[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.

[wms]

Cadcam, Hardmill,
And I will have to say that I too am sorry for over (or under) stating what I said.

As I have not been exposed to controls that require what you are talking about.

Now we are all even and can start fresh.

[CAMmando]

I have to kindly disagree with your statment that most Fanuc or fanuc like controls like different number from your tool number.

The point is Alot of Fanuc (and other controls use the same "bank" of registers for H and D comp numbers. On these machines by definition either the H or the D can have the same number NOT both. It is customary to use T1 H1 D31 or 41 or 51 etc.

We have 1 control that has completely separate registers for D and H. On that machine T1 H1 D1 is OK.

Just to clarify ...

Regarding moves or leadins to apply comp. The statement that 1/2 the tool diameter is required is not completely accurate. You need enough of a move to apply the amount of comp in the register. You need at least the value in the comp register as a leadin. If the program is written to part dimensions then yes you need 1/2 the cutter. If the program is written to cutter centerline (wear comp) you only need enough leadin for the amount of comp expected. I usually allow .03-.05 for regrinds.

[Paul_S]

In Milling when the D word is needed for tool comp. I place the D word for the tool in the same block as the fixture offset and tool length offset.

For example:
G0G90G40G80T1M6(tool change)
G54X-0.28Y-1.28Z1.G43H1D1(call offsets and first position)
S4000M3(turn on spindle)
M8(turn of flood coolant)
G4P2000(2000 millisecond, i.e. 2 second dwell for spindle)
(notice only 1.00 above part.)
Z-0.28 (rapide to cut depth or Z0.1, next block G1Z-0.28)
G1G41X0F30. (comp into part dim, a 1/2 cutter was .25 + .03 clear)
Y0.03(part 1.00 wide, 0.03 off part)
G0G40X-0.28(turn off comp off part, tool radius + .03)
Z1.M5(clear part, turn off spindle)
G49H0Z0D0M9(cancel all offsets & coolant.)

To cancel the tool length offset ether the G49 or H0 will do.
The G40 canceled the D1, but the D0 clears the D word.
The G41 was offset to the left for climb cut. Use G42 offset to the right for conventional cutting or left hand cutters climb cutting.
Since the G0 G90 G40 G80 are usually already set and are model, the tool change block can just be: T1 M6

But different machines with their controls may dictate certain formats or sequinces for T word and M6 calls.

The Fadal format does not use the G43, G49 or the D word. The H word is used for both tool length and tool comp.

[kbcnc]

The Fadal format does not use the G43, G49 or the D word. The H word is used for both tool length and tool comp.

This is true if your Fadal is set up to operate in Format 1 only!

If your Fadal is set-up for Format 2 operation, then you must use the "D" work to invoke cutter compensation.

Example:

M6T3 (.5 cutter)
M3S2500
G0G90X-.25Y-.35E1
H3D3Z.5M8 (D3 must be here so control can read Tool Dia. Offset
Page!!!)
G0Z-.1
G1G41X0Y-.35F10.
Y1.
....
....

[Rekd]

The H word is used for both tool length and tool comp.

Actually, the D is optional in Format 1...

'Rekd teh .02

[ARB]

The Bottom line is that Cutter Comp is one of the more powerful tools when it comes to programming. It will be your friend when you master it. I would sugest writing some simple programs and experiment with G41 And G42 until you are comfortable with how they work on the controls that you are using. This is one of the more critical concepts to master and when you do your whole CNC experience will be better.

Next up. Unlock the power of Sub Programs.

[rob2424]

wms
using a 1/2 endmill would you not enter the radius of the
cutter into the d offset which would be say .255 for roughing
and.250 for finishing when you are applying g41 or g42.

[Rekd]

Depends on the way the CRC is set up in the controller. It can be either set on Dia or on Rad, on Rad, yes, .25 for a 1/2" EM, on dia, .500 for 1/2" EM.

Why the difference? Preference mostly, but a bit of application. For instance, I use DIA because it gives me more control over the amount of CRC I can use, (well, when speaking of .0001 anyway.. ).

'Rekd