What's new
What's new

Looking for help with hard milling

Stang Bladeworks

Aluminum
Joined
Jul 9, 2019
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:
1656473593899.png
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.
1656473614815.png
Any advice is greatly appreciated. I am not a machinist so its more than possible I am missing something obvious here.
Thanks.
 

mhajicek

Titanium
Joined
May 11, 2017
Location
Minneapolis, MN, USA
You already know a lot of the answer. Get a cutter designed for hard steel, with as many flutes as possible, and use air blast. Use HSMAdvisor to get a starting point on your feeds and speeds; slowing down the cut from ideal or using coolant can actually shorten cutter life, because the heat is needed to soften the steel in the chip and activate the coating on the tool.

Maybe something like this:
 

5 axis Fidia guy

Stainless
Joined
Aug 17, 2006
Location
Wisconsin
You mention D-2 being similar. I cut allot of DC-53, which is carbide impregnated tool steel and it's a bitch to cut. I've tried just about every big name tool manufacture out there and none of them hold up worth a shit. SF in the range of 100 or 150 max, and that's crazy slow since I finish S-7 in the 500-700 SF range easily. I don't know what your rpm range is, but I might suggest finishing with a grinding wheel to get your desired finish. There a ceramic cup wheels made specifically for this purpose, Makino is the place to look for some info on this.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
Very nice work.
Perhaps having a very heavy fixture under the blade, 3/4" thick (or what() set off and above the table on very solid posts/legs with wing screws and hand-turned lock nuts from the underside that would be turned to touch the opposite blade side to increase the rigidity resting cutting forces.

The slightest vibration kills cutters.

The screws with a little pressure (finger tight and finger locked) would make the part (blade ) rock-solid like you were milling the 3/4" plate.

Such a fixture might even be angled (adjustable) if angled would help.

good to have a stout enough fixture that you can tap the part with a small hammer and feel no vibration.

For example, I used to wad a slug of modeling (children) clay on a grinding part that wanted to chatter. the weight of that slug took away the chatter.
 
Last edited:

Plane Parts

Aluminum
Joined
Apr 21, 2019
Lots of teeth. Maybe bump up to a 3/8 endmill. Look for a hydraulic collet setup and use VERY tight tolerance chucks, if you have lots of money. Another thing you might look at getting is a tool regrinder. You aren't plunging so you don't need center cutting. And it looks like you're only cutting with no more than 1/8" of the tip at max. After you wear out that 1/8 grind off the dull part and use that tool again. Might not be worth regringing the 1/4 but it would with the 3/8
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
Resharpening just the ends with snubbing off .050 is a very easy TC grinder task. good to dull perhaps 6 end mills and sharpen that many together to save set-up time.
It is not difficult to sharpen ends on a surface grinder. One-trick is you stand them up in a v block and flat grind the end...then when grinding the end to sharpen you just wipe away that flat grind so making them all the same length.

On a Tc grinder, you can just grind the next tooth off the tooth rest finger.

I am thinking that the milling is followed with a grinding operation?

QT(only get one blade out of a new tool. Which is about 140" of cutting. Even then, the finish isn't perfect.) makes it a pretty expensive operation.

The set screw backing fixture would be also good for a grinding operation
 
Last edited:

Orange Vise

Stainless
Joined
Feb 10, 2012
Location
California
Contrary to popular belief, hardmilling is easy, albeit tedious.

The secret to hardmilling? Swap out tools constantly and build this into your product cost.

Don't forget about the cost of labor in swapping tools. Even if you're just paying yourself in virtual "IOUs", it's costing you. You can mitigate this by having extra toolholders and/or fresh collets ready to go. Batch process the tool swaps rather than doing them one at a time.

I have tried a few things and my tool life is very short. I can only get one blade out of a new tool.

You answered your own question. Replace the tool with every blade.

Things could be much worse. You could have unpredictable tool life where some tools last for 10 blades and the next dies halfway through the first blade. If your tools consistently last the entirety of the first blade and then noticeably degrade in the second, consider this a win. The value of predictability cannot be overstated.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
Have you tried the tap test?
Tap a fixtured part where the cutter will cut to see if it vibrates, feeling it with your finger.

