Looking for help with hard milling

[PrintGymnast368]

Hi,

I am wondering if anyone can recommend some cutting parameters or maybe a different tool for my application. I make knives and I mill my bevels in. I am currently using a 4 flute 1/4" .030" corner rad carbide end mill (lakeshore carbide) for my finishing passes. I machine most of the stock away soft and do some finishing post heat treat. The steel I am using is CPM Magnacut run at 63 HRC. It is an extremely wear resistant steel. A more common comparable steel would be S90V or maybe a more wear resistant D2.

I am leaving .0075" stock both radially and axially (pre heat treat). A stair step effect is created. Each step is .0035" deep and the width of a step is about .030". I'll attach some pictures from my CAM that will probably show this better than I can explain it. I have tried a few things and my tool life is very short. I can only get one blade out of a new tool. That is about 140" of cutting. Even then, the finish isn't perfect.

I know that hard milling with coolant isn't ideal but at the moment it's the only form of chip evacuation I have. If necessary I will get an air blast set up. For now, If I could get a tool life of 4 blades or about 600" of cutting I could live with that until I can sort out a proper air setup. I have tried a few different recipes varying from 50 to150 SFM with chip loads ranging from .0005 to .0015 (not accounting for chip thinning).

I have seen specific hard mill end mills, maybe that is a better way to go? If anyone has any advice or recommendation I would really appreciate it. In the past I have done this process on CPM154 at 61 HRC without issue. This new steel (Magnacut) seems to be harder on my tools. My fixturing is "good" under minimal pressure. The bevels do have a negative space on the obverse side. I fill this void with hot glue and that seems to support it well enough. I would imagine it wouldn't hold up to significant downward tool pressure though.

Here is a picture of my finishing toolpath:
View attachment 367667
Here is a pic of a good blade. after the first one I'll get streaking or uneven surface finish and the part is scrap. Sometimes I cant even get through a single blade without some imperfection.
View attachment 367668
Any advice is greatly appreciated. I am not a machinist so its more than possible I am missing something obvious here.
Thanks.

Change tooling to a 5, 6, or 7 flute AlTiN coated as the stronger core and higher flute count means more carbide has to wear down(finishing). Ultra tool makes good endmills in the US at a nice price. You have to make a account. No coolant, i recommend air blast or mql as the coating needs to stay hot to oxidize the chips. Also unless you like the look of the scalloped "grind" you could do a 3d surfacing toolpath with a ball or bullnose endmill and make a more finished surface without having to grind down all that material with abrasives.
Also higher flute count means you need a lower rpm to achieve the same sfm. Be carful about burning out tools because of high or low speeds and feeds
you could also call up ultra tool or another tooling manufacturer they will most likely help you find the best tool and settings for your application
These are some good resources on tooling
The tools:

HEM End Mills

www.ultra-tool.com

MQL:

https://www.researchgate.net/publication/304708200_Investigation_of_MQL-Employed_Hard-Milling_Process_of_S60C_Steel_Using_Coated-Cermented_Carbide_Tool

Flute count:

Why Flute Count Matters - In The Loupe - Machinist Blog

One of the most important considerations when choosing an end mill is determining which flute count is best for the job at hand. Both material and appli...

www.harveyperformance.com

General:

Multi-Flute End Mills Produce Thoroughly Modern Milling

End mills, traditionally made with two to four flutes, are used in one of the oldest mechanized machining processes—milling.

www.sme.org

 

[michiganbuck]

QT Stang; . (I am not a machinist so its more than possible I am missing something obvious here.)
Nobody is an everything machinist. We are just to throw in techniques that might be related to your problem...
like in grinding one tries to see/find the Go Direction of forces and puts a solid brace/blocking in that direction..same for milling.

Perhaps a 1" thick steel table off/above your mill table high enough to have thumb screws with lock nuts to hand screw up to bump the underside of your part every 1/2 inch or what to make a very solidly held part.

OPS ..I see that I already posted this advice in post #4.

 

[michiganbuck]

QT Op (I am currently using a 4 flute 1/4" .030" corner rad carbide end mill.)
The tap tap on the top side of your fixtured part with a steel knocker can/will tell if your part is solid to the underside. if a tap tap seems hollow, the part can vibrate while milling. If so then the part deflects away while being milled. (Under bumps screws with hand wing nuts to lock)
Next, you may try a more robust end mill, perhaps a 3/8"... and find a grinding shop that can Resharper your cutters. CNC sharpening shop to "grind off .050 from the end(only)with a .03 Rad", and end sharpen only would be the better choice for the price. Half the price of new would be a fair price. A CNC sharpening will have all the corner radiuses in the cut( a non-CMC shop may not have all the corner radiuses in the cut.
*Dull 12 cutters to send out..and ask for a bid.
Tapping hammer, you might tap with a long shank 3/8" Allen wrench with rounded corners or the line.

tapping hammer - Bing

Intelligent search from Bing makes it easier to quickly find what you’re looking for and rewards you.

www.bing.com