cutter compensation C on 0m-A control with only H offsets?

my old 0m-A system only has H offsets. I think it is set for cutter compensation C. I have been reposting to hit tolerance but I'm trying to use the "wear" compensation feature in fusion360.

my machine runs the code using the D offset but there is no compensation. if I change the D to an H. the machine runs but changes the tool length offset and crashes.

should the machine be in cutter compensation C or should I change it back to A or B?

snippet of code that runs
T3 M06
S3979 M03
G57
M08
G00 X103.786 Y-46.143
G43 Z35.5 H03
G00 Z25.5
G01 Z1.045 F300.
X103.813 Y-46.115 Z0.797
X103.894 Y-46.035 Z0.574
X104.019 Y-45.91 Z0.397
X104.177 Y-45.752 Z0.284
X104.352 Y-45.577 Z0.245
G42 X104.635 Y-44.729 D23
G02 X106.332 Y-44.73 I0.848 J-0.849
G01 X106.39 Y-44.788

I'm a little confused by your post. Let me try to make sense of it. Your machine will have a certain compensation type that is typically not changeable. You might have choices in Fusion as to what type you want to use, but you typically do not have choices on the machine. Meaning you need to set up Fusion to match what is available on the machine. If you have only H offsets you do not have compensation Type C. All machines will use H as Tool Height Offset. Through parameter change you can generally select if you want your Cutter Radius Compensation to use D's or H's. I've been running a Fanuc OMC for years using only H's for both Tool Height and Cutter Comp without problems. I do not have Wear Offsets for either.

I don't know how Fusion applies cutter comp. To start you should be using G41 for comp and not G42. G41 will give you climb milling which is what you want. Set your comp radius using an H value that is not being used by another tool for Tool Height Offset. My machine has 32 H values available and only a 23 tool carousel. If you change you parameter to use D's, you still enter the comp values in the same place as if they were H's on the simpler versions of Fanuc Offset Types.

So you're saying if you run the exact sample above and change the D23 to H23, the machine crashes in the Z axis or plows into the work in X or Y? Which one? If it plows into the material in X or Y or both, you simply have the wrong value of Cutter Radius Compensation set in the control. Understand that Fusion still needs you to set the appropriate numbers into the control. Sorry I have no idea as to your amount of experience with using Cutter Comp.

As far as what parameter to change to use D's instead of H's you'll have to look it up. I've never bothered to.

Thanks for the input. You can change the compensation to whatever you like but it is an option parameter.

I discovered a little more today.

I found my machine is using the D in the code and points the offset to a combined offset table. I only have offsets 1-64 or somthing. The H points to the samle table as D. so if H 1 is 8.00 and you command D1 it will be D=8.00 also.

The machine keeps the tool length applied thoughout the z moves and on the control screen you only see the H value change. For example when D21 is commanded H01 changes to H21 but the tool length compensation still remembers H01. I'm only guessing at this point that D21 is being applied and will run some tests.

The crash happened as the H refers to height and D refers to diameter. The old 0m-b manual I have only uses H values.
This is the start of the example from the manual. N1 G90 G17 G00 G41 H07 X250.0 Y550.0 So I changed the D to a H and the 8.00 in H21 was appled and added to the -40.0 in H01. The tooled moved fown 8mm and crashed in the Z. luckilly the collet gave way.

in regard to the fusion360 CAM package and choice of compensations it still uses G41 G42. wear compensation just posts a tool path which is almost the tool diameter away and the offset in the machine becomes a difference between the programed tool diameter and the true tool cutting diameter. I'm still figuring it out but it looks like it is working on my control and I just have to run some more careful tests. When trying to use traditional tool diameter offsets I was getting an overcutting error. This was the lead in requirment but it seemed way to long. Over the diameter of the tool. The wear compensation option dosn't have this problem so far and has a very small lead >1mm.

It's still all a little confusing but I'm working on it. I knew you could get different Offset types on old Fanucs with Option Parameter change. The newer machines don't have all the information buried in them like the old ones do.

There are two ways to run cutter comp and you seem to have hit on them in one way or another. Technically if you're getting the over-cut error, it means you're trying to pass through a part feature that has a radius equal to or smaller then the tool you're trying to use. In general if you have a 3mm radius in the part you really don't want to be stabbing into that corner with a 6mm tool. But people want to anyway. The only way to get past the error is to set your radius very slightly smaller then it really is, which sort of defeats the purpose of using cutter comp, as you have no where to go to make a part feature larger then the tool is cutting. A 4 or 5mm tool would fix all that, but that's a story for another day. Usually cutter comp is applied to a tool path that exactly matches the part outline, and through the magic of cutter comp radius setting, the machine automatically offsets the tool the correct amount. BTW you keep saying diameter for D. Almost always a control uses a radius settings in cutter comp. Although "D" want's to say Diameter, what it really is is an address in the control like H or M or what have you. Anyway... the second way people run comp as you seem to have tried, is to create and cutter comp an offset path in your CAM (a path equal to the tool radius and not Diameter) and use very small settings of cutter comp to correct the part dimensions from there. That works to and I've tried it myself.

Curious were you getting that over-cut error. Is it during the lead in move or somewhere along the tool path?

I can't believe your machine is crashing in Z. If you set your tool height for tool 6 lets say in H6, and the cutter comp radius for tool 6 in H16, and call in cutter comp with something like

G1 G41 X250.0 Y550.0 D16 F400. it will crash in Z? Doesn't make sense. I'm also surprised the manual shows turning on cutter comp in Rapid G0 mode and not G1 feed. Never heard of that.

It might help to start all your tools with a safety line to make sure all previous things are properly canceled before bringing each tool into play. Something like

T6M6 (ANY TOOL)
G17G21G40G49G54G80G90G98

G0X250.0Y550.0
G43Z4.0H6S4000M3T7
M8
G1Z-15.F200.
G1G41X300.D16F400.
ETC-ETC...

BTW - if you feel you can change to whatever offset type you want, why not change to Type C and have all the bells and whistles you could want?

Also where on the control are you watching these H and D change? On the CHECK screen? They really just show what is last active, and not necessarily what is being applied at the tool.

It might be nice to see a picture of your offset screen(s) Stuff just isn't making sense. Maybe there is a parameter you have incorrectly set. The old O parameters aren't as well organized as the newer stuff but if you read through enough of them you might run across something that makes sense to change.