2mm Milling Cutter

Advert

New Replies

Report Bug

Help/FAQs

2mm Milling Cutter

This topic has 19 replies, 10 voices, and was last updated 17 April 2012 at 01:55 by GoCreate.

Viewing 20 posts - 1 through 20 (of 20 total)

Author

Posts
18 December 2011 at 07:35 #15547
Peter Bell
Participant
@peterbell11509
Advert

18 December 2011 at 07:35 #80002
Peter Bell
Participant
@peterbell11509
Hello,

Trying to mill out some clock wheel blanks from 1/16″ brass with a Sieg KX3 but not really really having much success–my only cutter has seem better days!

I know its a bit subjective but has anyone any general reccomendations on speed and feeds or even the best style of cutter ie slot drill of end mill for the job? Or is the data somewhere?

Thanks Peter
18 December 2011 at 08:18 #80003
Jens Eirik Skogstad 1
Participant
@jenseirikskogstad1
Here is the link about feed per tooth: http://docs-europe.electrocomponents.com/webdocs/001b/0900766b8001b8d5.pdf

And the cutting speed: http://www.uddeholm.com/files/Cutting_Data_Corrax_eng.pdf
18 December 2011 at 09:20 #80005
Ramon Wilson
Participant
@ramonwilson3
Hi Peter, As a general rule – in brass – the rotational speed should be high, probably around your top speed for a HSS 2mm cutter but the feed kept low to prevent overloading it as after all it has a pretty thin cross section.

Also in brass (or bronze) the cutter should be as sharp as possible, preferably new and definitely not used on steel previously as the material will tend to be ‘pushed’ rather than be cut putting an even greater load on the cutter.

Personally I use the HSS FC3 throwaway cutters for these small diameters but that’s because of my background – I would hazard a guess that small carbide cutters may be more easily obtainable but the sharpness factor should still be borne in mind

Brass is normally cut dry but I have found that Tapmatic tapping fluid is absolutely brilliant for improving the cutting ability and the finish on brass. It creates rather an unpleasant smell if it gets hot though

Hope this will be of some help,

Regards – Ramon
18 December 2011 at 11:51 #80010
Anonymous
Hi Peter,

First, and foremost, buy a new cutter!

Second, I assume you need to plunge into the brass before starting the cut proper, so a slot drill, or centre-cutting end mill, will be best.

Third, speeds and feeds. Machinery’s Handbook gives machining speeds for brass with HSS tools of between 200 and 350 fpm, depending upon the exact material. Let’s be conservative and take the lower speed of 200 fpm. For a 2mm cutter that equates to 9702rpm. I looked up the Sieg KX3; maximum speed 5000 rpm. So that sets the cutter speed. A starting point for chip load in soft materials is 1% of the cutter diameter, so for a 2mm cutter that’s 0.02mm, or a bit under 1 thou, per edge. A chip load of 0.02mm by 5000 rpm is 100mm/min. If we assume that the cutter has two flutes that’s a feed rate of 200mm/min. We could be cautious and make the feedrate 150mm/min. So, to summarise, 5000rpm and 150mm/min for a 2 flute HSS cutter.

Fourth, I’ve always machined brass dry. I might use flood coolant on a CNC mill, but only to get rid of the swarf.

Best Regards,

Andrew
18 December 2011 at 12:20 #80011
John Stevenson 1
Participant
@johnstevenson1
Andrew has covered the basics of speeds and feeds but the following tip is something I have just discovered.

Not saying it’s new but i have never seen it and after posting on a couple of forums no one else has come back to say they have.

However it’s so simple it MUST have been ‘invented’ before.

Making some M5 HTD pulleys which require a 1/8″ ball nosed cutter the only ones readily available had 3/4″ ling length of flute.

These were cutting OK but at the expense of having to take three passes per tooth as not to brake the cutter but familiarity stepped in and I broke one.

So I then took a piece of 10mm steel rod, faced and centred both ends, drilled one end 1/4 to match the shank for the length of the shank.

Turned it round and drill the other end 1/8″ then split it lengthwise with a hacksaw.

The cutter was pushed in so that only 3/16″ protruded and held in a 10mm collet.

This made the cutter that stiff i was able to do all the other pulleys in one pass per tooth.

John S.
18 December 2011 at 20:05 #80037
Ian P
Participant
@ianp
Thats a nifty tip!

I have certainly not seen it before and I will definitely bear it in mind for small diameter cutters.

