Home Workshop Mill Feeds & Speeds

[DaveH]

Given in the spirit of free knowledge. It welcomes discussion and even arguments (See if I care) ;D

It’s purpose is to promote a safe and knowledgeable start into Milling in the Home Workshop. It is not the “bee all and end all” by any means, just a start.

All you need is 5% knowledge (provided here) 5% skill you will have to provide that and 90% love, care and patience.

If I can do it so can you

Milling Speeds & Feeds.

These notes apply to Home Workshop Milling Machines covering the RF45/30 to the small bench top machines like the Sherline and Taig, in a normal milling operation.

The First 4 criteria.

A) Rigidity.
B) Rigidity
C) Rigidity
D) Rigidity

No not being funny - really important. More so than speeds and feeds.

A) The whole machine needs to be rigid, ideally bolted down –especially the bench types.
B) When moving 1 axis the other 2 must be locked. All the axis should be adjusted for minimum play. When using the hand wheel a slight drag should be felt.
C) The tool must be held in a rigid and proper manner, (a drill chuck is not good) and must remain such whilst rotating and cutting. A sloppy Z axis or quill will give a poor finish and can break your mills.
D) The work piece must be held in a rigid manner, this does not mean tightening the clamps as tight as you can. It means use 4 clamps instead of 2. Always try to mill against the fixed jaw if using a vice.

Slot Mill is only used to cut slots – that is what it is designed for.

The correct way to cut a slot whether an open or closed one is as follows:
Always cut in the same direction. At the end of the slot length raise the tool traverse back to the start, lower the tool and cut again. Cutting backwards and forwards will only make the slot over size and produces a poor finish. Keep removing the chips. The maximum depth of cut is half the diameter of the slot mill D/2. This is a maximum, it is not what you have to make the depth of cut.
On closed slots even though most slot mills are centre cutting, a hole drilled at the start can help to stop over sizing at the start. Hole size 50 – 80% of slot mill diameter.

End Mills are used for profiling – again that is what they are designed to do. Not facing using the end although we all do it. End mills should not be used for slots so the depth of cut has nothing to do with how deep the cut is as in the Slot mill. The depth of cut is how far the side of the mill goes into the work piece. The maximum depth of cut is ¼ of the diameter D/4, over a length D of the end Mill. For a 12 mm dia end mill on maximum cut will produce a step that is 12mm deep down into the work piece and 3mm deep (horizontal) into the work piece. A step 12mm deep 3mm wide.

So far so good, now comes the tricky bit.

It is the type of material that defines how it is cut, not the cutter. (Told you it was tricky) ;D
All materials have optimum cutting parameters, which are used in Industry, on big heavy rigid machines, with sharp cutters and a re-sharpened or new cutter every shift or ½ shift and flood coolant.
So we cannot just use these Industry parameters, they are just not suitable for the Home Workshop Mill.
However the data is still useful to us it gives us a good starting point.

“Please sir my cutter keeps on breaking” Huh some people are just bloody clumsy!

Cutter breakage is mainly caused by the following:

1) Feed rate too high. (The table is moving too fast)
2) Speed too slow (Spindle RPM is too slow)
3) Depth of cut too big.(Biting off more than you can chew)
4) Build up of chips. On the cutter, in the slot.

Not just one of the above can break your mill but 2 or 3 or all 4 working together can, so there is a lot out to get you!
They also give us the poor finishes.

Now the bit you are all waiting for how fast must my ½” end mill go?

Well disappointing not fast – more like how slow. Compared to what is used in Industry.

Let’s look at the data.

Feed. This is a measure of how far the table travels per tooth of the cutter, eg. Feed is .003” for mild steel, so on a 4 tooth cutter the table can move 4 x .003” = .012” per revolution of the cutter; because each tooth will cut .003”.

Cutting speed. This tells you how fast the cutter can go(RPM) The type of cutter (HSS / Carbide) and the work piece material determine it. The cutting speed is given in feet per minute (or Metres per minute). So for steel and HSS end mill this is 150 to 200 ft/min. To get the spindle speed all we have to do is divide the cutter’s circumference into the cutting speed. The distance around the ½’ cutter is = Pi x Dia.= the circumference. But (and there is always a but) everything needs to be in inches (or mm in metric). We will take 200 x12 makes it inches and we divide the circumference of the cutter into it. Thus (200 x 12) / (3.142 x 0.5) = approx 1500 RPM ( in your dreams) half it 750 RPM.
Now you have the speed of the ½” cutter 750RPM (fair whizzing eh!) Disappointed! you are an adult get over it!

