Milling around with bits

[Stuart Munro 1Participant @stuartmunro1]

Discussing the merits and uses of different types of mill bits

[Stuart Munro 1Participant @stuartmunro1]

Hi,

I'm a relatively new member, and a very new engineer. 67 years young with all of a year or so playing with metal. I'm gradually getting to grips with topics such as the use of different types of mill bits but want to test my limited academic knowledge alongside real world experience. This section has many references to suitable mill bits but I thought pulling this experience together would help apprentices like me.

To start the ball rolling, can I put raise a few mistakes that I've made and elicit any thoughts, from 'what an idiot and clearly no engineer' (both alas true) to what I should have done/used.

1/ Cutting Brass: I make small brass and aluminium components. I read that Uncoated HSS is the right way to go for brass and this was great initially. But I was not cutting deep enough to get a good finish – getting chatter. As my confidence grew I cut faster (moved the table into the brass faster with a deeper cut) and this seemed to work better until the bit dug into the brass.

So I now read that the cutting angle of the flutes is important. Can anyone explain this and suggest an approach to milling brass?

2/ Indexing: I moved onto aluminium and found this to be much harder to mill with regular hard judders as the tips of the mill bits broke. I've purchased mill bits that are stated as correct for non-ferrous metals and I've been very careful to fix the work piece securely but still get the problem. Is indexing the way to go and is this realistic with a MT1 taper shaft? I've experimented with indexed tools on my lathe (Sherline) to avoid sharpening HSS tool bits and this cuts efficiently, but not with a very smooth finish!

3/ Clamping the tool: generally confused about the advantages and disadvantages of Weldon bits to tool holders vs the range of collet types available. Perhaps it's the clamping of my bits to the mill that is my weak point?

I'd very much welcome any input from experienced engineers, and questions from other trainees like myself.

Thanks

Stuart Munro

[Stuart Munro 1Participant @stuartmunro1]

ps. from this site, I've had some very good advice on different types of aluminium and their suitability for milling; I've bought aluminium from GLR Kennions listed as good machinability so I'm confident the error is with me, not the metal.

Stuart

[Ian ParkinParticipant @ianparkin39383]

For alloy lubricate  copiously with wd40 to stop tip build up

Edited By Ian Parkin on 16/04/2021 17:21:56

[Martin ConnellyParticipant @martinconnelly55370]

Do you understand the difference between climb milling and conventional milling, it sounds like you may be climb milling on a machine that is not suited to it (juddering). There is a guide that can be reached from the home page but here is a link anyway.

Why climb mill?

Also as Ian said aluminium and its various alloys can easily clog up the flutes or stick to the cutting edge which causes problems. The fewer flutes the better with these metals, you can get special cutters with one flute but mostly two works ok, three at a push and avoid 4 flutes. Use polished cutters not coated as well. As soon as the cutting action starts to change stop at a convenient point and check for build up on the cutter. Some people suggest paraffin as a lubricant for aluminium but the smell is quite strong and you probably don't want a build up of flammable fumes in a workshop.

There are rules of thumb for cutting depth based on the tool diameter and you should learn about speeds (rpm) and feeds (thickness being cut by each pass of a cutting edge) to avoid either rubbing or overstressing the tooling and machine. There are online calculators to help with feeds and speeds.

Martin C

[Stuart Munro 1Participant @stuartmunro1]

Ian, thanks for this – I'm advised that Brass does not need lubrication and went on to treat aly alloy the same. Error no.1!

Can anyone explain the importance of the angle on the flutes (I think its called the helix angle). It seems that for Brass (I've not looked for Aluminium alloy) that mill bits with the correct helix are quite expensive so it would be useful to know why this is important to help decide if the expensive bits are worth it?

The same question presumably applies to Aluminium, but equally a different angle. If so, is my choice of 'non ferrous' bits too general in that one type does not suit both brass and aluminium? Perhaps my 'one fits all' bits are not appropriate for Brass nor Aluminium.

Argh, number of flutes, helix angle, coated or uncoated, type of shank…..now to lubricate or not. That's before discussing SPM, feed rate etc. You engineers know an awful lot of interesting stuff. I can read a lot on the 'net' but would really like to know what really works and why.

