Fanuc compensation A, B, C

Long story short: I'm confused of tool compensation A, B & C. We cannot use diameter compensation and have to program without G41/G42. So, two questions:
1. How should I change the parameters to make them work with compensation A or B or C?
2. How should I change the sample program accordingly to make it suitable for cutter compensation A, B, and C?
The parameters and the sample programs are attached. The controller is Fanuc 16-M and the machine is FAMUP MCX 600 with dual pallet.
Tnx in advance.

Your post is a little confusing. Tool compensation and cutter compensation are to separate things. Cutter comp is generally available whether you have tool compensation tables type A, B or C.

The problem is in your code.
First, you almost never use G42 because that will have you conventional milling and you normally want to climb mill. 2nd, you have to use a different H number with G41 then you already used for tool height. 3rd. get rid of the H call when canceling comp with G40.

If you have tool tables type A or B, with say 32 places of entry, put tool one height offset in H1, and the RADIUS of your tool in say H21. Then use H21 along with G41 when starting comp. There is a parameter you can change so you can use D for comp and H for tool height. (Look it up.) It may already be set up to use D for cutter comp.

I've run a machine for nearly 20 years with tool table type B and only 32 entry spaces and using H for both tool height and tool length without trouble. I have a 22 tool changer. Normally I just add 10 or 20 to the tool height number and use that for the cutter comp offset number.

Your code should look something more like this.

%
O100 (100.NC)
( MCV-OP ) (22-SEP-2020)
(SUBROUTINES: O3 .. O0)

M6 T11(TOOL -11- MILL DIA 50.0 R0. MM )
G17G21G40G49G80G90G98

M01

G57
G0 X76.78 Y-40.357
G43 H11 Z25. S1000 M3
M8
(-------------------)
(F-CONTOUR - PROFILE)
(-------------------)

Z2.
G1 Z-5. F50.
G41 X51.779 H21 F800.
Y40.357
X-51.779
Y-40.357
X51.779
G40 Y-65.358
G0 Z25.
M30
%

I can't promise this will work because you still have to have the proper lead in and lead out etc, which I haven't bothered to check.

Thanks the_gentlegiant
What is the difference between tool compensation and cutter compensation?
I just want the tool diameter compensaton work like the tool length compensaton, entering G41/G42 H_ and over!
Why should the tool number in H_ differ from the original tool number? How can they be the same?
and how do you use it yourself on your machine? What should be the setting for the correspondant parameters?

And BTW, the tool offset table contains Tool Height, it's wear, Tool Diameter, and it's wear in it.

Hi Hey you,

If you have four columns in your tool offset table then you have offset type C which is the latest and best one. I was thinking you had one of the earlier varieties like Type A or B which has only one or two columns.

Before I go any further, search Fanuc 16 Operations Manual B-62764EN. Everything you ever wanted to know about tool offset and cutter compensation is there starting about chapter 15. If you can't find one, drop the B and/or EN in your search.

Type C offset table uses H for tool length and D for cutter radius offset. Don't let the D at the column heading fool you. D is a computer address that happens, by convenience, to remind you of diameter, but you enter the tool radius there.

Tool height H settings are of course there to tell the machine how long your tools are. When you call G43 it looks in that table for the value. Yes use H1 for tool 1. H2 for tool 2 and so on like anyone would imagine. The H wear column is generally used to fine tune depth settings. If you're cutting say too shallow with a tool, you could add a negative number in the wear column to correct that without messing around with the original setting. It's only there for convenience. For all practical purposes, the two H columns are exactly the same thing and can be used interchangeably. The same holds true for the D columns. They extra, identical columns are there strictly as a convenience feature. That's it. Sometimes I use the H wear column to switch what I measured a ball end mill length at, and add a negative number to that to represent the core of the ball. A lot of times I'll program a ball mill from the ball core instead of the tip. Say I had a 1/2" ball end mill, measured it and got -14.3788 and entered that into the first H column. I will simply enter -0.250 in the H Wear column to pretend I measured at the core of the tool. The two columns are just added together by the control. Not sure your machine has it, but you generally can add or subtract incremental amounts from any number in the table using the soft keys under the screen. Say you want to do what I said about the 1/2" ball end mill. Type in -0.25 (you may have to be in MDI or EDIT Mode) and see if INPUT+ and INPUT show up at the bottom of the screen over your soft keys. If so, and with the cursor active in the part of the table you want to change, you would hit INPUT+ to add the negative (-0.25) to the existing negative number. Making the tool seem more negative (shorter) then it is. INPUT would simply change the current number to whatever number you just punched in. Hope that makes sense. That may be a manufacturers feature and not Fanuc, So you may find your machine doesn't work like that.

