I Know it Has Been Beat to Death, But Fanuc G41/42 Questions

alphonso · Apr 19, 2017

Fanuc 18MC, Cutter Compensation "C".

Program for threadmilling. New threadmill is slightly smaller OD(.347 as opposed to .35), thus threads are too tight. Thought that we would add comp to program rather than re-post or calculate how much to change values.

Not having any luck, keep getting 034 error.

So, can somebody show me what and where to add G41, D value(112), and G1 lead in? The X-1 Y0 is the position to start threadmilling the first hole.

N310 T12 (1/2 X 13 THREADMILL) M6
N320 G54
N330 G0 G90 X-1.0 Y.0 S4365 M3
N340 G43 Z.2 H12 T15
N350 G72.2 P0071 L3 I1.
N470 M09
N480 M05
N490 G28 G40 G91 Z.0 M09
N500 G28 Y.0
N510 G90
N520 M30

:0071 (SUB FOR 0070)
N370 G1 Z-.8192 F13.1 M8
N380 G3 X-.9435 Y.0 Z-.8 I.0283 J.0 F3.1972
N390 G3 X-.9435 Y.0 Z-.7231 I-.0565 J.0
N400 G40 G3 X-1.0 Y.0 Z-.7038 I-.0283 J.0
N410 G1 Z-.8192 F13.1
N420 G3 X-.9225 Y.0 Z-.8 I.0388 J.0 F4.0208
N430 G3 X-.9225 Y.0 Z-.7231 I-.0775 J.0
N440 G3 X-1.0 Y.0 Z-.7038 I-.0387 J.0
N450 G0 Z.2
N460 M99

Larry Dickman · Apr 19, 2017

alphonso said:
Fanuc 18MC, Cutter Compensation "C".

Program for threadmilling. New threadmill is slightly smaller OD(.347 as opposed to .35), thus threads are too tight. Thought that we would add comp to program rather than re-post or calculate how much to change values.

Not having any luck, keep getting 034 error.

So, can somebody show me what and where to add G41, D value(112), and G1 lead in? The X-1 Y0 is the position to start threadmilling the first hole.

N310 T12 (1/2 X 13 THREADMILL) M6
N320 G54
N330 G0 G90 X-1.0 Y.0 S4365 M3
N340 G43 Z.2 H12 T15
N350 G72.2 P0071 L3 I1.
N470 M09
N480 M05
N490 G28 G40 G91 Z.0 M09
N500 G28 Y.0
N510 G90
N520 M30

:0071 (SUB FOR 0070)
N370 G1 Z-.8192 F13.1 M8

Your G1 G41 D112 line should go here. You need a linear move
try this
G1 X-.980 Y0
G1 G41 D112 X-1.0 Y0

N380 G3 X-.9435 Y.0 Z-.8 I.0283 J.0 F3.1972
N390 G3 X-.9435 Y.0 Z-.7231 I-.0565 J.0

N400 G40 G3 X-1.0 Y.0 Z-.7038 I-.0283 J.0
Cant have G40 on a G3 line, do a lead out same as the entry in reverse
G1 G40 X-.980 Y0
g1 X-1.0 y0

and then the same thing on this pass
N410 G1 Z-.8192 F13.1
N420 G3 X-.9225 Y.0 Z-.8 I.0388 J.0 F4.0208
N430 G3 X-.9225 Y.0 Z-.7231 I-.0775 J.0
N440 G3 X-1.0 Y.0 Z-.7038 I-.0387 J.0
N450 G0 Z.2
N460 M99

too short?

alphonso · Apr 19, 2017

Where the fuck did the G40 come from? Edgecam strikes again. I have 5 other programs associated with this project with threadmilling in them and none of them stick G40 anywhere.