Thanks in anticipation

Stuart

[Howard LewisParticipant @howardlewis46836]

What speeds and feed rates are you using?

It is assumed that the work is rigidly clamped, and that your machine has minimal backlash on all axes, with the unused ones being clamped.

Similarly, cutters should be clamped as firmly as possible with minimal overhang.

Feed rates should be based on cutter speed, number of flutes and feed per tooth.

CUTTING SPEEDS

With HSS cutters, taken from my Apprentice Training Notes; think in terms of:

For soft Brass Roughing, 200 – 300 fpm Finishing 600 – 700 fpm

For hard Brass Roughing 150 – 200 fpm Finishing 200 – 300 fpm

Aluminium Roughing 400 -500 fpm Finishing 600 – 700 fpm

FEED per TOOTH Face Mill Slot Drlll End Milll Slitting Saw

Free Cutting Brass 0.022" 0.013" 0.011 0.005"

Hard Brass 0.009" 0.008" 0.005" 0.002"

Aluminium 0.022" 0.013" 0.011" 0.005"

HTH

Howard

[Howard LewisParticipant @howardlewis46836]

Climb milling will give improved surface finish, ON A MACHINE DESIGNED FOR SUCH WORK, with backlash prevention devices.

Hobby machines are NOT!

You are likely to have the cutter grab and pull the work into it with the risk of damage to both.

The work should travel so that the motion opposes that of the cutter tooth.

Howard.

[Tony Pratt 1Participant @tonypratt1]

Always use sharp cutters for Ally & brass & Ally needs lubricating to stop what is called 'pick up' where the cut material sticks to the cutter, on Ally I personally use Paraffin or even cutting oil at home but when I worked on CNC machines we used a water soluble cutting fluid.

Tony

[JasonBModerator @jasonb]

I think you may be getting mixed up with helix angles for drilling brass where a low or no helix angle is desirable to stop the drill bit being pulled into the work, this does not really apply to milling cutters.

Cutters made specifically for aluminium will also work well on brass and bronze. These tend to have a higher helix angle which is mainly used to help remove the larger volumes of swarf that can be produced from these faster cutting materials.

I think you mentioned that you also have a Sherline mill so quite light and only able to use relatively small cutters so some of those chip loadings mentioned above will need to be reduced as the small cutters are not as strong. For the same reason your depth of cut and approach (sideways depth) will also need to be less than larger machines can manage. 

Climb milling can be used with care on most machines but on the lighter ones it is best kept as a very light finishing pass rather than a way to hog out the majority of the material.

Edited By JasonB on 16/04/2021 18:48:02

[SillyOldDufferModerator @sillyoldduffer]

Posted by Stuart Munro 1 on 16/04/2021 17:56:59:….

Argh, number of flutes, helix angle, coated or uncoated, type of shank…..now to lubricate or not. That's before discussing SPM, feed rate etc. … can read a lot on the 'net' but would really like to know what really works and why.

…

 

Well I like to keep it simple! I use the same coated HSS cutters on steel, brass and Aluminium, simply adjusting feed rate, depth of cut and RPM for best results.

Two flue cutters, aka slot drills. can plunge and cut slots. The big gap between flutes helps eject swarf. Four flute cutters are for flattening and edge cutting – they remove metal faster and produce a better finish provided the swarf can get out of the way. They can't plunge (usually). Keep meaning to try some 3 flute cutters, which are a compromise between 2 and 4 flutes, but never got round to it.

Coated cutters have a thin covering of something extra hard like Titanium Nitride to extend tool life, but Aluminium tends to weld to it, spoiling cut and finish. Not a big problem if spotted because the Aluminium can usually be scraped off, or dissolved in Caustic Soda solution, though having to stop does delay work.

I don't lubricate brass or cast-iron. Aluminium benefits from a light oil such as paraffin or WD40. On steel I use neat cutting oil, mainly because I have an irrational fear of suds causing rust. Or I go gently and don't lubricate at at all.

