Help! > Machines, Tools and Fixtures
Horizontal Milling - Speeds and Feeds
Brendon M:
Hello
As you may know I have a Hercus "OLM" Horizontal Mill (see http://www.lathes.co.uk/hercusmiller/) and while it is a marvelous old Aussie iron machine, the one minor drawback is the info available to hobby machinists on how to really operate this thing in it's native mode. (There is a vertical head attachment for these but I didn't get one with this machine).
I had purchased a bunch of second hand cutters and have now since determined they are all blunt, after today's testing.
With the second hand cutters, I was constantly getting incredibly bad chatter (i.e. table shaking) and shrieking, regardless of RPM, feed rate, DOC etc.
I finally managed to track down a local company that will sell brand new horizontal cutters, and also got a NOS cutter from ebay.
I did some testing with the NOS 3 1/2 inch 7/16 wide cutter on some 10mm flatbar. Speed was estimated to be 98 RPM, and I went for 1mm DOC. The cutter was as close to the spindle as possible.
I once again got some bad chatter and producing metal needles. I have read this can happen because the feed rate is too low i.e. the teeth are rubbing instead of cutting.
Tried reducing to 0.5mm DOC and still no good.
Tried reducing the RPM to 74 RPM and the chatter was replaced with sort of squeal, but now the cutter was producing curled chips. The test flat bar had an increasing DOC due to previous milling attempts but the cutter was "happily" going through until it reached a max DOC of 4.5MM. At least I know it was the cutters and not the rigidity of the machine.
Edit: I should clarify that the Hercus has a 4 pulley belt drive with back gears just like the lathe plus an additional set of pulleys that require more effort to change but effectively doubles the ratios. I pick the closest ratio offered and use the VFD to adjust. Edit: VFD setup is running at 415V using a step up transformer so motor is running at full power.
I had to really feed this thing to keep up! Must have been completing a revolution of the X axis hand wheel around every 5 seconds, which is about 2 inches per minute! According to Little Machine Shop Speeds and Feeds calculator my 20 tooth cutter wants a feed rate of 28 inches per minute! :o
What I have read about horizontal cutters is that they can blunt if not using enough feed. Apparently running a slower RPM is no problem though.
So here is my question/pondering: can I get away with running a much lower RPM which would then theoretically allow me enough time to keep up with the feed rate? Or am I doomed to eventually blunting my cutters until I fit some sort of powerfeed? After all, at too lower SFM the cutter starts tearing instead of slicing.
Next on the list is either finding someone to sharpen them or be on the lookout for a Tool and Cutter Grinder.
Threads I have managed to find on the subject of speeds and feeds:
https://www.practicalmachinist.com/forum/threads/feed-speeds-on-horizontal-mill.90169/
https://www.practicalmachinist.com/forum/threads/spindle-speeds-for-horizontal-mill.113424/
https://www.practicalmachinist.com/forum/threads/help-computine-horizontal-mill-table-feed.297976/
https://www.practicalmachinist.com/forum/threads/horizontal-mill-depth-of-cut-or-utilization-of-machine-hp.236303/
Jasonb:
Your 20T cutter at 74rpm gives 1480 cuts per min, rigidity of the machine and motor power will determine what sort of chip load you can use but even if you said 5thou per tooth that would only give a feed of 1480 x 0.005 = 7.4"/min
Looks like the LMS site is working on about 0.020" chip load which is quite a lot
This maker gives cutting data for their side & face cutters, if you take the top row for free cutting mild steel and the 80mm diameter then the Fz (chipload) suggested is 0.07mm which is just under 3 thou. So 3 x 1480 = 4.440". A smaller machine may need to take off less.
https://www.zps-fn.cz/en/products/detail/narrow-side-and-face-milling-cutters,-type-n,-din,-high-speed-steel-hss-co5/
If Andrew is looking in he should be able to give you a better idea of what may work as he uses a horizontal, would help to know what sort of size and power your mill is, his one is 5HP
Jo:
I also have two horizontal mills which I normally use in vertical mode... And cutters up to 8" diameter :paranoia: and 6" wide slab mills
Speed of the cutter: The cutting speed is the main factor to determine tool life. A quick and dirty indication of cutter speed is to think if you were using a lathe to cut a piece of metal the diameter of the cutter how fast would you want the lathe spindle rotating? When in doubt use a lower speed.
Feed rate: those calculators are for professional shops who need to make a profit so they work their machines hard - it pays to work the cutters hard and regrind often. Not forgetting they use huge solid machines, not the little wimpy ones we use.. So Feed Rate is governed by tooth load: Too high a tooth load will result in poor finish, too low and it will cause rubbing, especially if the cutter is a bit worn.
The feed rate calculation is: Feed rate = Tooth load factor (=0.003) X Cutter Diameter X RPM X No of flutes = Inches per minute.
Depth of cut: The depth of cut should be as deep as the power of the machine will permit for the type of cutter. The critical factor for the type of cutter is the width of the cutting edge as a wider cutting edge needs more power to drive it through the work. Very light cuts should be avoided if the cutter is not dead sharp.
Blunt cutters: if the cutter is blunt then it is difficult to get either the speed or the feed rate to feel or sound right. You can use a stone to bring back a bit of an edge but better still find someone with a tool and cutter grinder :)
Jo
Brendon M:
@JasonB
My Hercus Mill is a hobby level machine :embarassed:
1/2 hp 415v 3 phase with a VFD to drive it
@Jo, thank you for that advice. Your formula suggests a 15 IPM which is still very quick
I have a picture where I was using a 2 inch shell mill to chomp through 1.5 inches of mild steel at 7mm, I believe this was utilising the full power of the machine.
The Shell mill cut absolutely wonderfully but most of the horizontal side milling cutters are straight tooth and I suppose are harder for the machine to drive
Jasonb:
--- Quote from: Jo on December 17, 2022, 08:18:17 AM ---
The feed rate calculation is: Feed rate = Tooth load factor (=0.003) X Cutter Diameter X RPM X No of flutes = Inches per minute.
Jo
--- End quote ---
Diameter does NOT factor in feed rates it is chip load, x Z (tooth count) x rpm as per my worked examples above,
Brendan this will reduce Jo's fast feed of 15"/min.
Diameter is used to work out spindle speed.
Navigation
[0] Message Index
[#] Next page
Go to full version