All we need now is how fast can we move (travel) the table – more slow than fast.
We have from the Feed .012” per revolution, so 750 revolutions per min x .012” = 9” per minute. Too quick for us so half it.
Here it is then - ½” 4 flute HSS cutter @ 750rpm and a feed rate (table movement) of 4.5” per min.
Nearly finished! -Still with it.
This is all at the maximum depth of cut of 1/8” D/4. Until you get to know your machine and the material you are cutting lets start with 1/32” depth of cut. Listen to the machine – feel the vibrations. The machine will let you know if it does not like it.

If all seems well, increase the depth of cut – keep clearing the chips away! This is your starting point, try increasing the feed rate first – then increase the speed say to 1000rpm listen, watch and feel the machine. Be careful not to just increase the speed RPM because the cutter will get too hot.

The cutter must always cut never rub – rubbing will blunt the cutter in no time.

Remember the chips come off fast and hot; be careful – try to preserve your one good eye! ;D

So why does industry like the carbide end mills so much.

You said it is the material that defines the cut not the cutter.
I did and it does, a carbide mill Feed is still .003” same as the HSS but the carbide can go 2 to 3 time faster, therefore the feed rate (table speed) is 2 to 3 times quicker. Job done in 1/2 to1/3 rd of the time.

But sadly not for you or me our machines are just not rigid enough for those sorts of speeds and feed rates. Nevertheless there are some benefits for us, they will stay sharper longer than a HSS and we can run 50% faster and thus increase the feed rate by 25% to 50% . or just run them at the same speed, feed rate and depth of cut as HSS cutters and they will last a lot longer.

Another way to use carbide mills is to increase the speed by 50%, leave the feed rate and decrease the depth of cut to .005” to improve the quality of the finish. A finishing cut. ;D

The above covers slot and end mills 3mm (1/8”) to 20mm (3/4”) normal conventional milling.

Slot and end mills below 3mm are another story.

Happy milling

DaveH

 

[Anko]

Hi DaveH!

great info!

Im just curious, but how bad are if you not clean the chips during cutting?

I have a manual machine (mini mill) and cuting get my two hands bussy with the feed and lubricant, if I want to clean the chips I need to stop the machine and clean with a vacuum cleaner, so just let the chips there until I finish the pass, then use the vacuum cleaner

is there some kind of danger to the endmill?? I most use 4 flutes on steel

there is a secret technique to clean the chips during cutting that not involve powerfull coolant flow rate??

anyway thanks a lot for the info!!

Saludos

 

[DaveH]

Saludos.
Chips can and will break your cutter one day. The more blunt the cutter greater the chance. Mainly cutters below 12mm dia, and you won't see it coming either.
I blow the chips off the cutter and immediate cutting area with air, sort of a hard puff, or a gentle blast, every 4-8 secs.
The major problem arises in cutting closed slots, with small cutters say below 4mm here the chips can be a real problem.
Last thing all those chips can also mar your finish.

Hope that's helped.

Dave

 

[Bill S]

Thanks for the write-up Dave. How do you tell a slot mill from an end mill?

Bill

 

[DaveH]

Hi Bill,

Slot mill has only 2 flutes and nearly always (99%) has centre cutting.

Looking at the bottom of the mill you will see one of the cutting edges goes right up to the centre.

This allow you "plunge" the cutter in to the work piece.

4 flutes always an end mill. Normally no centre cutting.

Hope this helps ;D

Dave

 

[Bill S]

Thanks for the clarification, now how do 3 flute end mills fit into the equation?

Bill

 

[DaveH]

Hi Bill,

Introduced in an attempt to have a cutter that could cut slots and profile without having to change tools.

The finish from the 3 flute when profiling is not as good as the 4 flute.

Now in the home workshop where time is not the main concern the finish can nearly be over come. (Sometimes the finish may not be that important).

So buying one cutter to do 2 jobs is quite a cost saving.

