Printable View
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
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.
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
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
Code: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"
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
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.
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
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
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. *
*
I give it a try later in week.Quote:
%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
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. ;)
Code:
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)"
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
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
Team-Mgn What kind of company is that by the way? :violin:
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
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
Thanks for the comment got lost trying to make it work and also trying to visualize
tool position.
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.
OK
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
This is the stock one straight out of the library.Code: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