I can think of a variation to it that could be used if the prospect of keeping the two bores accurately concentric is a concern.

Basically drill a hole in a piece of brass rod the OD of which is slightly larger than the cutter shank and press it on the the cutter flutes. Grip the cutter shank in a collet (in the lathe or mill) and turn the OD to match the same diameter. In use the collet should grip both the steel and the brass sleeve.

If the hole is sized correctly the cutting edges should come to no harm but as in John’s method it will add a lot of support.

I should have said the brass rod has to be shorter than the flutes!

Ian Phillips
18 December 2011 at 21:20 #80042
Peter Bell
Participant
@peterbell11509
Hi Everyone,

Thanks for all the help, that the first time that I have really understood the basics of feed and speed and been able to apply them, those tables are good as well.

Not having a new cutter and now that I have learned a bit being unable to wait I have found a reasonable 2mm HSS slot drill and success!

I have now mounted my Arc Euro high speed spindle on the side of the head so can go up a bit with the speed (12000 rpm seems ok) a bit and the blanks come out really well with clean chips. I was going to try flooding with coolant but as the brass sheet is scewed to a piece of plywood pleased I didnt.

Thats a cracking idea with the cutter sleeve, all small cutters look very vunerable to me especially as they get near to metal

Going to treat myself to some new cutters, another lesson learned on the voyage into CNCing

Best Regards

Peter
18 December 2011 at 21:33 #80044
John Stevenson 1
Participant
@johnstevenson1
When milling it’s all about keeping the cutter cool and getting rid of chips.

Recutting left over chips is the main reason for bad finishes and undersize slots etc as the tool get deflected by the chips building up.

If flood coolant isn’t handy or possible then just a constant air blast helps in the same way, especially on smaller machines.

Sorry if I’m teaching anyone to suck eggs but all sorts read these forums.

John S.
18 December 2011 at 21:40 #80045
Peter Bell
Participant
@peterbell11509
Thanks for the advice John—got an air supply almost rigged up so could try that soon—got to be better than soggy plywood!

Peter
22 December 2011 at 21:53 #80284
Anonymous
Hi Peter,

Is your high speed spindle the ArcEuroTrade high speed motor and associated VFD setup? If so I’d be really interested in your experiences. I keep running out of top speed on my CNC mill, particularly so when engraving. I like the look of the ArcEuroTrade high speed spindles, but there’s nothing like practical experience!

Best Regards,

Andrew
23 December 2011 at 09:27 #80305
John Stevenson 1
Participant
@johnstevenson1
Peter,

This post may seem bias as I have one of the first high speed spindles that ARC brought in as a test exercise buy I do have a lot of experience with high speed spindles.

At my last job I was responsible for looking after upwards of a 100 Pershe spindles up to 7 HP. On the smaller 0.37Kw spindle some machines had p to 7 of these fitted.

The ones ARC sells were the third lot brought into the country, the first two lots were terrible and basically didn’t have inside them what the build up said. Saying they have ceramic or German bearings doesn’t mean that to some exporters.

Anyway these units work fine, in fact there is no different IMHO between the expensive Pershe and these.

They are rated at 24,000 rpm by virtue of being run at 400 HZ hence the VFD and will gladly drop to 12,000 with no problem.

I would not advise going lower as the fan speed drops and heat would be a problem.

They are high speed spindles and not designed to run at 3,000 or 5,000 rpm.

I usually run mine on engraving laminate at 12,000, noise isn’t a problem in fact they are quite quiet but even at high speed the cutting action of the tool on the material is far louder than the spindle.

I have had mine 3 years now and it’s gets regular use as it’s fitted to my router and is the only spindle I use now, the Kress has been sold on.

The two larger models were also sent out for testing with other high use users and again no problems reported.

John S.
23 December 2011 at 09:39 #80307
Anonymous
I can corroborate the low noise; I’ve had a normal ‘phone converstion with John while he was standing next to the high speed spindle running at, I think, 15000rpm.

Andrew
23 December 2011 at 12:51 #80316
Peter Bell
Participant
@peterbell11509
Hi All,

Yes my spindle is one of the ARC 0.75kw but with an e-bay 1.5kw VFD. I have only recently started using it after bolting it on the side of the KX3 so it’s early days yet but I am really pleased with it. The VFD seems to do all that is asked of it and at £85 delivered I thought it was worth a go, time will tell. I have fitted an external pot to control the speed and I intend mounting it on a board so that I can use it with other kit, ie my hydraulic log splitter which is a little slow on the return stroke.