One last point Industry is quick to catch on, so if the 3 flute in it’s duel roll was as good as 2 and 4 flute mills, there would not be any 2 or 4 flute mills about.

I can remember when we used 6 flute end mills. ;D

Dave

 

[deverett]

Good information there, Dave.

Dave
The Emerald Isle

 

[ruzzie]

Hi
Just to start another debate on using end mills to cut slots or drill holes, the end mills I use have 4 flute with two 2 flutes going to the center like a slot drill which allows it to drill a hole.
They are made by Sutton Tools here in Australia

 

[DaveH]

Hello Ruzzie,

Interesting end mills you have brought up. ;D

Now I say end mills because the box in your photo says ENDMILL so these are end mills, 4 flutes with centre cutting. They are not slot mills. So what gives me the right to say that? Well slot mills have a minus tolerance on their diameter and end mills have a plus tolerance on their diameter. This tolerance difference is fundamental to slot or end mills. It tries to make sure that a slot mill does not cut over size.
The end mill has a plus tolerance on D its diameter; this along with the cutting geometry is why slots with end mills tend to be over size.

Having said all that I think they are a great idea especially for the home machinist, including slotting. ;D

The one you have shown are 4mm dia. and whilst a 4mm slot may be over sized a 5mm slot won’t be.

This is how sometimes I cut slots, by enlarging the slot each side of the original slot. I like this idea to cut slots because I can slowly creep up on it without it knowing and get the exact width of slot I want and I also get a much better finish because I am using the end mill in a profiling mode. ;D

Thanks Ruzzie for bringing them up makes for an interesting discussion.

Dave

 

[TroyO]

Hmmm, why are they called *end* mills, if they are supposed to be used for profiling/side milling? (I know... the same reason we drive on the parkways and park in the driveway!) I wonder if it differs depending on "What side of the pond" you are from? I recently found out that "Ball mills" are more properly called "Hemispherical nose mills" as the term "Ball mill" means something entirely different.

http://en.wikipedia.org/wiki/Ball_mill

I also generally see 2 flute cutters listed as "end mills" in catalogs. How does one tell?
(IE http://www.use-enco.com/CGI/INPDFF?PMPAGE=139&PMITEM=328-0084

If it is a "center cutting 4 flute end mill", is it really then just a misnamed 4 flute slot drill? (Again... Slot Drill is the term on Wikipedia.... not that it's like the infallible source or something.)
http://en.wikipedia.org/wiki/Milling_cutter

I had heard (somewhere?) that the 2/3/4 flute decision was guided by 1) How fast your spindle goes and 2) Chip clearance for the material in question. In other words, the cut per flute remains the same but half the flutes run twice as fast to attain the same cut per tooth.

If the ideal rate on a 2 flute is say 6,000 RPM but your mill only goes 4,000 RPM then you should move to a 3 flute.... and so on. If you are having chip clearance issues with a 3 flute, speed up the spindle and use a 2 flute.. Etc.

Le-sigh..... probably what I find to be one of the most confusing aspects of machining, LOL. The charts are wrong, the tables are wrong (Being based on an assumed perfectly rigid machine and ummm.. “Optimistic” manufacturers specs), the names are wrong, I have neither a RPM gauge, nor a IPM gauge, the surprising thing seems to be that it works at all,

It has been a steep learning curve (Opps, burned that one! Yikes, that one got clogged with chips! How long do I have to stand here and crank so slowly I fall asleep?) But I *think* I have been getting the hang of it.

You know.... until I break the next one....

 

[tel]

Rof}

Confusing, ain't it! Yeah, a ball mill is a rock crushing machine! 'Ball-end mill', 'round nose end mill' , 'round nose mill' all crop up and the ones from out mate at Richon are labelled 'tapered end mill'. It doesn't only vary from country to country but also from state to state - probably town to town in some places!

 

[DaveH]

Troy,

Interesting post.

I don’t know how the word “end” originated may be someone may be able to answer that one. The word “mill” came from “milling machine” and was shortened by common usage to “mill”. Although I suppose it is hardly a mill, in the old proper sense of the word.

