1> F<Frate>
end

Cancel
i1      # 1 inch safety position and cooling off
end

Ask <Val1> "Max Rpm" "500"

Replace "% " with "%"
Replace " t" with "."
Replace "O" with ""
Replace "C" with "X"
Replace "J" with "Z"
Replace "i01" with "G0 Z1. M9"
Replace "i02" with "G0 Z1. M5 M9"

[Jerseycnc]

Find attached a program just changed extension to a .txt from .ncc
Yes using X-..I edit it to speed it up
This program was hand written as a turnkey and explained to my Boss
that posting is consistant and alot quicker to do new parts. Again its a
gang tool lathe..

JC

[Anders6612]

G5 and G7, is it round and square corners?
When, or with what tool do you use it,
or do you want to select it at posting?

It is quite a difficoult post, i also have to figer out about the X-
I think i can fix that with questions at posting to.

[Jerseycnc]

I can send you an IGS file.
Its a gang tool lathes.
As far as tools I would pick them at posting but will be using same all the time..Just got in will send soon. Thanks

JC

[Jerseycnc]

Here is the sample part in IGS format and info on tooling stated in a text file. I hope this helps. And definitely
appreciate the help. First time doing Lathe work. I'm Ok doing mill but of course not going to help now.

JC

[Anders6612]

Ok, so these 2 tools are the only ones to go X-?
I think i need toolnumbers for all X- tools.

Aso, what cycles do you use, (Drill, peck tapping) any examples?
And the start of the program, is that to be all the same, with
collet etc. *

*

%01001
N10 (REVISED RB 6/21/12)
N11 (THIS PROGRAM SAME AS 01000)
N12 (ONLY CHANGES MADE IN IPR)
N13 (AND RPM TO SPEED PROGRAM TIME)
N14 G0 G90 G70 G7 T2.2
N15 G53 (OFFSET)
N16 G0 X.25
N17 (Z.15 ORIGINAL Z OFFSET)
N18 G0 Z.110 (NEW Z OFFSET)
N19 M0 (PULL PART TO STOP AND CLOSE COLLET)
N20 G0 Z.35

I give it a try later in week.

[Anders6612]

Try this for your turning tools, if i guess right you use only T1 and 2
for outside turning?

I am not sure about Gside and Interpolation at RevX,
and you have to draw and process your work normal in
Surfcam, (X+) it dont seem to work smowley to draw in X- as your example show.

As the post is made now, T1 and 2 (only outside) is going to be RevX and Gside
(Nose radius Compensation) is reversed.
Your offset is set to ask you, and Collet is set to close and open with
M10 and M11. Also i added max rpm for G96, if you use that. G5 ang G7 for
rough and precision is also added. But why G53 only?
Never use G54?

Gome back, i am probebly not finished.

name Fagor 8025TG (Inch)

% 00
O 5
N >3
j 2
G >2
X ->3.>4 Mult 2
Z ->3.>4
B ->3.>4 Mult 2
E ->3.>4 
D 2
I ->3.>4
K ->3.>4
U ->3.>4 Clamp 0.001 0.3
W ->3.>4
P ->3.>4
C ->3.>4 Mult 2
J ->3.>4
A 60 P
Q ->4.>3
q >4 Q
R ->3.>4
S >4          # SET YOUR SPEED LIMIT. EX: S >4 Limit 20 6000 
T >2
t >2
i 2
F >3.>6    # SET YOUR FEED LIMIT. EX: F >3.>6 Limit 0.0001 15 
M >2
u 2

ModalLetters B E X Z F M R P S

ModalGs 0 1 2 3 4 40 41 42 70 73 76 80 81 82 83 84 85

First#? N
Sequence#s N 1 1 10
Comment ( )