It sounds like you should study up a little about Cutter Compensation, which uses the D columns in the offset table. Here is where you put the radius of your tool. It's only needed if you're using Cutter Compensation. Otherwise you can leave it blank if you're using offset tool paths. You can use cutter comp on offset paths too, but let's leave that alone for now. Cutter compensation has start up and shut down rules that must be followed or the machine will give you an alarm. It's sort of a huge subject and It would take all day to explain it here. Best you read up on it in the Fanuc Manual I mentioned, or better yet, in Peter Smids book on CNC Machining which is written in a much easier to read style then Fanuc manuals are. I'll just say it again. The two D columns represent the tool diameter (by setting its radius) and are identical. The D WEAR column is there only for convenience.

Say you're cutting the periphery of a 2 inch boss or post with an end mill and it's coming out 2.0026. You would enter -0.0013 (half the error) in the wear column to correct this. This makes the machine think the cutter is smaller in diameter then it is so it moves the tool path closer to the work to make up for it, and cuts an extra 0.0013 off the post all the way around. If you were doing the same thing to a bore, meaning the bore is cutting oversize, (2.0026) you would set 0.0013 to correct it. This makes the machine think the tool is bigger then it is so moves the tool path away form the work and cuts the hole smaller by 0.0013 all around. See how they're opposite when you 're cutting an outside feature compared to an inside one? If you're using the same tool for both inside and outside features and for some reason one comp setting can't seem to satisfy them all using the same D number, just give it a 2nd unused D number to use. One for inside work and the other for outside work, Just make sure the different D numbers appear at the proper places in your program. What I'm saying is there's no law saying you can't use D32 for tool 2 if you want to. As long as you program asks for D32, that's what you'll get. The number entered in D32 on the offset page.

That's about all I got for that. Comp is something best studied up on. Meaning hit the books for awhile and try a few things out.

I sure wish they gave you more time to edit a post.

BTW - The business above about using the INPUT+ and INPUT soft keys is especially helpful on the work coordinate pages. (G54-G59 etc). Again this may be a machine builder option. You can make changes to the work coordinates using these keys. Saves having to type things into a calculator and possibly making a mistake, which with work coordinates, especially Z ones, can be real bad news.

Quote:

---

Originally Posted by the_gentlegiant

Hi Hey you,

If you have four columns in your tool offset table then you have offset type C which is the latest and best one. I was thinking you had one of the earlier varieties like Type A or B which has only one or two columns.

Before I go any further, search Fanuc 16 Operations Manual B-62764EN. Everything you ever wanted to know about tool offset and cutter compensation is there starting about chapter 15. If you can't find one, drop the B and/or EN in your search.

Type C offset table uses H for tool length and D for cutter radius offset. Don't let the D at the column heading fool you. D is a computer address that happens, by convenience, to remind you of diameter, but you enter the tool radius there.

Tool height H settings are of course there to tell the machine how long your tools are. When you call G43 it looks in that table for the value. Yes use H1 for tool 1. H2 for tool 2 and so on like anyone would imagine. The H wear column is generally used to fine tune depth settings. If you're cutting say too shallow with a tool, you could add a negative number in the wear column to correct that without messing around with the original setting. It's only there for convenience. For all practical purposes, the two H columns are exactly the same thing and can be used interchangeably. The same holds true for the D columns. They extra, identical columns are there strictly as a convenience feature. That's it. Sometimes I use the H wear column to switch what I measured a ball end mill length at, and add a negative number to that to represent the core of the ball. A lot of times I'll program a ball mill from the ball core instead of the tip. Say I had a 1/2" ball end mill, measured it and got -14.3788 and entered that into the first H column. I will simply enter -0.250 in the H Wear column to pretend I measured at the core of the tool. The two columns are just added together by the control. Not sure your machine has it, but you generally can add or subtract incremental amounts from any number in the table using the soft keys under the screen. Say you want to do what I said about the 1/2" ball end mill. Type in -0.25 (you may have to be in MDI or EDIT Mode) and see if INPUT+ and INPUT show up at the bottom of the screen over your soft keys. If so, and with the cursor active in the part of the table you want to change, you would hit INPUT+ to add the negative (-0.25) to the existing negative number. Making the tool seem more negative (shorter) then it is. INPUT would simply change the current number to whatever number you just punched in. Hope that makes sense. That may be a manufacturers feature and not Fanuc, So you may find your machine doesn't work like that.

