Corner Rounding Tool

[JohnJW]

Hi,

I was wondering what is the proper way to use/program corner rounding end mill. Let's say I have a .25D .031R corner rounding end mill. Do I just go Z-0.31 and use (.25 - 2*.031 = ) .1880 as the tool diameter when I use cutter comp around the profile of the edges?

If I need to chamfer the lips of a shallow radius groove do I just switch to XZ or YZ interpolation and use G02/G03 to round the lips of the radius groove?

Thanks,

John

[HuFlungDung]

Go Z-0.031 for depth or maybe a thousandth or two less to prevent the top edge of the tool from creating an undercut along the top of the corner.
As for the amount of the offset, it depends where your geometry is drawn. IF the geometry overlies the original sharp square edge, then the tool diameter would be .188 (or a tad more) as you described above for full radius compensation.

I do not think the tool will perform well in the vertical plane at all. For that you'd need a different approach using an angle milling head, or else interpolating the corner radius with several passes cut with a ball mill.

[extanker59]

If I was doing this by hand coding, I'd program the perimeter (or what edge needed to be radiused) and put the diameter of the TIP into the offset. The Z is as HuFlungDung says.

We use numerous radius cutters and it seems like they all have a different tip diameter for each size regardless of the tool diameter. Maybe we should standardize on one manufacturer.

[sti2011]

I have always programmed my rad. cutters to go to Z0. I have my guys either throw the tool on the comparator to check the "length" in Z and touch off the bottom of the tool then move it down that dist. minus .003 or so. Or as some of them prefer to hold the block against the side of the cutter then dial up in Z till the block starts to slip under the top edge of the rad.. This way you don't "stripe" a valuable part accidentally. BTW there are alot of different styles of rad. cutters that have slight flat angles at the edges to ease blending issues. I believe Harvey Tool has some good examples of some different types in their cat.. This why all seem to have no standard "lengths" The only caveat is to prog for the "added length" that hangs below the tool length offset. Just add the rad. value to all your clearance planes and youwill be good to go.........Diametral offsets are a must as H.F.D. said.