Corner Radius Tools?

[machred23]

Hello all again!

So is there no definition for a corner radius for tool for rounding of top corners? Do you just have to program it as an endmill and figure the math based on the tool for how deep it needs to go? Let me know if I am missing something.

Thanks,

[HuFlungDung]

I don't run your software, so I don't know what options you might have.

But personally, I can make do with a 90 degree chamfer mill as a suitable alias for a corner rounding endmill. Make the body diameter of the chamfer tool same as the outside diameter of the corner rounder, and the tip diameters should also match. You can fudge the numbers a little bit either way to improve the way the actual (or particular) tool seems to align itself with your workpiece.

No, they don't simulate exactly the same, but that's what you've got an imagination for

[Brakeman Bob]

Originally Posted by machred23 So is there no definition for a corner radius for tool for rounding of top corners? Do you just have to program it as an endmill and figure the math based on the tool for how deep it needs to go?

I use corner rounding cutters (or "EDGE RAD CUTTER" as they are defined in my tool library). What I have done is set up a "user defined tool type" using endmill as the basis, then define a Shaped Tool with the geometry of the corner rounding tool required. Then I add a tool to my tool library of Tool Type "EDGE RAD CUTTER", assign it the form defined in Shaped Tools and, crucially, given the tool diameter on the "Topology" tab the value of the smallest diameter on the cutter. For example, a 3mm edge rad on a Ø16 cutter has a core diameter of Ø10, so I put 10 in the diameter box. When using the tool in a program you just program to the depth of the shoulder which here in the UK is usually the size to the radius you are cutting.

This method works with cutter comp if you use the smaller diameter (or radius) of the tool for setting your D offset on the machine. It also shows nicely in SolidVerify.

Bob

[jmcglynn]

I assume you're talking about round-over cutters?

Define it as a standard end mill, then select the "shaped tools" option (on 2009 it is one of the tabs in the tool setup). You specify the diamater of the tip of the cutter as the cutter diameter, then in the shaped tools edit dialog you specify the bottom diameter and radius.

I like to use the round-over tools from Harvey Tools, they have a .005 cyl etension on the tip, so I can model the cutter as a shaped tool, touch it off and my round-overs come out perfect. I've used other brands, and when I call the factory or look in the catalog they can't tell me the accurate measurements of the cutters so it's trial and error until you get the depth set right.

[machred23]

Thanks all for you help!