3-axis cutter comp?

[ghyman]

I've never tried this before, but a friend has asked me if it is possible to use cutter comp (or something similar) on a reground ball endmill (ø3/8" ball mill reground to ø.365 / R.1825) that would control the cutter path in 3-axis profiling.
He is doing some fairly detailed profiling, and would like to be able to use reground tooling to help control costs.
Unfortunately, I do not have access to a machine that would let me play around and see what I can find out.
And to be honest, I'm starting to burn out brain cells trying to figure it out.

The three hardest words I've ever had to say... "I Don't Know"

Anyone have any thoughts?

Thx.

[HuFlungDung]

Use of a 3d cadcam system like OneCNC will make whatever alterations are required in the toolpath to match the ball radius, whatever it may be. This is so simple for the user to do, that it is practically a non-issue.

Full 3 axis movement cannot be compensated with the typical machine control running the built in cutter compensation, because the contact angle of the ball can vary anywhere from zero to 90 degrees. The control itself can only compensate in X and Y, and makes the assumption that the part profile path is always at 90 degrees to the cutter axis.

[arfonce]

When I started to learn cnc programming back in '88 I was taught how to use cutter comp. in x,z and yz planes as well as the more popular x,y plane. I've been doing it ever since on various Fanuc controls. When you turn the comp. on you need to tell the control what plane your comping in so you give it a g18 for x,z or g19 for y,z. Normally the control is using g17 by default for the x,y plane.Plus the usual g41 or g42. That's the hard part-figuring-out what side of the programmed path to comp on.

You also have to "adjust" for the radius of your tool by shifting the tool down by an amount equal to it's radius.So if you tell it to go to zo it'll go 1/2 the tool below zo with a tool comp=0 and right to zo with a tool comp=1/2 your cutter.

You can also use this type of cutter comp for sharp-corner tools or bull-nose tools. There's another shift you have to use for them.

But this is still only 2-D cutter comping, not the true 3-d comping that is also possible with the newer controls and which I've never needed to try-Easier to
use cadcam for that.

Hope this helps

[titleist]

G17, G18, G19 will allow you to compensate in 2D moves for a reground ball. if you are doing a 3D and milling in all axes at the same time you will not be able to comp the ball in Z

[psychomill]

3D tool comp is an option on on Fanuc and Mazak boards as well as a couple others. Only have a limited knowledge on this stuff as I don't use it. I do know that in order for it to work, you turn it on durring a 3 axis move setting all comps with I, J, and K. If one is is skipped, it only activates Comp C ( or your standard "2 axis" ) with the comp in the direction of the control plane. It can also use variables U, V and W.

So it is possible by the way it sounds. But I've never seen a control loaded with the option.

[routalot]

I have no idea what your friend is running by way of software,consequently the following advice may be irrelevant.I used the tool library in Mastercam to do the work by adding a new tool and calling it "reground 3/8 ball mill".I then entered the actual diameter of the tool and regenerated the toolpath using the newly added tool.

[ghyman]

Psychmill -- You're my HERO!

Do you know of any specific controls that support this option?

I've never heard of such an option being available, but it sounds like just the ticket!
No offense to everyone who suggested re-posting the code. That is actually what they are doing in this guy's shop now, and it's actually causing more problems with "too many people messing with the CAM system" than it is worth.
It seemed logical that someone would have a fairly simple "offset-type" adjustment on a control rather than re-inventing the wheel every time a path needs 'tweaked'.

[psychomill]

Psychmill -- You're my HERO!

I wouldn't go that far just yet, like I said, I've never actually used this so I don't know what the results are. And I'm not sure of how "simple" this is to use. The program format is something like this:

G41 Xx Yy Zz I? J? K? Dd

I'm not sure what input values need to be present for I J and K. I know that a zero is effective so you could try that first with comp in D and see what moves it makes.

BEFORE you go through all of this though... This is a controller OPTION! Not all controls have this. I'm not even sure that I've come across one that had the option installed and I don't know of anybody that uses this in a G-code program. You'll have to call someone or talk to the factory about its uses. The controls I know of that have this option available are Fanuc (16, 18, 21, 160, 180 and 210 - "i" series anyway) and Mazatrol (M+ and Fusion - not sure about M32 or older).

I also have a couple thoughts and reservations about using this. Even if this option works in the manner we "want" it to,... I don't think the end result will be satisfactory. In a simple spline type, single "line" cut, this may work ok. But in say a cavity or other complex surfacing ( complex as in multiple blends and tangents ), this may not result in the desired effect. Even if the machine were to comp in 3D, the machine still can't comp the programming for it. In other words, a .01 stepover is still a .01 stepover, just with comp. So, picture this ( and this is exagerated on purpose ), say you're cutting a cereal bowl with a 3/4 ball mill and a .030 stepover. Say this creates a finish that you like. Now change that to a 3/8 ball mill posted to the same stepover and DOC. It still cuts a bowl and if you can measure it at the actual tangents of the cut, the bowl dimensionally is still "accurate". But now your finish sucks because of the increase in scallop height. You can't change the programmed cutting data even with comp so I see this as a possible problem.

