compensation in Fanuc programme

Hi All,
Today I thread-milled a 36mm (1.417")thread 4mm (0.156")pitch with a 27.5 (1.082")cutter dia.
with compensation in the programme .I used an I. and K. for the radius output. Not a problem.
Normally when programming using cutter comp. If you travel less distance than the radius of the cutter it normally faults out. Is this because I am using a R. (Radius output)?
Am I explaining this ok

I think you may be confusing yourself which isn’t hard with these things it took me a while. Your machine is moving less than the tool radius, but your program is moving your tool radius plus the extra distance which is about 4.25mm to get to the thread OD assuming you put the tool at the center of the hole.


If you tried to apply an offset of 27.5mm to the tool in a hole of 27mm for a hole machined at 27.1 then it probably would alarm. Where tool comp does funny things is when you rapid traverse from one direction to a line, drop down to cutting height and then machine a line arc or otherwise at a different angle. Sometimes it will do a radius movement as the cutter is not positioned perpendicular to the first line or combination of lines. Generally you just don’t do that however. It depends on your machine and how and where you approach from. IME however if your applied tool comp distance is less then the next feature distance where the offset is started, by any amount your good.

Also for full circle machining you have to use I and K if you weren’t aware, if use R it should alarm unless your using a circle cutting G code. Dont know if Fanuc has them, the 80’s vintage I have used didn’t.

Gerrythewelshman said:

Hi All,
Today I thread-milled a 36mm (1.417")thread 4mm (0.156")pitch with a 27.5 (1.082")cutter dia.
with compensation in the programme .I used an I. and K. for the radius output. Not a problem.
Normally when programming using cutter comp. If you travel less distance than the radius of the cutter it normally faults out. Is this because I am using a R. (Radius output)?
Am I explaining this ok

Click to expand...

You are explaining it fine. But the only question is in contradiction with the statement that "I used I. and J. for the radius output" The only question you posted is "Is this because I am using R (radius output)?".

So what is the question?

R

It is nowhere mentioned in Fanuc manuals that lead-in/lead-out distances should be greater than the tool radius. However, this might be a requirement on some controls. Therefore, it is best to make these moves larger than the radius of the tool.

It depends. If the comp move is less than your straight line move to activate comp it should be fine, if it is greater than you should see an alarm. If you are using cam (?) and use the wear comp option, you can have a lead in of .05-.01-.015" and be fine if your comp is less than that (thinking dialing a part in a few thou). Using I,J,K or R values should not matter, unless (like Haas) your machine won't take a comp move on a G02/G03 line, you need to activate comp with a G01 move (possible G00 but not seeing why you would?).

Mike1974 said:

(possible G00 but not seeing why you would?).

Click to expand...

One may compensate in air using G00, then plunge and start cutting.

sinha said:

It is nowhere mentioned in Fanuc manuals that lead-in/lead-out distances should be greater than the tool radius. However, this might be a requirement on some controls. Therefore, it is best to make these moves larger than the radius of the tool.

Click to expand...

This is where the penny dropped for me. If your start up move isn’t greater then the tool radius or the same as then your already cutting, unless you do as you said above apply above and drop down to cutting height.

This subject keeps coming up on a very regular basis, and I think the primary reason is due to the wording used in most of the manuals and descriptions for cutter comp moves.

For me, the easiest way to explain it to the guys here is to have them substitute the word "move" with "programmed move".

And then, I use a real life example such as this one.

Imagine that you have a 10mm dia endmill, and you have to interpolate an 11mm hole, assuming the hole ctr is X0 Y0

So, your program would look like this:
N10 G00 X0 Y0
N20 G01 Z-1. F10.
N30 G01 G41 X5.5 Y0
N40 G02 X5.5 Y0 I-5.5 K0
N50 G01 G40 X0
N60 G01 Z1.

In block 10 and 20 , you've positioned your tool to the ctr of the circle and plunged to the required depth.
In Block 30, you've ramped onto your diameter of 11mm, which has a radius of 5.5mm.
Your tool is 10mm, so it has a radius of 5mm. You have programmed a move of 5.5mm, which is larger than your tool radius, so you have complied with the rules.
The fact that the cutter will only move .5mm is immaterial to the rules!

In Block 50 you've done the same thing in reverse. You've programmed a 5.5mm ramp-off move, which again is in compliance with the rules, even though the tool will only move .5mm.

So in closing, the following comment:

Normally when programming using cutter comp. If you travel less distance than the radius of the cutter it normally faults out.

Click to expand...

is incorrect!
The correct wording should be:

Normally when programming using cutter comp, If your programmed move ( or commanded move ) is less distance than the radius of the cutter, it faults out.
The actual travel distance is determined in the control by way of: distance = programmed move - tool radius

Click to expand...

SeymourDumore said:

This subject keeps coming up on a very regular basis, and I think the primary reason is due to the wording used in most of the manuals and descriptions for cutter comp moves.

For me, the easiest way to explain it to the guys here is to have them substitute the word "move" with "programmed move".

And then, I use a real life example such as this one.

Imagine that you have a 10mm dia endmill, and you have to interpolate an 11mm hole, assuming the hole ctr is X0 Y0

So, your program would look like this:
N10 G00 X0 Y0
N20 G01 Z-1. F10.
N30 G01 G41 X5.5 Y0
N40 G02 X5.5 Y0 I-5.5 K0
N50 G01 G40 X0
N60 G01 Z1.

In block 10 and 20 , you've positioned your tool to the ctr of the circle and plunged to the required depth.
In Block 30, you've ramped onto your diameter of 11mm, which has a radius of 5.5mm.
Your tool is 10mm, so it has a radius of 5mm. You have programmed a move of 5.5mm, which is larger than your tool radius, so you have complied with the rules.
The fact that the cutter will only move .5mm is immaterial to the rules!

In Block 50 you've done the same thing in reverse. You've programmed a 5.5mm ramp-off move, which again is in compliance with the rules, even though the tool will only move .5mm.

So in closing, the following comment:

is incorrect!
The correct wording should be:

Click to expand...

ehh... you are in 'murica so try explainin' in inches and feet and people might pay 'ttention...

Mike1974 said:

ehh... you are in 'murica so try explainin' in inches and feet and people might pay 'ttention...

Click to expand...

OK, How'bout a .5004 hole with a 1/2" em?

N10 G00 X0 Y0
N20 G01 Z-1. F10.
N30 G01 G41 X.2502 Y0
N40 G02 I-.2502
N50 G01 G40 X0
N60 G01 Z1.

Is that better?