The rotational direction (right hand/Left hand) and feed direction of a cutter can be a factor if there is better part rigidity with one direction over the other.

looks like about $25 per end mill, that is a lot of money per blade.
Perhaps a CNC sharpening shop can run them ends only for $12 or so.
Good to send a dozen to a sharpening shop to get a better price.

Radius corners are better done on a CNC machine.
 
Last edited:

Stang Bladeworks

Aluminum
Joined
Jul 9, 2019
Resharpening just the ends with snubbing off .050 is a very easy TC grinder task. good to dull perhaps 6 end mills and sharpen that many together to save set-up time.
It is not difficult to sharpen ends on a surface grinder. One-trick is you stand them up in a v block and flat grind the end...then when grinding the end to sharpen you just wipe away that flat grind so making them all the same length.

On a Tc grinder, you can just grind the next tooth off the tooth rest finger.

I am thinking that the milling is followed with a grinding operation?

QT(only get one blade out of a new tool. Which is about 140" of cutting. Even then, the finish isn't perfect.) makes it a pretty expensive operation.

The set screw backing fixture would be also good for a grinding operation
Thanks for the advice. I'll have to look into sharpening and weigh out the pros and cons. There is no grinding operation after the milling, that's why I need the milled finish to be as good as possible.
 

Stang Bladeworks

Aluminum
Joined
Jul 9, 2019
Contrary to popular belief, hardmilling is easy, albeit tedious.

The secret to hardmilling? Swap out tools constantly and build this into your product cost.

Don't forget about the cost of labor in swapping tools. Even if you're just paying yourself in virtual "IOUs", it's costing you. You can mitigate this by having extra toolholders and/or fresh collets ready to go. Batch process the tool swaps rather than doing them one at a time.



You answered your own question. Replace the tool with every blade.

Things could be much worse. You could have unpredictable tool life where some tools last for 10 blades and the next dies halfway through the first blade. If your tools consistently last the entirety of the first blade and then noticeably degrade in the second, consider this a win. The value of predictability cannot be overstated.
Thanks, I feel I needed to hear this. I am still on the hunt for a tool that can reliably finish even one blade. I did order some hard mill tools and I'll see how that goes. To be honest I was hoping that that my tool life would have been an anomaly and someone would have pointed out an obvious mistake I was making. It kind of seems like burning through tools will be something I have to accept in this case.
 

Stang Bladeworks

Aluminum
Joined
Jul 9, 2019
Have you tried the tap test?
Tap a fixtured part where the cutter will cut to see if it vibrates, feeling it with your finger.

The rotational direction (right hand/Left hand) and feed direction of a cutter can be a factor if there is better part rigidity with one direction over the other.

looks like about $25 per end mill, that is a lot of money per blade.
Perhaps a CNC sharpening shop can run them ends only for $12 or so.
Good to send a dozen to a sharpening shop to get a better price.

Radius corners are better done on a CNC machine.
I haven't tried the tap test but I certainly will next time. I'll research a few sharpening places too.
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
When you are working on a magnet like surface grinding, you slide shims under the part to just fill the openings along any gaps and then turn on the magnet. that makes parts rock solid.
Clampdown mill jobs are the same, you want rock-solid if you can get it, in all direction the cutting forces might push.
 
Last edited:

BT Fabrication

Stainless
Joined
Nov 3, 2019
I would wonder if the curve right at the end of the blade is overloading it and chipping the teeth off as it makes it way around the radius. basically that radius increases the feed probably by 2-3X right at the end of the cut.
 