It sounds like you should study up a little about Cutter Compensation, which uses the D columns in the offset table. Here is where you put the radius of your tool. It's only needed if you're using Cutter Compensation. Otherwise you can leave it blank if you're using offset tool paths. You can use cutter comp on offset paths too, but let's leave that alone for now. Cutter compensation has start up and shut down rules that must be followed or the machine will give you an alarm. It's sort of a huge subject and It would take all day to explain it here. Best you read up on it in the Fanuc Manual I mentioned, or better yet, in Peter Smids book on CNC Machining which is written in a much easier to read style then Fanuc manuals are. I'll just say it again. The two D columns represent the tool diameter (by setting its radius) and are identical. The D WEAR column is there only for convenience.

Say you're cutting the periphery of a 2 inch boss or post with an end mill and it's coming out 2.0026. You would enter -0.0013 (half the error) in the wear column to correct this. This makes the machine think the cutter is smaller in diameter then it is so it moves the tool path closer to the work to make up for it, and cuts an extra 0.0013 off the post all the way around. If you were doing the same thing to a bore, meaning the bore is cutting oversize, (2.0026) you would set 0.0013 to correct it. This makes the machine think the tool is bigger then it is so moves the tool path away form the work and cuts the hole smaller by 0.0013 all around. See how they're opposite when you 're cutting an outside feature compared to an inside one? If you're using the same tool for both inside and outside features and for some reason one comp setting can't seem to satisfy them all using the same D number, just give it a 2nd unused D number to use. One for inside work and the other for outside work, Just make sure the different D numbers appear at the proper places in your program. What I'm saying is there's no law saying you can't use D32 for tool 2 if you want to. As long as you program asks for D32, that's what you'll get. The number entered in D32 on the offset page.

That's about all I got for that. Comp is something best studied up on. Meaning hit the books for awhile and try a few things out.

---

Hi again the_gentlegiant
Thank you for your time and effort, I really appreciate that.
It's just about 4 months that I've started working with CNC, but I'm not new to it. As soon as I started to work with the machine, I started manipulating the parameters. So lucky that it hasn't blown up yet :) :).
There is a guy in our workshop that programs the parts, but he was unable to solve the radius compensation issue. He said the program used to work properly on other machines. I thought this may be due to parameters settings, so I started reading the operator's manual B-62454E/04 and parameters manual B-62760EN/01. But the more I read, the less I find. I changed the parameter 5001 with no success. Still the machine runs the sample program as if it doesn't have any G41/G42 in it, it overcuts. But the tool length codes are executed properly. I hope your changes take effect and solve the problem.
The machine has type C tool offset, but it depends what type of tool offset you activate on parameters (parameter 5001). I think it is type A now bcs all bits in parameter 5001 are set to zero and tool lengths in programs are executed with this type of offset.
About the Input keys, yes; the controller has Input and Input+ and I've just added the Input C. to it.
And BTW why do the admin(s) move the posts? This topic wasn't unrelated to this forum. I can't figure it out.
Again thank you for your help.

Hey Hey You,

It was Sunday and I had time to kill. Hence the long post.

I hope you have your original parameters backed up. A new guy messing with parameters is a little like playing with matches. Just sayin. Parameters 5000 and 5001 are mostly about tool LENGTH offset and have little or nothing to do with tool radius compensation. or Cutter Radius Compensation. (like "Interference in CRC" as you might see in certain alarms) Having them both at all 0's is fine and is what my machines show also. 5002 is for lathes, and 5003.0 (SUP) can be put to 1 for Cutter Compensation Type C startup type B, which I think is a more advanced form, but don't quote me on that. There are pictures in the Operations Manuals that show the differences. I have one machine set at 0 and one at 1 and I get them to both work fine, so take that with a grain of salt.

If you stick with linear to arc startups and shutdowns, meaning arc into the work and arc out of the work you should have no problems getting comp to work without alarms. Fanuc comp has a two block read ahead, so as long as your lead in and lead out arcs are at least a thou or two larger then the tools radius you will not get an alarm. Though it's still better, if you have free area to move in, to make the lead in arc radius a fair bit bigger then the tool radius. Say 0.100 to 0.250 or more then minimum. Not only does this leave less of a start-stop mark, it also broadens the scope of how big of tool can be used with the same tool path should a person decide to change to a larger tool then originally planned on. Of course if you're doing thread milling where you have almost no room, using lead in and out arcs of sufficient radius will still get you through without alarms. In thread milling the lead in and out of cutter comp will hardly move the tool at all, even though the tool path has length to it. The tool will do all it's compensating from the center of the pre-drilled hole to the start of the lead in radius along a very short linear move. It is the fact that the read-ahead sees the radius of sufficient size as the very next move, is what allows it all to go off without a hitch. Remember these lead in and out arcs MUST be headed and ended first with a LINEAR move (G1) You cannot start and stop Cutter Comp with an arc (G2/G3) move.

