Need Help!- G65 P9510 A0 B18.5 C16. D81. R.1 Z-2.00 F6.7 W98.

[casta-baga]

G65 P9510 A0 B18.5 C16. D81. R.1 Z-2.00 F6.7 W98.

G65 = calls the P
P = macro
A = starting angul
B = diameter
C = number of holes to be drilled
D =
R = returning point in canne cycle
Z = depth
F = feed
w =

bolt circle programming that the previous programmer left me, I'm used to
work with a software and generate the codes but this looks more advanced...

can anyone please let me know what means the D and W

thanks

[psychomill]

If I had to guess...

D = cycle type like "G81"
W = Clearance plane select like "G98"

Without seeing the macro itself though, not 100% sure. You need to post the sub routine (program number O9510) and any other sub calls it might have.
The only thing is that if I'm right, it seems awfully strange to have to write a drill macro like this when a standard canned cycle call can do basically the same thing. Maybe there's more to the macro? This might be a pattern macro. Anyway... need to see the macro....

[casta-baga]

this is it.....

%
O9510(BOLT CIRCLE MACRO)
#2=#2/2
#1=#1-[360/#3]
N10#11=#11+1
#1=#1+[360/#3]
M1
IF[#11GT#3]GOTO20
#15=#25+[SIN[#1]*#2]
#16=#24+[COS[#1]*#2]
G#23G#7X#16Y#15R#18Z#26Q#17F#9
GOTO10
N20G80M99
%

my question is, can I just edit the main PGM (G65P9510A0B18.5C16.D81.R.1Z-2.00F6.7W98.)
withe a new A,B,c and Z values?

[samu]

psychomill is right, D is drill cycle and W is retract plane selection. You can change A B C and any value you want in the G65 line (except G65 and P9510) But, after reading macro, I can tell you that you have to add X (x coordinate of bolt circle center) and Y(y coordinate of bolt cicle center) in the G65 line.

[casta-baga]

Originally Posted by samu psychomill is right, D is drill cycle and W is retract plane selection. You can change A B C and any value you want in the G65 line (except G65 and P9510) But, after reading macro, I can tell you that you have to add X (x coordinate of bolt circle center) and Y(y coordinate of bolt cicle center) in the G65 line.

hello guys,
I understood that if I change the A B C values in the G65 line I do have to add a X -.- and Y -.- in the same line.

I'm I right or not?

hey guys...
good weekend

[stevo1]

You do not need to add the X,Y in the G65 line you can just specify G54-G59 in your macro program(these being set to the center of your part). If you choose not to use the G54-G59 then you have to do as Samu said and put the X,Y center of part in the G65 line. Given the fact that you did not post a X,Y value in the first post and the macro shows no G54-G55 value in it I would assume that the previous programmer was using G54 defualt for every part. This is being programmed off the center of the part and the X,Y location for the holes are triged out in the macro with the (SIN & COS). You can change all of the values in the G65 line except the P for the program. Change these to fit what you need. Don’t forget the Q value in the G65 line. This is your pick value. This will be used if you use a G73 or G83 peck cycle for your “D” value. If you are not using these cycles just set Q0.

I typically never use the G98 in the macro call. My control is set as G98 default. If you always want G98 either have your control default to this or hard code it right in the macro. It is just one less number you have to set in the program then.

What kind of control are you using??

Stevo

[casta-baga]

I got it all, thank you guys.

I'm already thinking about getting some books from the library on this topic and etc...

seicos control

[stevo1]

Seicos controls are pretty user friendly and similar style to Fanuc programming.

Is that all of the macro that you posted in post #3? There should be more to it. I would have went a little different style but all in all the same. There should be something for a clearance plane(initial level). A few other things as well.

I have all my VMC work written in the style of that macro. However I set up S&F's in 1 program for all tools so you don't have to program that in the macro line. If you are intrested I have programs for tapping, threadmill, counterbore, single flute thread, backchamfer,ect. all in the same style as what you have. I also have all of these programmed for a rotary axis.

Stevo

[casta-baga]

Yes Seicos controls are pretty user friendly; with my Fanuc experience I can learn these machines very easy.

I posted all the macro, I notice some programs are using the exact same macro for tapping; I also got macro for chamfering, set the tools, probing, tool change and etc….

I’m curious about your macro; can you please post it with the initial level plane and etc?

I think I’m interested on those macros you got for tapping, threadmill, counterbore, single flute thread, I’m very curious, I like to learn new things all the time.



[stevo1]

A=number of holes
C=starting angle
K=G-code for drilling
D=angle between holes
R=radial distance of holes
Q=pick size
W=starting depth
T=tool number
Z=final depth
U=next tool(pre call)
M=coolant code


O0001(MAIN PROG.)
#525=3.(CLEARANCE PLANE)
G65P8000A12C0K81D30R9.25Q0W.05T5Z1.3U12M8
M30

O8000(RAD. DRILL)
M6T#20
T#21
G90G80
#2=SIN[#3]*#18
#4=COS[#3]*#18
G55G0X[#24+#4]Y[#25+#2]Z#525M3
#10=0
#11=#3
#12=#11
N1#2=SIN[#11]*#18
#4=COS[#11]*#18
G#6X[#24+#4]Y[#25+#2]Z-#26R#23Q#17M#13
#10=#10+1
#16=#7*#10
#11=#12+#16
IF[#10NE#1]GOTO1
G80M9
#3006=10(CHECK HOLE WITH GAUGE)
M99

Speeds & Feeds are set in a sperate program that way they only have to be changed 1 time. This program is called with every tool change. The H-value's are also set in the tool change macro with no tool movement. The M6 code is bypassed if the tool being called is already in the spindle. The reason I use #525 for the clearance plane(initial level) instead of using a variable(A,B,D,R ect) is because if you write a macro line and forget the clearance plane in the line it will not have a clearance. Variables #1-#33 are cleared at reset. #100-#199 are cleared at power down. #500-#999 stay until changed.

I will post more programs.

Stevo