RPM, DOC and feed-rate are all a rule of thumb. Recommended industrial parameters are chosen to balance tool-life, metal removal rate, and economic use of power. They are more aggressive than most hobby machines are comfortable with, so back off! Don't expect a Sherline mini-mill to perform lanything ike a hefty Horizontal milling machine

I determine RPM by dividing 10000 by the cutter diameter in mm. This is about right for mild-steel, increase for Brass and Aluminium. Slow down by half for cast-iron. Depth of cut, up to 10% of the diameter of the cutter, feed rate fairly fast. It's important to cut rather than rub. I adjust DOC and feed-rate by ear; I like the mill to sound as if it's working, but not labouring. Reduce rpm if chatter occurs, and increase DOC and feed-rate so it sounds right. The exception is finishing cuts, which can be much lighter or climb milled, but avoid climb milling whilst taking deep cuts because 'our' machines are too weedy!

All this assumes the material is a machinable alloy rather than unknown scrap. Many alloys don't machine well, and some are downright evil! Learn on the right stuff so you know what to expect before experimenting with scrap just in case your junk box is full of rubbish. Mine was!

Dave

ps I don't think the people I buy cutters from offer different helix angles!  As I understand it, they are optimised for roughing or finish, or in between.  I think mine are all 'in between'.  I doubt helix angle matters unless something special is in hand.

 

Edited By SillyOldDuffer on 16/04/2021 19:45:07

[Martin KyteParticipant @martinkyte99762]

For creating flat surfaces on aluminium as opposed to slots and steps I suggest you fly cut . I use an insert for aluminium in a fly cutter and produce a mirror surface cutting dry.

regards Martin

[Anonymous]

Posted by SillyOldDuffer on 16/04/2021 19:27:06:

ps I don't think the people I buy cutters from offer different helix angles! As I understand it, they are optimised for roughing or finish, or in between.

It's more dependent upon material. Cutters intended for aluminium often have high helix flutes. But they are only advantageous if one can run at the high speeds and feeds required. Similarly for tough materials cutters can have esoteric coatings and variable helix angle and/or flute spacing to reduce chatter. Again one needs a mill that is capable of utilising the features.

I don't regard my Bridgeport as being able to make proper use of the fancy cutters, so I don't buy them, other than polished cutters for aluminium.

Andrew

[old martParticipant @oldmart]

Assuming you have only a small ammount of backlash on the Xaxis, say 0.01", 0.25mm, you can get away with climb milling using shallower depth of cut than conventional and applying a little braking from the locks. This is useful for the finish cut which will be smoother.

[Stuart Munro 1Participant @stuartmunro1]

Thanks everyone. I was aware of climb milling and plan to mill conventionally except a very light cut to finish where I find climb milling is preferable.

As to milling speeds, for a novice without someone looking over my shoulder its quite unnerving pushing the feed rate up yet I theoretically understand that the balance between Surface feet per min (Have I got the term right), the cut depth and feed rate sometimes needs me to increase feed rate. As an alternative I reduce the RPM.

Dave – your 'feel the right rate' view makes sense to me which I hope comes with practice.

But I've not been lubricating on my mill; I have an oil/water mix a friend gave me for a bit of iron I turned on m lathe – also a Sherline. But might try the WD40 – seems to be akin the the wild west elixir cure all but for engineers!

I clearly misunderstood the whole helix angle thing but got he coated vs uncoated bit right – although I still don't understand quite why – important to my satisfaction not to the machining as long as I follow the 'rules'. Is it that somehow uncoated cutters are sharper because the coating itself thickens the cutting edge? But without this the sharp uncoated cutters will blunt quickly. This moves me towards heap (I see Arc Euro and ACCU selling 2 flute 8mm uncoated bits for £3 – £4. Use one for a few days and throw it away!

I don't want to hog every ones time so if there are any other ex office dwellers moving into a useful pastime in retirement perhaps you have some questions. If not, any thoughts on holding the bits; I use tool holders and weldon mills but most people use collets. Why?

Many thanks

Stuart

[Anonymous]

Posted by Stuart Munro 1 on 16/04/2021 22:02:02:

If not, any thoughts on holding the bits; I use tool holders and weldon mills but most people use collets. Why?

