radius mill contour settings

[MattW]

when using a radius mill to roundover edges, I have to play with the countour depth to get the depth right. It sure looks like the depth is calculated from the top edge of the radius, although the tool is touched off the end. How do I set this up so that backplot and verify match reality? The immediately obvious answer is to add the distance from the tool end to the top of the radius to the tool offset register. Is that how this is normally done?

[Colin Gilchrist]

Matt,

 

It is measured from the top edge in Mastercam...

 

What I do is view and measure my corner rounding tools with an optical comparator and get the distance from the tool tip to the upper tangent edge of the radius. Then I subtract this distance from the tool length compensation register and you should be home free.

 

If I can I will usually make some test cuts with the tool to find the perfect length offset measurement distance, then I scribe that onto the tool...

 

Because of the difference between corner rounding endmills, I prefer to use inserted cutters whenever possible. This means you only need to setup the tool once, and then you can just change the insert...

 

HTH,

[MattW]

Thanks. I was worried about the calculation for feed plane being wrong if I adjusted the offset, but it looks like everything is properly accounted for, although I haven't really tried. Of course, comp is calculated from the smaller diameter, so I guess I have to either create geometry at the theoretical sharp edge or I have to put in "X-Y stock to leave" equal to the radius. Correct?

[Colin Gilchrist]

Yes, or drive the bottom rail of the radius, not the top...

 

No matter how you do it, I find you have to mess with something. Fuss with the depth, change the XY stock to leave, something...

 

Like I said my biggest gripe whenever I have to do this is the variation in geometry from one corner rounder to the next. I just hate it when I have to program for one of these things without a comparator. Then you basically have to sneak up on it and I almost always blow it and take off too much either on the radial or length offset and end up undercutting the radius...

 

If you can get a solid carbide or carbide insert cutter you will be money ahead. Most manufactures of the carbide tools will hold tolerances and publish the specifications of their tools...

 

I think Micro100 had some nice ones if I remember right...

[GMM]

we touch off the top of the radius not the end of the tool just for the reason that all corner rounding end mills are not alike.

There is usually enough extra to touch off of if you are carefull.

you need extra retract with this method.

A few years ago I played with the geometry file that shows the tool.

I tried to shift the geometry so it verified correctly from the top of the radius. limited success.

[htm01]

the rad cutters i have from harvey have a .005+rad , you can also get ones with a 5deg flair if you can get away with it to eliminate that step.

 

http://www.harveytool.com/products/search.php?keyword=17125

[GoetzInd]

I usually just draw a custom tool.

 

Mike

[Bryan Johnson]

Program from btm edge of rad so that backplot and verify is correct in mastercam.

At machine, set tool length by touch off at shoulder (easy to do), and then shift the Z offset by the corner rad.

 

Plug and play. No comparators, no sneaking up on it. But you do need to allow for extra retract to clear the full tool length.

 

I will set stock to leave at .001 to allow for a nice blend.