Tom-AMS

Plastic
Joined
Aug 27, 2020
Location
TEXAS, USA
Any advice is greatly appreciated. I am not a machinist so its more than possible I am missing something obvious here.
Thanks.
about few years ago, I milled similar hardened blades for a knife-maker in Glen RoseTexas. IRCC, material was a Japanese version of [email protected] - harder than woodpecker lips after heat treat. We called the "stair-step" surface "Kellering" . I used a YG-1 3/8 diameter insert-type end mill holder (ZRT1032) and 1/32 corner radius inserts (XR2A024 02) for up to 65 HRC. Blanks were roughed while "soft" with a 5-flute 3/8 x .030 corner radius end mill. I "nested" 4 blanks at a time on a fixture made from 3" thick slab of hot roll (no real reason, other than I hand, after a thinner 1" aluminum version of same failed due to vibration. Another thing I did was to leave an "eye" on the blades tip, for a hold down screw. The eye later ground off, leaving just the keller surface/sharp point). Machine /spindle rigidity is also critical. I was using a 10k pound 4-axis Atrump E320 with only 6k rpm spindle. IIRC, I finished at 2000 rpm, 25"/min, cutting 0.003" both radial and axial; with air blast - no coolant.
contact tech support at www.yg1usa.com Also ask about CNB inserts and maybe ceramic inserts. This is the only photo I could find - shows drilling handles for 5 blanks at a time, while held in soft jaws. I initially water-jetted the blanks, including the "eye" on tip.
 

Attachments

  • softjaw3.jpg
    softjaw3.jpg
    290 KB · Views: 23

cmccull166

Hot Rolled
Joined
Mar 29, 2013
Location
NW Pa
Have you looked into high feed end mills such as
mitsubishicarbide.com/en/products/rotating_tools/face_mills/ajx
maybe you could incorporate the taper on the insert to
eliminate the serrations left with the standard end mill.

Also ceramic endmills but expensive and your fixturing has to be rock solid.
 

D Nelson

Stainless
Joined
Jan 7, 2015
Location
Missouri Ida
Have you looked into high feed end mills such as
mitsubishicarbide.com/en/products/rotating_tools/face_mills/ajx
maybe you could incorporate the taper on the insert to
eliminate the serrations left with the standard end mill.

Also ceramic endmills but expensive and your fixturing has to be rock solid.
Go up and down the blade instead of long ways with about .06 rad Endmill about .01 step over it will be a better finish
 

michiganbuck

Diamond
Joined
Jun 28, 2012
Location
Mt Clemens, Michigan 48035
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 can't even get through a single blade without some imperfection.

Can you take a milling failure and grind the blade to save some value?

A set-on fixture that is rock solid heavy can help get longer tool life.
 

aarongough

Stainless
Joined
Oct 27, 2014
Location
Toronto, Canada
Hey Derek!
We have spoken a little on Instagram, but not in a fair while! I do a LOT of hard-milling for knife blades and have learned a lot through trial and error mainly... Here are some of the things I've learned:

Chip Clearing:
Air blast is very important to clear chips, prevent chip re-cutting and to help prevent the workpiece from slowly building up heat. Air blast MUST be well aimed, I use loc-line aimed at the tip of the cutting tool. Experiment with nozzle size to get good air velocity, too large of a nozzle will produce slow air without enough velocity to clear chips reliably.

Using air from your compressor to provide the air blast is expensive and noisy... The best source for air for this application is a small oil-free rotary vane air pump like the ones made by Gast. I use a little 1/4HP unit. Plumb it with BIG hoses as they don't make much pressure and you will lose a lot of airflow using normal 3/8" air-line. I am using 3/4" ID line like you'd use for a coolant pump. These are expensive to purchase ($750+ new) but can sometimes be found on ebay cheap. It will pay for itself quickly with cost saved on electricity and compressor maintenance!

Rigid Setup:
Rigidity of your setup, both in tool-holding and work-holding is absolutely vital. Any chatter in the cut will drastically reduce tool life. A squeaky chattery cut will cost you dearly vs a good cut that makes no noise, might reduce tool life by 90%!!

Use the shortest tool holders you possibly can, use the shortest stick-out on the tool that you possibly can, use the shortest flute length that you possibly can, use the most flutes that you possibly can. All of these things contribute to tool stiffness and optimizing this will get you HUGE gains in tool life.