It seems very quiet up to about 22,000 rpm when a bit of resonance prehaps from the fan (not vibration) comes in but at any speed above about 12,000 there is loads of air.

My only gripes at present are the table seems to run out of travel very quickly so you have to set up carefully and the coolant tray needs changing for something more useful/friendly

Regards Peter
28 December 2011 at 11:56 #80679
Anonymous
Hi Peter,

Thanks for the information. The high speed spindle looks good; I’ll have to put it on my wishlist.

Best Regards,

Andrew
16 April 2012 at 17:13 #89216
harold
Participant
@harold
I'm shamelessly bumping this thread because, speaking as a relative newb, it's the most useful I've found on the subject of cutting speeds. Jens' second link lists some very simple formulas which I've used to write a table to adorn the shed, while Andrew's post demonstrates the method.

Thanks, chaps.

John
16 April 2012 at 20:46 #89228
MICHAEL WILLIAMS
Participant
@michaelwilliams41215
Hi Peter ,

(1) For a normal clock wheel with spokes and many other similar components it is much easier and faster to do most of the profiling with a larger and robust cutter running at something like its correct speed and then use your smaller cutter just to do the detail areas like internal corners .

Even a 3 or 4 mm cutter is much more rigid than a 2 mm cutter .

Not usually any problem in setting two different cutters to cut to the same line and merge the cuts neatly . Doing this is a standard facility in all reasonable CNC software .

(2) There is a big difference in the way cutters perform in the two possible cases :

(a) Cutter cutting in passes and (all but the last pass) cutting is on side and end of cutter .

(b) Cutter right through the work and cutting in one go on side teeth only .

Wherever possible have the cutter right through the work and cutting on side teeth only . This can increase cutter life by a large amount compared with using side and end teeth together .

A technique well known in industry to prolong cutter life when profiling is to dither the cutter . There is more to it but basically you set the cutter at different heights relative to the work so as to keep presenting new cutting edges . To do this you need some room under the work – normal method is to use (eg) an aluminium plate and use the actual component profiling program to cut out a deep groove to give cutter clearance .

(3) If you have a very high speed spindle available and a reasonably rigid set up you don't actually need bought milling cutters . DIY HSS cutters ground like engraving cutters , taper or parallel , and with just one cutting edge work extremely well .

Regards ,

Michael Williams .
16 April 2012 at 21:31 #89229
Sub Mandrel
Participant
@submandrel
Just an observation in the light of some 'engraving' I did last week. The job was a fail because HDUSWELL is not spelt like that

But as I was using a 1.5mm cutter in 1/16" brass I think it was relevant. The cutter speed was about 1200 rpm i.e. top speed in low gear on my X2 – I forgot to to put it in high gear. Brand new FC3 cutter and feeding at about 60-90mmm per minute (based on the speed I was turning the handles at 1.5mmm per turn). Depth of cut 1/32". Very clean cut, chippy swarf no problems. Sadly I don't know the type of brass as it was an offcut – but I would say fully hard sheet, not compo (leaded).

Neil
16 April 2012 at 22:09 #89231
John Stevenson 1
Participant
@johnstevenson1
Posted by Stub Mandrel on 16/04/2012 21:31:09:

Just an observation in the light of some 'engraving' I did last week. The job was a fail because HDUSWELL is not spelt like that

Neil

HDUSWELL is spelt like that, it's the only way to spell it

John S.

P.S. Be grateful it was only one word and not one word in about 17 lines of text. Mind you i heard about this, didn't happen to me, no, no way.
17 April 2012 at 01:55 #89238
GoCreate
Participant
@gocreate
Hi

After breaking a couple of 1mm and 2mm slot drills on my cnc I now almost exclusively use carbide (pcb) engraving cutters on brass and gunmetal. Now I can do small milling with confidence and have never broken one of these, I am using 1mm wide cutter for most milling but down to 0.1mm or finishing and engraving.

One problem is, although my spindle max is 10,000 rpm, it's much happier at about 6000 rpm so not great.

Mind you these slot drills, although new ,were not great on sharpness, they were cheap but expensive to break.

Because the engraving cutter has tapered sides, sides need to be finished will the slot drill/endmill but for some jobs it does not matter.

I am using a small Sherline I converted to cnc.

These engraving cutters have one flat side like a 'D' bit, the 0.1mm cutter (very sharp) actually makes a good scriber point, the flat edge helps when scribing a line along a rulers edge.

Nigel
Author

Posts