G41 and G42 How are works ?

[bunalmis]

Hello,

I am learning G codes but I didnt understand the G41, G42.

Who can teach to me these commands by example?

Bulent UNALMIS

[Klox]

It's offsets from the program line. When you're cuttining in a straight line (G01) is G41 offset to the left of the program line and G42 offset to the right of the program line. You must use D in conjunction with the G41 & G42 as the D value sets the amount of the offset. Eg: G41 G01 X10.0 Y25.0 D0.15, this translates to a offset of 0.15mm to the left of the program line.

Am I clear? If not Pm me and i'll e-mail you an example of a program.

Klox

[bunalmis]

Thanks Klox,

I add 2 examples. May you said which motion must use G41 or G42 ?

(Arrow numbers show sequence of motion)

[CAMmando]

Usually .....

A = G41
B = G42

But nothing would prevent a user from using them in reverse (in fact I worked in a shop that did just that). The operator just would put negative comp values in the register rather than positive and vice versa.

[Mortek]

In most fanuc based controls the D references a Diameter or radius entered into a registry page in the control. Hence if you called G41 D1 it would reference a pre-entered diameter or radius in register 1. Same goes for height offsets where you would call G43 H1 and that would select Height offset 1.

[cadcam]

Mortek , Most of the time Fanuc like to have a diffrent D value so more like T1 H1 G41 D21.

hope this helps just extra things to know.

[JamesBond]

Also an important thing to remember when manually programming G41/G42 is that before your cut, you need to enable the G41/G42 with a move that is at least 1/2 the cutter diameter. This also goes for turning off cutter comp with a G40.
You might get some unexpected results if you try to turn cutter comp on with your first cut.
-JamesBond

[wms]

Originally posted by cadcam Mortek , Most of the time Fanuc like to have a diffrent D value so more like T1 H1 G41 D21. hope this helps just extra things to know.

Cadcam,
I have to kindly disagree with your statment that most Fanuc or fanuc like controls like different number from your tool number.
I use the same offset as the tool number, have for about 15 years, never seen any problem.

You can use a different offset number, if you want to leave extra material, say for a finish pass.

So if you are using tool #1 that is a 1/2 mill, you could set offset #1 to .500 and use offset #21, set at .505 to leave .0025 material for clean up.

[HuFlungDung]

Originally posted by JamesBond Also an important thing to remember when manually programming G41/G42 is that before your cut, you need to enable the G41/G42 with a move that is at least 1/2 the cutter diameter. This also goes for turning off cutter comp with a G40. You might get some unexpected results if you try to turn cutter comp on with your first cut. -JamesBond

Good point, James.

BTW, for the uninitiated, this is what we machinists refer to as "an approach", that extra bit of toolpath that we add onto the actual part toolpath, to give the machine a chance to apply cutter compensation without forcing the tool into the wall of the part (gouging we call it), before the machine can figure out which side of the path it is supposed to be on. The reason the machine doesn't know how to apply compensation from a standstill, is that left and right are meaningless until a move is made down a path. In other words, there is no left or right to a starting point, but there is left or right to a starting movement.

A lot of this depends on how smart your controller is. If it can "look ahead" in your program before executing any movement, it may be able to apply compensation quite intelligently.

Nonetheless, at minimum, the machine is going to have to move your commanded amount from your compensation table before it is on path. Whether it makes this move all by itself when it reads a G41/G42, or combines it with the first linear/circular) movement, it has to do something to get the cutter in position. This is why the first entity in your path must be either "in the waste", or "in the clear".

[hardmill]

Originally posted by wms Cadcam, I have to kindly disagree with your statment that most Fanuc or fanuc like controls like different number from your tool number. I use the same offset as the tool number, have for about 15 years, never seen any problem. You can use a different offset number, if you want to leave extra material, say for a finish pass. So if you are using tool #1 that is a 1/2 mill, you could set offset #1 to .500 and use offset #21, set at .505 to leave .0025 material for clean up.

Sorry Wms,
I have to dissagree also. Fanuc controls are actually 50/50
in regards to using the same offsett. As far as multi passes
for finish thats what our cadcams are for. JM2C

PEACE

[wms]

Originally posted by hardmill Sorry Wms, I have to dissagree also. Fanuc controls are actually 50/50 in regards to using the same offsett. As far as multi passes for finish thats what our cadcams are for. JM2C PEACE

So maybe the word "most" should be "Some" or even "half".

I too agree that the cad/cam will handle the finish stuff. I was just giving an example of how different offset number and values could be used.

[cadcam]

I know that not all fanuc controls do it this way.
But at least half would be a btter statment from me.

As the last few years that most of the controls the customers keep telling me that they have to add 20 to the D value and that it can not be the same.

I know that the Yasda 5axis that has a Fanuc 16i control does not have to have a diffrent D as I have mentioned.

But most of the older ones do like the OM, 6M and many more have it this way.

So I have to do this again today and say I am sorry for a over statment.