[Steven74]

Hello everyone,
I have a problem with a G81 in a program and I cant quite figure it out. Im drilling out a .50" through hole in a 1.50" block. The .50" hole is within another hole or pocket. The tool does not seem to be retracting to the Initial Z and I'm not sure why. Any ideas? Here is the code and a picture of the drawing of the part.
(T5)M09
G0G91G28Z0
M6T5
G90G54.1P20Y-2.25X2.S3000T23M3
G43H5Z.1M18F30.
G98
G81R-1.625Z-1.650
G54.1P19Y2.25X2.
G54.1P17Y2.25X2.
G54.1P18Y-2.25X2.
G54.1P16Y-2.25X2.
G54.1P15Y2.25X2.
G54.1P13Y2.25X2.
G54.1P14Y-2.25X2.
G54.1P12Y-2.25X2.
G54.1P11Y2.25X2.

[chucker]

Try putting your G98 on the same line as your G81 thats the way I have always done it may not make any differance

[Steven74]

Thanks, I'll give it a try.

[sinha_nsit]

The program does not seem to exactly correspond to the drawing you supplied.
Where is Z0? If it is on the top surface, R-value is incorrect. The tool would plunge into the workpiece at rapid rate.
Any specific reason why you use so many G54.1's?

[fordav11]

Hmmm. A very strange program indeed.
I don't think you can change workshifts in the middle of a canned cycle like that.

R is an incremental distance from the initial level to the R level.
Your R-1.625 would rapid to Z-1.525. Unless your mill is a punching machine that would not be a good move ;-)

With Z0 being the top of the block and using just one workshift the G81 should go something like this......

G90 G98 G81 X2.0 Y–2.25 Z–1.65 R–1.25 F30.
X2.0 Y2.25
X Y
X Y
X Y
X Y
X Y (etc)
G80

The initial level is set to Z0.1 so R-1.25 rapids to Z-1.15


if you have to use multiple workshifts put the drilling in a sub program and call it like this.....

%
O0001 (MAIN)
G40 G80 G91 G28 Z0
M6 T5
S3000 M3
G54.1P20
G90 G0 X2.0 Y-2.25
G0 G43 H5 Z.1 M18
M98 P0002
G54.1P19
M98 P0002
G54.1P17
M98 P0002
G54.1P18
M98 P0002
G54.1P16
M98 P0002
G54.1P15
M98 P0002
G54.1P13
M98 P0002
G54.1P14
M98 P0002
G54.1P12
M98 P0002
G54.1P11
M98 P0002
G28 G91 X0 Y0 Z0
M30
%

%
O0002 (SUB)
G90 G98 G81 X2.0 Y–2.25 Z–1.65 R–1.25 F30.
Y2.25
G80
M99
%

This example assumes you have no other obstacles like vice, clamps etc in the way of XY rapid movements. The XY rapids are at Z0.1
If you do have obstacles and you need to clear them before XY rapids, change the line with G43 to set the initial level higher up.
i.e.
G0 G43 H5 Z10.0 M18
and adjust the R- to suit.


Have a look at the G81 pages (from Fanuc manual) for an explanation of the format for G81.....

[chucker]

You can change the work offsets on the fly as the Op has it I do this a lot for muti part setups he did not state the control type but on my fanucs his program would work it would rapid to the Z.1 then read the G81 line and rapid to the -R value after drilling with a G98 it should rapid back up to the
z.1 which G98 is default on my on my machines if the G99 was used it would have came back up to the R plane also you can change the Rs and Zs with in a G81 as needed for different depths or R values for different surfaces on a part if you are changing the Rs around watch that you dont drag across a part some where and use G98 or G99 in the right place. his program may run into the part but I thought he said there was already a hole there he was going down into.

[fordav11]

yeah he said he's doing the smaller hole at the bottom and it's within a larger hole so we could assume the larger hole/pocket is already machined. but his R-1.625 would rapid into solid material. Not good.....

[Steven74]

The controller is a fanuc series 16 on a Monarch 150. The top of the block is Zero. The multiple G54's are for the vises which there are 10 vises on each pallet. Im having difficuly understanding how this canned cycle deal works in between moves from vise to vise. I have a ABB robotic programming background and CNC is all new to me.

The first hole in the block (large hole) is drilled out first with a carbide insert drill down to 1.125" then drill our the .500" hole in the center.

Thanks for the feedback and for the imfo on the G81 and G82.

[chucker]

I think fordav11 has it right in his exzample.

Quote:

With Z0 being the top of the block and using just one workshift the G81should go something like this......

G90 G98 G81 X2.0 Y–2.25 Z–1.65 R–1.25 F30.
X2.0 Y2.25
X Y or your G54.1s
X Y
X Y
X Y
X Y (etc)
G80

[Steven74]

Thanks for the help. Its making a little sense now.

[Steven74]

What would happen if the canned cycle was not canceled out before going to the next process which has a different canned cycle?

[chucker]

if there were no G80 given then the control would think the can cycle was still active and give you an alarm or try to drill and the next set of coordinates in the program or alarm out depending what code was next.

[Steven74]

OK, good to know. I read somewhere that G0 cancels out canned cycles. Is that true for fanuc controllers?

[chucker]

That may be true but I have not tried that I always use the G80

[sinha_nsit]

IIRC G00, G01, G02, G03 all cancel the canned cycles.
But what is the harm in using G80 if you want to cancel it.

[fordav11]

what you need to do is pretty stock-standard.
just make the initial level higher up to clear anything as per my example.
if you use my main/sub example the cycle is cancelled before going to the next G54.x
it's good practice to always cancel a cycle when you have finished with it or you can
get unexpected results.

[Steven74]

OK, Thanks to everyone for there help.