HCode Z
VCode X
HCode2 E
VCode2 B
RevSigns B
FeedCode F

Spindle 3 4 5
Coolant 8 9 8
SpeedType G 97 96
FeedType G 95 94
Dcomp 41 42 40

CtrIncremental? Y
Inc/Abs G 91 90
CtrCode R

Sbackdoor Supressheader

Feed G<1>
Rapid G<0>
Cw G<3>
Ccw G<2>

Leading0s? N

UppercaseComments? N

StartCode
%<0> O<Program#>
end

1stToolChange
if <Tool> = 1 or <Tool> = 2    # TOOLS TO GO REVX
set <Turret> to 2
else
set <Turret> to 1
endif
i4
M1
if <Tool> = 1
j1 G7 T<Tool> t<Tool>      # G7 BLOCK DECELERATION CHECKING ON
endif
if <Tool> = 2
j1 G5 T<Tool> t<Tool>      # G5 BLOCK DECELERATION CHECKING OFF
endif
if <Tool> <> 1 and <Tool> <> 2  # TOOLS NOT TO GO REVX
j1 T<Tool> t<Tool>
endif
j2
set <Val2> to 0.11
U<Val2>
i3
M10 u1                     # COLLET CLOSE. REMOVE THIS LINE IF YOU DONT WANT IT
G0 Z.35
if <SpeedType> = 96
Ask <Val1> "Max Rpm" "1000"
G92 S<Val1>
G<FeedType> G<SpeedType> S<Speed> M<Direct>
else
G<FeedType> G<SpeedType> S<Speed> M<Direct>
endif
G<0> X<V>
Z<H> F<FRate>
End

Linecode
G<1> X<V> Z<H> M<Cool>
end

Infeed
if <Tool> = 1 or <Tool> = 2
set <Side> to 41
endif
G<1> G<Side> X<V> Z<H> M<Cool>
end

Outfeed
G<1> G40 X<V> Z<H> 
end

ToolChange
if <Tool> = 1 or <Tool> = 2
set <Turret> to 2
else
set <Turret> to 1
endif
i1
M1
if <Tool> = 1
j1 G7 T<Tool> t<Tool>     
endif
if <Tool> = 2
j1 G5 T<Tool> t<Tool>    
endif
if <Tool> <> 1 and <Tool> <> 2
j1 T<Tool> t<Tool>
endif
G53
if <SpeedType> = 96
G92 S<Val1>
G<FeedType> G<SpeedType> S<Speed> M<Direct>
else
G<FeedType> G<SpeedType> S<Speed> M<Direct>
endif
G<0> X<V>
Z<H> F<FRate>
End

EndCode
i2 
M11 u2              # COLLET OPEN. REMOVE THIS LINE IF YOU DONT WANT IT
M30
End

Drill
G<74> R<Depth>
G<74> Z<Depth> F<FRate>
end

Tap
G<84> Z<H> F<FRate>
end cancel

Ream
G<85> Z<H> F<FRate>
end cancel

Bore
G<74> R<0>
G<74> Z<H> R<SClear> F<FRate>
end

AutoThread
G<76> A<TParams> Q<VBite> R<0>
G<76> X<V> Z<H> R<StartAng> P<Depth> q<Peck1> F<Frate>
end

Cancel
i1
end

Ask <Val2> "Wp offset?" ".11"      # WP OFFSET. REMOVE THIS LINE IF YOU DONT NEED IT. DEFAULT IS .11 

Replace "% " with "%"
Replace " t" with "."
Replace "O" with ""
Replace "B" with "X"
Replace "E" with "Z"
Replace "U" with "Z"
Replace "i01" with "G0 Z1. M9"
Replace "i02" with "G0 Z1. M5 M9"
Replace "i03" with "M0 (PULL PART TO STOP AND CLOSE COLLET)"
Replace "i04" with "G0 G53 Z1."
Replace "j01" with "G0 G90 G70"
Replace "j02" with "G0 X.125"
Replace "u01" with "(COLLET CLOSE)"
Replace "u02" with "(COLLET OPEN)"

[Jerseycnc]

I will give a try assisting with more info I only have one program (hand written) to work from and thats
the one I sent you. I have no examples of dril,peck or tapping. The gang lathe at this point will only have tools 1and 2 and this clamping device which is tool 3. Im attaching info that may assist. G53 not sure why
It seems nobodys fault each programmer writes a different way. Thats why these issues. I will get back.
Thks again
JC