Ball mill tends to be an UK term, here I call them ball nose, hemispherical nose – well a bit “posh” for me! :big:

If the supplier calls it an end mill albeit a 2 fluted one, then it is 99% an end mill. 2 fluted end mills are used mainly in Industry to take off big chunks of metal. More metal can be removed without breakage using a 2 flute mill than with a 4 flute mill. (Chip removal within the flutes)

A “slot drill” is the more preferred term than my “slot mill” ( Being old does have it’s excuses ) :

Quote If it is a "center cutting 4 flute end mill", is it really then just a misnamed 4 flute slot drill? Definitely not, it would probably come under some legal thing – as misleading.

A slot drill must be made very slightly under it’s nominal size in accordance with the appropriate standard(s).
An end mill must not go under it’s nominal size, again standards.

Quote If the ideal rate on a 2 flute is say 6,000 RPM but your mill only goes 4,000 RPM then you should move to a 3 flute.... and so on. If you are having chip clearance issues with a 3 flute, speed up the spindle and use a 2 flute.. Etc Absolutely correct.
Just remember lots of chips and lots of speed = lots of heat – not good for the cutter.

All the charts and tables are for Industrial use and like you say perhaps a bit of commercial “optimism” goes on a little. Never do the say if yours is a home type mill this data should be halved.!

Not only is it a steep learning curve I think it is a difficult one as well, but TroyO you have mastered it well done. ;D

Yea turning that handle is a real pain but you have just modified your mill X axis, I hope you took notice of my post suggesting you need a slow speed.

TroyO You have got the hang of it – more art than science, congratulations. :bow:

Thanks for your post - remember others will learn also.

Dave

 

[DaveH]

Tel,

Rof}
even house to house,
Rof}
what would we do without you Tel?

Rof} Rof} Rof}

Luv ya
Dave

 

[TroyO]

Not only is it a steep learning curve I think it is a difficult one as well, but TroyO you have mastered it well done. ;D

Here's some more fall-down laughy-guys.....
Rof} Rof} Rof} Rof} Rof} Rof} Rof}

I have mastered nothing! And even if I had I would never admit it! :big:

The power feed sure is nice though.... and it does go down to something less than 1 IPM if you are gentle with the dial.

On the plus side, I can crank it up and break end mills (Or slot drills, or whatever the heck they are) faster than ever before!

I did at one point consider hacking up some drill rod and using it as cutters.... you know, no teeth or anything. Why spend all that time taking the teeth off end mills when you can make one that way from scratch right off the bat?

On a more serious side... that is exactly why I buy dirt cheap cutters. My end mills are still way more likely to fail through misadventure than getting dull. As soon as I legitimately “Dull” an end mill through use I will double my end mill budget. (I might even pay a whole $5 for one then! ;-)

Until then.... I see no point spending big money on “Educational” tooling.

 

[DaveH]

Hi TroyO,

Someone once asked Edison (this is the guy all the Americans think invented the incandescent lamp) “don’t you think you are wasting your time this is your 20th attempt”, Edison replied “No - I know 19 ways how not to make it”

Only people who have broken end mills Know how to mill. ;D

The only people in the World who never make mistakes are those who never do anything. ;D

You are as near as damn it there, can’t rush these things especially home milling.

Slow and easy, small cuts, slow speed, and just build it up.

Gary Player said –“Do you know the more I practice the luckier I get”

Just make it fun ;D But mind your eyes and fingers.

Dave

 

[ruzzie]

:wall: Remember not to confuse your Ball nose with your Bull nose :wall:

 

[TroyO]

Hey, I have both kinds of end mills..... gold AND silver! :bow:

One thing that sold me on getting a DRO was exactly the information I mentioned before, IPM and SFPM. It actually calculates it out and displays it in real time, how cool is that?

IPM is cool enough, but calculating out the SFPM and displaying it live could be an invaluable piece of info.

 

[shred]

FWIW, if you ask for a 'slot mill' anywhere around here, they'll just look at you like you're daft. We have end mills. 2-flute, 4 flute, center-cutting and not (plus all the oddities in ball-ends, 3,5,8.. flutes, angles, etc). The 'end' is because they stick out the end of those newfangled verrteecal milling machines, not lashed securely to a horizontal arbor and overarm like Gorton intended.

 

[tel]

That's cos you have to ask for a 'slot drill'