I have been operating on the assumption that the G41 should be called in the main program rather than the sub. My thinking is:

N310 T12 (1/2 X 13 THREADMILL) M6
N320 G54
N330 G0 G90 X-1.0 Y.0 S4365 M3 <-------- Change to X-.980(or X-1.02) Y.02
N340 G43 Z.2 H12 T15

G1 G41 H112 X-1. Y0 F.1 <--------- Insert

N350 G72.2 P0071 L3 I1.
N470 M09
N480 M05
N490 G28 G40 G91 Z.0 M09
N500 G28 Y.0
N510 G90
N520 M30

Wouldn't this work if I get rid of the G40 in N400?

TeachMePlease · Apr 20, 2017

This is gonna sound dumb, especially because it ran before you tried to add comp... But is there a reason your height offset (T12) and your D offset (T15) don't match?

Booze Daily · Apr 20, 2017

H12 T15. Staging the next tool.

TeachMePlease · Apr 20, 2017

Booze Daily said:
H12 T15. Staging the next tool.

Gotcha. Don't get/need to do that on a Swiss, been awhile since I was on a mill haha.

ghost_rider · Apr 20, 2017

It looks like it has an arc in as well as a arc out with no straight line.

Try this for your sub. I just wrote it out long hand the way I do most of my thread mill cycles. Make sure you use the D you need in there for your tool size.

:0071
G1Z-.8192F13.1
G1G91G41Y-.211 F3.1972
G03X.250Y.211I.0031J.25Z.0192
G03X0.Y0.I-.250J0.Z.0769
G03X-.250Y.211I-.2469J-.039Z.0192
G1G40Y-.211
G1G90Z-.8192F13.1
G1G91G41Y-.211 F3.1972
G03X.250Y.211I.0031J.25Z.0192
G03X0.Y0.I-.250J0.Z.0769
G03X-.250Y.211I-.2469J-.039Z.0192
G1G40Y-.211
G0G90Z.2
M99

gorrilla · Apr 20, 2017

alphonso said:
Where the fuck did the G40 come from? Edgecam strikes again. I have 5 other programs associated with this project with threadmilling in them and none of them stick G40 anywhere.

I have been operating on the assumption that the G41 should be called in the main program rather than the sub. My thinking is:

N310 T12 (1/2 X 13 THREADMILL) M6
N320 G54
N330 G0 G90 X-1.0 Y.0 S4365 M3 <-------- Change to X-.980(or X-1.02) Y.02
N340 G43 Z.2 H12 T15

G1 G41 H112 X-1. Y0 F.1 <--------- Insert

N350 G72.2 P0071 L3 I1.
N470 M09
N480 M05
N490 G28 G40 G91 Z.0 M09
N500 G28 Y.0
N510 G90
N520 M30

Wouldn't this work if I get rid of the G40 in N400?

As to whether it would work or not, I don't know.But I would put G40 in the line before G90. I always do. Should cancel it out when it hits M30 I think, but I always call for the control to cancel tool offsets. Seems like I had it NOT cancel one time. Pulled quite a bit of hair(that I can't AFFORD) out on that one, and it may have even been on THAT exact machine.
But you are correct, that is the most glaring error I see. And I missed it as well, reading the OP. As you said, Edgecam strikes again.

tay2daizzo8 · Apr 21, 2017

You can actually comp a threadmill? Ive been edditing I Values for years hoping i dont fat finger 1 wrong number

ghost_rider · Apr 21, 2017

tay2daizzo8 said:
You can actually comp a threadmill? Ive been edditing I Values for years hoping i dont fat finger 1 wrong number

yes you can comp a threadmill. been doing it for years.

Search

Largest Manufacturing Technology Community on the Web

Search

I Know it Has Been Beat to Death, But Fanuc G41/42 Questions

alphonso

Titanium

Larry Dickman

Titanium

alphonso

Titanium

TeachMePlease

Diamond

Booze Daily

Titanium

TeachMePlease

Diamond

ghost_rider

Aluminum

gorrilla

Stainless

tay2daizzo8

Hot Rolled

ghost_rider

Aluminum

Similar threads