[mariojl]

Hi there:
I just get here, and after seeing the pictures you posted, I realized why the problems having to use Turn ID in the OD and going on with the post.
You are drawing the part backwards. No matter what kind of machine you have. It can be a parallel, gang-tool, turret, or vertical lathe; SURFCAM is configured in such a way that you MUST draw your job from X 0 towards the plus direction; and then let the post-processor take care of changing directions, like X…..Mult -1.
If you do this, SURFCAM will care about your Side (G41-42), nose radius compensation, interpolation and so on.
You are doing a good job in the post with many IF – Then that really don’t need, SURFCAM will cover all that.
Kind regards
Mario

[Anders6612]

Team-Mgn What kind of company is that by the way?

[Jerseycnc]

Mario,
Thanks for the response back, appreciate the comments. I tried the post and got an error which I sent you as a JPG for you to read. Just to let you know the previous post that you had up earlier in your first thread I tried it and posted out. I may be doing something wrong with this one not sure..

JC

[Jerseycnc]

Mario,
Thanks for the comment I got carried away with the visual on the backplot. I tried the post and recieved an error. I sent it as a jpg for you to read. The first post you had up on the thread (8025TG inch) I tried and it posted out.
I may have done something to cause error - not sure.

JC

[Jerseycnc]

Thanks for the comment got lost trying to make it work and also trying to visualize
tool position.

[Anders6612]

You probebly removed the space betwen % and 0
at format, in line 2.

This is right

name Fagor 8025TG (Inch)

% 00

This is wrong

name Fagor 8025TG (Inch)

%00

Spaces is very important in the post, no space, no posting and
one to mutch, wrong code.

Mirror your work and process in X+ direction, that is the way to go.
The post will reverse the code for tool 1 and 2 only.

[Jerseycnc]

OK

[bad69]

I'm new to cnc programming and I need a siemens 810 post processor for surfcam v4.
Any sugestions?

Sent from my GT-S7710 using Tapatalk

[Billetgrip]

name Siemens 810M
      # Modified added RapidCode logic sequence 3/27/2014

% 00
/ 00
O >4
N >4
G >2
g >2 G
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

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 85  # List of g codes that are modal    

Sequence#s N 0 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                         # 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

ArcToLineWarnings? Y                        # Small Arc Warnings

MinArc .0099                                # MinArc Default = .0099
MinRad .005                                 # MinRad Default = .005   

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

CtrCode I J                           # I J or R or I J K L               
Helical? N

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  

UppercaseComments? Y                  # Y or N 'Require uppercase comments

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

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

Tap                                   # Tapping canned/manual cycle       
G84 X[H] Y[V] Z[D] R[Vclear] F[FRate] Q[VBite]
end cancel

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

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

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

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

Cancel                                # Cancel a canned/manual cycle      
G80
end

RapidCode                                   #(Include 'Z safety' logic)
Comments
 
IF [D] < [LastD]                            #Going down?
 G0 X[H] Y[V]                               #XY first, 
 Z[D]                                             #then Z.
 exit                                       
ENDIF
 
IF [D] > [LastD]                          #Going up?
 G0 Z[D]                                    # Z first, 
 X[H] Y[V]                                  # then XY.
 exit            
ENDIF

IF [D] = [LastD] 
G0 X[H] Y[V]
exit            
ENDIF
END

StartCode                             # Start of the program              
%0
O[Program#]
"(MACHINE: " {TemplateName} {TemplateExt} " MPOST Library)" 
G90 G80 G40 G17
End

1stToolChange                         # First tool change                 
T[Tool]
M6
M[Direct] S[Speed]
G90 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
g91 G28 Z0 M5
M1
T[Tool]
M6
M[Direct] S[Speed]
G90 G0 X[H] Y[V]
G43 Z[D] H[Lcomp]
M[Cool]
End

Upon [Speed]                                # Output spindle speed change
M[Direct] S[Speed]
End

EndCode                               # End of the program                
M9
g91 G28 Z0 M5
T[Tool1]
M6
G90 G0 X0 Y0
M30
%0
End

This is the stock one straight out of the library.