[Mortek]

I'm wondering if you maintain chipload per tooth can you raise the spindle speed and ipm to high speed mill in 4140 soft material? For instance, recommended sfm for the cutters I'm using is about 280(1/2" carbide 4 flute tialn coated) So 1900 rpm and 17 ipm gives me a .0025 chipload. So would it be acceptable to go 6000 rpm and 50 ipm to maintain same chipload but not as deep of a cut, and the cutter survive the action?

[HuFlungDung]

Mortek,

Are you roughing with this tool? Wet or dry?

I would not recommend going much faster sfm when roughing, but you can likely get away with quite a bit more speed when finishing at .01 or .02 doc. That is if cutter vibration doesn't start up.

But, Ward would likely have more experience to relate to, than I do.

[wms]

Ken,

That may be possible but the increased surfaces speed may be more than the cutter and /or coating can handle.

As you increase surfaces speed you create more heat and the coating may fail, then the cutter substrate will be next.

Tialn is a coating that likes a little heat to work best. But it too has limits.

Tialn is normally run dry, but I have under some instances run coolant. I would run dry in this material, with maybe an air assist to clear chips.

If you are using a sharp corner mill, that corner is what will fail first so watch it like hawk until you know your setting are OK.
Once the corner chips then more heat will be generated and major chipping or fracturing will occur and the whole thing will go.

[Mortek]

Ok guys now for a finish using 1/2 carbide ball mill 4 flute uncoated wiht .010 remaining stock. How does 3000 rpm 40ipm .025 depth of cut (.003 chipload per tooth) in z level finish sound?

[wms]

Ken,

.025 might give you a little rougher finish that you want. But should be about 125 rms.

You could try a section and see. Just section off a small portion of your model in OneCNC and let it write the code for that section only. Then you could see how it looks.

The tool would have no probelm at that speed or feed.

[Mortek]

OK guys,
Here's what the endmill manufacturer suggested for the 1/2" Hanita varimill for a roughing pass. 4000 rpm, 45 imp side milling, and 17 ipm plunging. I'm going .075 deep per pass. Pretty impressive.

[camminc]

Mortek: Each cutter has a best RPM to run and to find this RPM one needs to do an Impact Test. Once this is done, it only takes a few minutes when you have the equipment, you will know what suggested RPM and depth of cut to maximize, it will tell you what highest RPM you can go by calculating the SFM, then set your parameters for feedrate. See article - Chatter Myths in June - MoldMaking Technology for a more indepth explaination. Also see: http://members.cox.net/camminc/