View Full Version : Learning

Get lucky
11-19-2009, 12:21 PM
Little backgound

I have worked For this company for two years now. this is a fab company and they wanted to start a machine shop so they hired a guy to start it. He did an ok job of getting it up and going but never got the dnc going and never really made any money for the company.

So now for my part. As as I had said I have worked for this company for two years. When they hired me, my job was to get the shop making money. So i got the DNC hooked up and working and a way to save programs so they were not entering every program at the machine. Now the shop is making money and every one was happy. The owner has just found out that I had not be using surfcam and reamed my boss a new one. So here we go must learn a new cam system surfcam. I have went through the help section and I have played with the post with success of a few Programs that worked fine.

My only real question right now is when I tap in a fanuc It requires a M29Swhatever before the G84 so in the post I put the m29 before the g84 and it didn't work all my other edits to the post worked but not that one If anybody could tell me why that would be great.

Well done with my babling and back to work. I'm sure I will have more question to come thanks in advance to all help.

Thank you
Get Lucky

11-19-2009, 01:25 PM
I'm not sure what Fanuc you are using but I am running a mill with a 21-M controller. The machine is set up with rigid tap. If this is what you are trying to get to work, then this is part of the code that I use on my postform.m file:

Tap # Tapping canned/manual cycle
if [Rigid] > 0
G84 G[RetPlane] X[H] Y[V] Z[D] R[VClear] F[FRate]
G84 G[RetPlane] X[H] Y[V] Z[D] R[Vclear] F[FRate]
end cancel

and then under the "StartCode" section, I modified it to this:

1stToolChange # First tool change
G0 G30 Z0
if [Rigid] > 0
G00 G90 G[WORK] X[H] Y[V] T[NextTool]
G43 Z[D] H[Lcomp] M[Cool]
S[Speed] M[Direct]
G00 G90 G[Work] X[H] Y[V] T[NEXTTOOL]
G43 Z[D] H[Lcomp] M[Cool]

This machine is set up with the tool staging so you may have to remove the T[NextTool] to make it work on yours. I hope this helps.

Get lucky
11-20-2009, 01:30 PM
This is what i have for a post I'm not sure were I should put the code you posted.

Machine is fanuc OI-MC

% 00
/ 00
O 4
N >4
g 2 G
G 2
X ->3.>4
Y ->3.>4
y ->3.>4 Y
z ->3.>4 Z
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
S >4
M >2
m >2 M

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

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

CtrCode I J # I J or R or I J K L

Spaces? Y # Y or N 'Spaces between words

Helical? Y

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

Drill # Drilling canned/manual cycle
G81 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

StartCode # Start of the program

1stToolChange # First tool change
g00 g90 g40
g91 g28 z0
g91 g28
N100 M00
T[Tool] M6
G0 G90 G[work] X[H] Y[V] S[Speed] M[Direct]
G43 Z[D] H[Lcomp] M[Cool] T[NextTool]

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

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

ToolChange # Secondary tool changes
g28 g91 z1. M9
T[Tool] M6
N[Block] M01
T[Tool] m6
G0 G90 G[Work] X[H] Y[V] S[Speed] M[Direct]
G43 Z[D] H[Lcomp] M[Cool] T[NextTool]

EndCode # End of the program
g0 g28 z1. m9
g28 g91 y0
T[NextTool] m6
M99 P100