Not me. On the Bridgeport and CNC mill I mostly use the Tormach TTS system. My two main holders are 6mm and 10mm side lock, used with carbide cutters with no flat. They're simple and have a short overhang so one can run the cutters hard, note the blue swarf:

For cutters other than 6 or 10mm I use ER collets, this one is 4mm:

I have a selection of Autolock style chucks, mainly used with HSS cutters, imperial and metric:

I also use sidelock holders with larger cutters (1" slot drill in this case) for convenience:

I have been known to use a milling cutter in a drill chuck. Personally I use whatever holder I think is suitable for the job in hand and don't worry what other people do.

Modern carbide cutters with coatings are pretty darn sharp, and will slice a finger just like a scalpel – I speak from bloody experience. For aluminium I use uncoated and polished cutters, as it reduces the tendency for the swarf to stick to the cutter. For other materials I use mid-price cutters with TiAlN, or similar, coatings. I suspect my mills will not run fast enough to use the more esoteric coatings – so I don't waste money on them. Neither do I machine the really tough materials and 'orrid materials, like inconel. The coatings generally provide a thin, but very hard, surface to counteract wear and pitting from the swarf. But as always the devil is in the detail. With TiAlN the aluminium helps with lubricity meaning the swarf slips more easily. but the coating needs to be very hot for the aluminium to do its job. So running a TiAlN cutter at slow speeds doesn't make use of the coating.

Andrew

[Stuart Munro 1Participant @stuartmunro1]

Thanks all. So to summarise for anyone coming to this blog in the future.

We have mainly focussed on Aluminium alloys as the object material. To mill this effectively:

1/ Use uncoated polished two flute mill bits. The consensus is that these are both sharp and as effective as possible at removing swarf.

2/ Nevertheless, lubricant is advisable, paraffin is effective but pungent and runs the possibility of fumes building up. WD40 is another option. The lubricant is unlikely to be enough to remove all swarf so it is advisable to check the bit periodically and manually remove swarf.

3/ The exact type and grade of aluminium alloy is important. Some cheap aluminium is very difficult to machine. Source the aluminium carefully from a reputable supplier (see elsewhere on this site).

4/ Speed of cutting; Remember the relationship between RPM and Surface Feet per Minute (SFM). Lower diameter bits must rotate faster to achieve the same SFM. My Sherline mills came with a chart of recommended SFM for various materials (including 3 grades of Aluminium) so presumably all milling machines are provided with such information. Howard Lewis summarises similar information above. Take care to get the feed rate and depth of cut right. Some commentators mention that experience allows them the 'feel' and hear the mill to know that they have this right. My reading indicates that the swarf coming off – with aluminium in particular – is indicative of a good cut if it 'spirals'.

5/ Conventional milling vs climb milling. Smaller machines tend not to be as rigid as say a Bridgeport and can not hold a piece and bit firmly enough to climb mill unless it is a very shallow cut aimed at producing a fine finish. The bulk of milling should be conventional where the feed across the surface of the aluminium is against the rotation of the bit.

6/ Holding the bits in the mill; it seems to be personal preference which method of securing the bit is used when 'hobby' milling. High speed industrial work and/or very high precision may require specialist collets. On my Sherling a tool holder with side screw holding a weldon shaft is efficient – similar to but much smaller than Andrew Johnsons Bridgeport Tormach TTS system in the prevoius blog.

7/ Some discussion on specialist coatings of mill bits; TiAIN can be useful but at high speeds as it needs to be hot to work well, smaller and/or non industrial use will be unlikely to be sufficiently fast to achieve the heat needed. More esoteric coatings will generally suffer in the same way. The conclusion is that for the hobbyist cheaper uncoated and polished bits are preferable.

Many thanks everyone for your contribution

Stuart

[JasonBModerator @jasonb]

1. Although a lot of aluminium specific cutters are two flute I would not rule out using more flutes provided the cutter was sharp and uncoated. About 50% of the time on the manual mill ill use 3-flute cutters on aluminium and even on the CNC maybe 75% of the time I go to 3-flute carbide high helix cutters depending on the size of cutter being used and the type of cut. I don't push my machine hard enough or have a high enough spindle speed to really produce the amount of swarf.

2. Yes lubricate. That smell from Paraffin has it's advantages as it will mostly evaporate out of the swarf and off the machine where WD40 can leave a sticky film. It's not been mentioned but if going with WD40 then get the 5lts can and pump spray as it's a lot cheaper than aerosol cans.

