Constant surface speed ball nose end mill

[jeepnuk]

I have to profile a cavity with rounded edges and a flat bottom. It has already been roughed and semifinished to .01". I intent to use a .5" ball nose to finish the entire cavity (sides and floor). When I'm cutting the walls I'm using the sides of the cutter (.5" dia). When the cutter is approaching the floor along the rounded edge the effective diameter of the cutter varies but keeps getting smaller. When the cutter is at the floor a .01" DoC gives and effective diameter of .110".

 

I would like the machine to maintain a constant SFM and IPT. As the effective tool diameter changes I would like the rpm and feed to go up automatically (think of a lathe).

 

I'm not expecting 1 rpm changes but let's say 100 rpm at a time at the proper intervals.

 

Is there a Surface finish command that I'm not aware of? Is there a C-Hook?

 

Thanks in advance.

Ed.

[mold100]

Ed,

 

No such luck, you can not change rpm during machining the mill makes drastic changes in the cut and this would not be an easy feat. The lathe handles it differantly than the mill. This has been brought up in the past by differant people. The machine tool and software company that pair up and accomplish this would become legendary. The feedrate that is possible depending on your machine controller. Welcome to the forum.

[chip]

Hi Ed,

 

There has been numerous attempts at tring to compensate for surface feed rate for milling applications.

 

I used to program for Fadal's and their approach was a (G08 G09). Some kind of incremental acceleration blah baleh blah. No Bueno.

I have alway's turned it off with a G08.

 

Steve the Mexican!

[Redfire427]

The best approach to this is to use high speed waterline machining using a slope angle of 30 to 90 degrees with a suitable rpm as you are more or less cutting on the diameter of the endmill. I would then follow it up with a raster or scallop toolpath machining between 0 and 35 degrees of slope. Now you can crank up the rpm and feedrate to create a much more effective cycle time. You could even use a bullnose and a horizontal toolpath for the flat areas and then change your slope on the raster toolpath to .1 to 35 degrees and it will only cut the shallow areas and nut cut the flat floors.

[jeepnuk]

So I guess the only alternative I've got is to post a surface finish countour and manually up the feeds and RPM's in G-code at various Z depths? Not too quick but it will accomplish the desired effect.

 

Ed.

[gcode]

Vericut's Optipath can do this ... but it is

expensive

[Colin Gilchrist]

+1 for Optipath, I love Vericut...