Tooling:
Get the right tools. 4 flute tools are nowhere close to optimal for hard milling... big gullets and small tool core means the tool will be floppy like a noodle when hard milling! 6 flutes at a minimum and more if you can get them. Hard milling makes small chips so only small gullets are needed to clear them. More flutes means larger tool core which increases rigidity.

Bull-nose tools are the way to go for machining shallow contours. Ball-nose tools have practically zero SFM at the tool center and will die quickly when machining shallow contours like knife bevels, and they don't leave a very good finish either. Bull-nose tools with large corner radiuses are the way to go!
Avoid sharp-cornered (square) endmills, the corners will chip off quickly. Even a small corner radius helps drastically.

Toolpaths:
Prefer high-feed style roughing tool paths if you can make them work. Large stepover (90% of flat bottom of tool) and very shallow depth of cut (maybe 1% of tool diameter) plus slow RPM and high feedrate. This works really well for roughing and keeps workpiece cool with long tool life.

Some parameters from my process:
Material:
A2 Tool Steel heat-treated and tempered, 62-63 HRC
Tool: 1/4" Diameter, 8 flute, 3/8" length of cut, 0.06" Corner Radius, TIALN coated (Frank @ Maritool makes these for me custom, but they are publicly available) The same tool is used for roughing and finishing, fresh tool for finishing and then it's moved over to separate slot in the tool changer for roughing duty.
Toolholder: Maritool CAT40 ER25 holder, 1.85" Gage Length. Tool stickout below holder is about 0.625", could be shorter but I need the extra length to reach over some parts of my fixtures.

Cutting parameters:
'High Feed' roughing:
2,780 RPM, 80 IPM, 0.1235" WOC, 0.0025" DOC
Finishing: 7,500 RPM (all my machine has got), 96 IPM, 0.002" Stepover, 0.001" DOC

With these parameters I get approximately the following tool life:
- 352 minutes as a finisher
- 585 minutes as a rougher (after already being a finisher!)

Which works out to about 10 knife blades per tool, which is very economical.

Here is a photo of a blade finished using these parameters, bear in mind my machines are Fadals from 1994. Any more modern machine should get you even better results and possibly better tool life:


Hope this is helpful! Always happy to answer questions.
-Aaron
 

Stang Bladeworks

Aluminum
Joined
Jul 9, 2019
Hey Derek!
We have spoken a little on Instagram, but not in a fair while! I do a LOT of hard-milling for knife blades and have learned a lot through trial and error mainly... Here are some of the things I've learned:

Chip Clearing:
Air blast is very important to clear chips, prevent chip re-cutting and to help prevent the workpiece from slowly building up heat. Air blast MUST be well aimed, I use loc-line aimed at the tip of the cutting tool. Experiment with nozzle size to get good air velocity, too large of a nozzle will produce slow air without enough velocity to clear chips reliably.

Using air from your compressor to provide the air blast is expensive and noisy... The best source for air for this application is a small oil-free rotary vane air pump like the ones made by Gast. I use a little 1/4HP unit. Plumb it with BIG hoses as they don't make much pressure and you will lose a lot of airflow using normal 3/8" air-line. I am using 3/4" ID line like you'd use for a coolant pump. These are expensive to purchase ($750+ new) but can sometimes be found on ebay cheap. It will pay for itself quickly with cost saved on electricity and compressor maintenance!

Rigid Setup:
Rigidity of your setup, both in tool-holding and work-holding is absolutely vital. Any chatter in the cut will drastically reduce tool life. A squeaky chattery cut will cost you dearly vs a good cut that makes no noise, might reduce tool life by 90%!!

Use the shortest tool holders you possibly can, use the shortest stick-out on the tool that you possibly can, use the shortest flute length that you possibly can, use the most flutes that you possibly can. All of these things contribute to tool stiffness and optimizing this will get you HUGE gains in tool life.