3. It's not just cheap aluminium that can be hard to machine as you can pay good money for know grades that are not free machining. More a case of knowing what grades machine well and suit the particular job and then buying them rather than using "unknown" material.

4. Very few milling machines will have any suggestions for cutting parameters included with them

5.Yes on small hobby machines keep climb milling for light finish cuts

6. Holding can be a personal thing, although I do have side lock holders I seldom use them as I find the ER more versatile and rather than having to keep raising and lowering the head to take sidelock cutters out of the spindle I can hold all sorts in the ER such as edge finder, drills, small flycutter, milling cutters, etc.

7. I don't give much thought to coatings apart from trying to avoid them on aluminium but sometimes its a case of a particular cutter not being easily available without coating so may have to make do.

[Tony Pratt 1Participant @tonypratt1]

Sharp 2, 3, 4 flute cutters are fine on Aluminium. In fact if you need to do a deep pocket or similar 2 flute 'slot drill' cutting edges are generally not as long as 'end mills' so they may not be an option.

Tony

[JasonBModerator @jasonb]

Luckily you can get long series aluminium specific cutters with long flute lengths not just extended shanks that will have far longer flutes than a "standard" endmill if you do have a need for deep pocketing. I was down 4.5D during the week and still had a bit of length to spare on an 8mm cutter (36mm deep slot)

[SillyOldDufferModerator @sillyoldduffer]

Posted by Stuart Munro 1 on 16/04/2021 22:02:02:

…

As to milling speeds, for a novice without someone looking over my shoulder its quite unnerving pushing the feed rate up yet I theoretically understand that the balance between Surface feet per min (Have I got the term right), the cut depth and feed rate sometimes needs me to increase feed rate. As an alternative I reduce the RPM.

…

But I've not been lubricating on my mill; I have an oil/water mix a friend gave me for a bit of iron I turned on m lathe – also a Sherline. But might try the WD40 – seems to be akin the the wild west elixir cure all but for engineers!

… although I still don't understand quite why – important to my satisfaction not to the machining as long as I follow the 'rules'. Is it that somehow uncoated cutters are sharper because the coating itself thickens the cutting edge?…

… any other ex office dwellers moving into a useful pastime in retirement …

Stuart

In reverse order:

• ex-Office dwellers are the salt of the earth!
• Don't get hung up on 'rules' : look on them as guidelines. The number of combinations of rpm, doc and feed-rate that will cut satisfactorily is often broad and the sweet spot is often determined by the limitations of your machine and cutter relative to the material rather than the book. Use a rule a thumb to get into the zone and experiment for best results. Varies by machine: heavy, rigid, powerful machines are more tolerant than light, bendy, weedy ones. Hobby machines are all on the light side. By all means look up Surface Feet per Minute, but working from rpm = 10000/dia in mm is more scientific than it looks. Be aware time is far more important to professionals than hobbyists: time is money. Handbook cutting speeds are for economic production, which is rarely practised in hobby workshops. Book values are useful for 'difficult' materials, because these cut within a much narrower range, if at all! For a hobbyist, the two most important things are to go in hard enough to cut because rubbing ruins tools in short order, but not so hard as to challenge the machine's rigidity, gears, or motor! Gorillas and weeds are equally bad machinists. Both are common beginner mistakes – I was a weed until Andrew Johnston put me right.
• Cutter coatings are extremely thin and unlikely to reduce sharpness. Coatings don't mix well with Aluminium, and cutters made specifically for non-ferrous metals are sharper than others because optimum sharpness depends on material. Using the right cutter just makes it easier to get a good finish and they last longer too; it's not that coated cutters fail miserably on Aluminium or uncoated cutters fail on steel.
• Don't use suds (oil and water emulsion) on aluminium or paraffin on steel! Why not is another essay question! I'll leave it to someone else!
• I like to set the RPM and adjust DOC and feed-rate to load the machine by ear. I only reduce RPM to stop chattering when reducing the other two risks rubbing. This depends on the motor: speed controlled electric motors tend to lose power and torque when their rpm is reduced. I find it pays to keep RPM high if possible.