So, G1 G41 with small linear move of any length large or small, then arc of sufficient radius, then the actual part outline tool path, then the lead out arc of sufficient radius, and finally the G40 linear move (G1) to turn off comp.

Now I have to get back to work. Good luck. Hope it helps.

Thanks a lot man.

huhhhhhhh

- - - Updated - - -

hahhahahhaha....OMGGGGGGGGGGGGGGGGGGGGG

Quote:

---

Originally Posted by the_gentlegiant

Hi Hey you,

If you have four columns in your tool offset table then you have offset type C which is the latest and best one. I was thinking you had one of the earlier varieties like Type A or B which has only one or two columns.

Before I go any further, search Fanuc 16 Operations Manual B-62764EN. Everything you ever wanted to know about tool offset and cutter compensation is there starting about chapter 15. If you can't find one, drop the B and/or EN in your search.

Type C offset table uses H for tool length and D for cutter radius offset. Don't let the D at the column heading fool you. D is a computer address that happens, by convenience, to remind you of diameter, but you enter the tool radius there.

Tool height H settings are of course there to tell the machine how long your tools are. When you call G43 it looks in that table for the value. Yes use H1 for tool 1. H2 for tool 2 and so on like anyone would imagine. The H wear column is generally used to fine tune depth settings. If you're cutting say too shallow with a tool, you could add a negative number in the wear column to correct that without messing around with the original setting. It's only there for convenience. For all practical purposes, the two H columns are exactly the same thing and can be used interchangeably. The same holds true for the D columns. They extra, identical columns are there strictly as a convenience feature. That's it. Sometimes I use the H wear column to switch what I measured a ball end mill length at, and add a negative number to that to represent the core of the ball. A lot of times I'll program a ball mill from the ball core instead of the tip. Say I had a 1/2" ball end mill, measured it and got -14.3788 and entered that into the first H column. I will simply enter -0.250 in the H Wear column to pretend I measured at the core of the tool. The two columns are just added together by the control. Not sure your machine has it, but you generally can add or subtract incremental amounts from any number in the table using the soft keys under the screen. Say you want to do what I said about the 1/2" ball end mill. Type in -0.25 (you may have to be in MDI or EDIT Mode) and see if INPUT+ and INPUT show up at the bottom of the screen over your soft keys. If so, and with the cursor active in the part of the table you want to change, you would hit INPUT+ to add the negative (-0.25) to the existing negative number. Making the tool seem more negative (shorter) then it is. INPUT would simply change the current number to whatever number you just punched in. Hope that makes sense. That may be a manufacturers feature and not Fanuc, So you may find your machine doesn't work like that.

It sounds like you should study up a little about Cutter Compensation, which uses the D columns in the offset table. Here is where you put the radius of your tool. It's only needed if you're using Cutter Compensation. Otherwise you can leave it blank if you're using offset tool paths. You can use cutter comp on offset paths too, but let's leave that alone for now. Cutter compensation has start up and shut down rules that must be followed or the machine will give you an alarm. It's sort of a huge subject and It would take all day to explain it here. Best you read up on it in the Fanuc Manual I mentioned, or better yet, in Peter Smids book on CNC Machining which is written in a much easier to read style then Fanuc manuals are. I'll just say it again. The two D columns represent the tool diameter (by setting its radius) and are identical. The D WEAR column is there only for convenience.

Say you're cutting the periphery of a 2 inch boss or post with an end mill and it's coming out 2.0026. You would enter -0.0013 (half the error) in the wear column to correct this. This makes the machine think the cutter is smaller in diameter then it is so it moves the tool path closer to the work to make up for it, and cuts an extra 0.0013 off the post all the way around. If you were doing the same thing to a bore, meaning the bore is cutting oversize, (2.0026) you would set 0.0013 to correct it. This makes the machine think the tool is bigger then it is so moves the tool path away form the work and cuts the hole smaller by 0.0013 all around. See how they're opposite when you 're cutting an outside feature compared to an inside one? If you're using the same tool for both inside and outside features and for some reason one comp setting can't seem to satisfy them all using the same D number, just give it a 2nd unused D number to use. One for inside work and the other for outside work, Just make sure the different D numbers appear at the proper places in your program. What I'm saying is there's no law saying you can't use D32 for tool 2 if you want to. As long as you program asks for D32, that's what you'll get. The number entered in D32 on the offset page.

That's about all I got for that. Comp is something best studied up on. Meaning hit the books for awhile and try a few things out.

---

WHAT THE **** YOU SAY HERE BRO?:)))))))))))