Now, in a conversational control (like Mazatrol), this takes on a whole different aspect. You can comp in full 3D but thats because the part is 'calculated' when it runs. You only identify the physical part in programming then the machine does the rest. You can totally change endmill size and it will still come out correct.

I do my fair shair of 3D programming and 5 axis swarf stuff, but I'm no expert on using the 3D comp. Maybe someone here has ( any mold guys or 5 axis gurus use this?). Sorry for the long post.

What do I do? I repost the program if I have to change cutters or comp something. I never use regrinds as finishers. When a finisher becomes worn (or needs to be comped), it becomes a rougher and I get a new finisher. Or the tool gets ground into something else.

...."too many people messing with the CAM system" than it is worth.

"everybody" shouldn't be messing with the CAM system. But IMHO, with today's CAD/CAM systems, processing speeds, ease of generating the code,.... I just repost the program.

[Fredkc]

God what fun!

Now, as long as you don't mind an old fart chiming in, I did this for a living from 1978 until about '96. From '94 until about 98, I was back and forth between CAD and CAM work.

So naturally what you're about to read is a teeny bit dated, but from a quick read, it doesn't sound like they've changed totally run off and left me. So...

The 10M and 11M series controls were basically shipped with two major levels of software built in them. The options for the controls were abut 90% there, and only needed "turning on" by changing parameters. The lower level package was capable of std. 2D cutter comp only.

You needed to have the higher level software package for 3D cutter comp to work. A mixed blessing, really. Previous poster was right. 3D cutter comp. is initiated by making a G41/42 call while moving in a 3-axis move. You need to move in all three axis at once, moving at least 2-3 times the cutter diameter during the move. Now I have heard a lot of folk say the machine can figure the tangent vectors with a 1.5 x cutter Dia. move. but it's cutting it close, and if you don't have to, why do it.

Hint: I certainly hope your cutting something fairly substantial. 17-4 etc. Operators can be very hard on aluminium and this kind of work. The reason: is that the load on the processors goes clean outa sight. Fast feedrates and this kind of computing intensity can, or would back then, push the control right to the limits.

Not uncommon when you push the feed too far to have the Fanuc get "lost" at which point they can either "wander" or the control will simply drop out of cutter comp mode. Duck, things get exciting.

If it's a job where you can push tools then you're actually better off getting hard numbers from a CAM system. That way the control is only concerned with driving the motors, and isn't having to calculate as it goes.

Fred,
ps: I did shop programming for about 10-12 years, then off and on I worked for FEMCO lathes, Machinery sales, Nakamura, and several other machine tool builders in SoCal. Time studies, and in-shop teaching for about 5 years, then back into shops. Finally I got tired of sweatin' my but off in the shop, while some jerk sat there in the A/C drawing lines on a CAD system for e to cut. I joined the other side. My last job in the field was programming 6-axis, twin spindle, twin turret lathes with live tooling. Nakamura TW-10's mostly.
Now that was fun!

[dertsap]

depeding on how tight the surface cutting is for step over and the way the cam system configures the arcs and such , i ve had .001 d comp alarm out the machine due to tight arcs, easiest thing to do is like HuFlungDung said use the cam system to set the program to that dia of tool
i don t understand your concept of 3d d comp for x y z diameter compensation is for the diameter of the tool 2d xy , you can profile with d comp x and y will change with what ever value you add but z will remain the same , i ve done surfacing to make fixtures for parts and used d comp but the z remained the same , the part only opens up more

[cadman]

Another controller to throw out there is the Okuma OSP-P100M. It has 3D cutter compensation (G43,G44), 3D circular interpolation (G2, G3 X Y Z I J K [P,Q,R]) and 3D Arc Rotating Direction (G256). We just finished replacing 15 Fadals with 15 Okuma MB-46VAE & MB-56VA machining centers. These are all options on our controllers.

Do we use them? No. All tool compensation for 3,4,and 5 axis tool paths is done in the cam software. If the toolpath needs to be compensated in some way the program is edited and reposted. We also have two NURBS options and use one of them, Hi-NURBS, for all 3 axis+ toolpaths and even most of our 2D programs. As powerful as the controller is, we would rather not have it calculating both 3D comp and NURBS at the same time.

Our parts are very complex geometry-wise, and the best approach in our shop to eliminate as many unneeded variables as possible from the process, 3D comp being one of them.

CM

[wjbzone]

Ghyman,

We have a couple of Mazak M2 mills with a "3d option" that will do this. You define the surface in a Mazatrol unit, and the machine calculates the path each time it runs.

You can set the actual diameter of the ball end mill in the tool data.

This M2 control may be limited on some shapes compared to what you can generate with today's CAM systems, but it has covered most of the things I have tried on it. Also the path may not be as efficient as new CAM system.

I bet the newer controls have a lot more capability. These M2's are near 20 years old now.

Bill Barrows