Tooling:
Get the right tools. 4 flute tools are nowhere close to optimal for hard milling... big gullets and small tool core means the tool will be floppy like a noodle when hard milling! 6 flutes at a minimum and more if you can get them. Hard milling makes small chips so only small gullets are needed to clear them. More flutes means larger tool core which increases rigidity.

Bull-nose tools are the way to go for machining shallow contours. Ball-nose tools have practically zero SFM at the tool center and will die quickly when machining shallow contours like knife bevels, and they don't leave a very good finish either. Bull-nose tools with large corner radiuses are the way to go!
Avoid sharp-cornered (square) endmills, the corners will chip off quickly. Even a small corner radius helps drastically.

Toolpaths:
Prefer high-feed style roughing tool paths if you can make them work. Large stepover (90% of flat bottom of tool) and very shallow depth of cut (maybe 1% of tool diameter) plus slow RPM and high feedrate. This works really well for roughing and keeps workpiece cool with long tool life.

Some parameters from my process:
Material:
A2 Tool Steel heat-treated and tempered, 62-63 HRC
Tool: 1/4" Diameter, 8 flute, 3/8" length of cut, 0.06" Corner Radius, TIALN coated (Frank @ Maritool makes these for me custom, but they are publicly available) The same tool is used for roughing and finishing, fresh tool for finishing and then it's moved over to separate slot in the tool changer for roughing duty.
Toolholder: Maritool CAT40 ER25 holder, 1.85" Gage Length. Tool stickout below holder is about 0.625", could be shorter but I need the extra length to reach over some parts of my fixtures.

Cutting parameters:
'High Feed' roughing:
2,780 RPM, 80 IPM, 0.1235" WOC, 0.0025" DOC
Finishing: 7,500 RPM (all my machine has got), 96 IPM, 0.002" Stepover, 0.001" DOC

With these parameters I get approximately the following tool life:
- 352 minutes as a finisher
- 585 minutes as a rougher (after already being a finisher!)

Which works out to about 10 knife blades per tool, which is very economical.

Here is a photo of a blade finished using these parameters, bear in mind my machines are Fadals from 1994. Any more modern machine should get you even better results and possibly better tool life:


Hope this is helpful! Always happy to answer questions.
-Aaron
Hi Aaron,

Thanks for the reply. I have since found that I have been unable to get a decent finish with magnacut reliably using my old strategy. I ended up buying some 6 flute hard mill specific mills from lakeshore (.010" rad, .250" diameter).

I am still using my old contour toolpath in fusion but I adjusted my stepover to .00035" and ran it at lakeshores recommended speeds and feeds. I just did 5 blades that way and the finish isn't degrading yet. That being said the finish is OK but there is room to improve.

I am guessing that "contour" may not be the best toolpath for what I'm trying to achieve but I already had it set up. As is, the finish requires blasting in my opinion. I have ordered some die makers stones and a pneumatic tool to see what that does to the finish.

My end goal is to offer a stonewash finish with no media blasting required. Obviously if I could go right from the machine to the tumbler that would be better than messing around with stones. I am still leaving .0075" with a contour path before I heat treat. I remove this all in one pass using the smaller stepover.

The stepover lines are visible when viewed at the right angle but I cant detect them a fingernail. My current settings take 24 min per side to finish the bevel after heat treat. My settings are:
300sfm
4600rpm
66in/min
.0024in fpt (from fusion)

I did test my work holding with a tenths indicator to see if there is any movement. The glue seems surprisingly rigid. I had to really lean into it to move the tip a tenth. The cut sounds decent to my untrained ear. I did set up a makeshift air blast that works for now. The pump is a great idea.

I'll post a pic of my results, if you have any toolpath recommendations or anything else for that matter I would love to hear. I'll post up some results with the stones once I test them. Your machined finish looks a lot better. Do you have to stone anything? I know yours get coated but do you think you would be able to stonewash right off the machine if you wanted to?

I also realized my notifications must be off. I didn't know anyone had replied here. Thanks to everyone who replied. I will update as I learn more.

finish pic.JPG
 








 
Top