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.