Reading about how all these variables interact is intimidating. Don't worry because starting by rule of thumb and experimenting reveals what's needed and it soon becomes second nature. Theory is essential to making money in cut-throat production but absolutely not vital to producing results at home. The hobby is a mix of art and science and skill is more important than theory.

Practice!

Dave

Edited By SillyOldDuffer on 17/04/2021 11:02:32

[Anonymous]

A few more notes:

There's no fundamental reason not to use high flute count cutters on aluminium. The advice to use 2, or possibly 3, flute cutters arises from the fact that aluminium alloys are easy to machine and so feedrates can be much larger than those used for steel. So there is more swarf. Using fewer flutes helps prevent jamming of the swarf in the flutes. For instance the manufacturer of my cutters recommends, for a 6mm cutter, 3800rpm and 210mm/min in steel cutting full width and 0.5D deep. But for aluminium the recommendations are 7600rpm and 440mm/min, cutting full width but also 1D deep, so roughly four times the removal rate. Interestingly the feed per tooth is only slightly higher for aluminium. This is what happens when aluminium swarf clogs flutes:

No idea why SoD says don't use suds on aluminium. On the manual mill I machine aluminium dry, or with the odd squirt of WD40. The WD40 doesn't lubricate, or do much cooling, but it does help prevent swarf from gumming up the cutter. On the CNC mill I use suds flood coolant, mainly to wash away the swarf. Recutting swarf is a quick way to kill a cutter. I've never used paraffin on anything.

You don't need long flutes to cut deep pockets. It's unlikely you'll be doing a full depth pass, and if you do the cutter will deflect. A cutter with short flutes and large stickout will be stiffer than a cutter with long flutes and the same stickout. So less tool deflection. This pocket is 48mm deep and was machined with a 2.5mm stepdown and standard length flutes:

I start with selecting a width and depth of cut and then select an appropriate chipload. Then a spindle speed appropriate to the cutter and material, and that then allows the feedrate to be calculated. The critical parameter is chipload, in mm/tooth, rather than feedrate. It's counterintuitive but increasing chipload is often a cure for chatter. When I first started using my horizontal mill I was cautious. Result, the whole machine shook, which was impressive given it weighs 3500lbs. Double the feedrate, and hence chipload, and it cut perfectly with no chatter or vibration.

Andrew

[Stuart Munro 1Participant @stuartmunro1]

Andrew, hyper clarity! Your comments make sense to me so I must have taken something in from this blog.

I think you have identified two misunderstandings on my part.

1/ Your picture of swarf is a familiar sight. I had thought it was due to the aluminium alloy melting at the edge and sticking to the bit, so thought slowing the SFM/RPM and feed rate would help. But clearly reducing the swarf with say WD40 will also ease the problem.

2/ I had read that two flutes was the way to go with aluminium but did not align this knowledge with the speeds that large CNC milling go at. So for my speeds 4 flutes should be no harder to use than 2 flutes. My Sherline has a maximum RPM of 2800 so I'm never going to go too fast unless my bits diameter exceeds the capacity of the mill! Worth understanding but I'll probably stick with 2 flutes for price and to be able to use a 'slot drill' when needed.

As to the chatter issue, I know the theory about increasing feed rate or reducing SFM but it is challenging to a novice. I've only been machining during lockdown so have never had an experienced machinist work with me. I do believe that one session with someone telling me 'you can feed a bit faster' will give me the confidence but that may still be a few months off. Happily, there is a professional engineer with his own shop in the family who I'm sure will help when we can do so!

Regards

Stuart

[Tony Pratt 1Participant @tonypratt1]

Don't want to get in a 'pi****g' contest but I have done quite a few jobs in Aluminium where only a long series end mill will do the job to drawing requirements & of course you get more deflection the longer the cutter, that's where the skill comes into the equation.

Tony

Edited By Tony Pratt 1 on 17/04/2021 13:08:30

[Stuart Munro 1Participant @stuartmunro1]

Tony,

Sounds like your skill level is a different order to mine, as an accountant I could deflect numbers anyway you wish (but of course didn't) but deflecting a cutter sounds beyond me.

Stuart

[Author]

Posts