By continuing to use this site, you agree to our use of cookies. Find out more
Forum sponsored by:
Forum sponsored by Forum House Ad Zone

2mm Milling Cutter

All Topics | Latest Posts

Search for:  in Thread Title in  
Peter Bell18/12/2011 07:35:34
399 forum posts
167 photos

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
Jens Eirik Skogstad18/12/2011 08:18:01
avatar
400 forum posts
22 photos
 
 
Ramon Wilson18/12/2011 09:20:11
avatar
1655 forum posts
617 photos
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
Andrew Johnston18/12/2011 11:51:55
avatar
7061 forum posts
719 photos
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
John Stevenson18/12/2011 12:20:50
avatar
5068 forum posts
3 photos
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.
Ian P18/12/2011 20:05:14
avatar
2747 forum posts
123 photos
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
Peter Bell18/12/2011 21:20:25
399 forum posts
167 photos

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
John Stevenson18/12/2011 21:33:05
avatar
5068 forum posts
3 photos
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.
Peter Bell18/12/2011 21:40:09
399 forum posts
167 photos

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
Andrew Johnston22/12/2011 21:53:26
avatar
7061 forum posts
719 photos
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
John Stevenson23/12/2011 09:27:53
avatar
5068 forum posts
3 photos
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.
Andrew Johnston23/12/2011 09:39:01
avatar
7061 forum posts
719 photos
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
Peter Bell23/12/2011 12:51:04
399 forum posts
167 photos

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
 
 
Andrew Johnston28/12/2011 11:56:33
avatar
7061 forum posts
719 photos
Hi Peter,
 
Thanks for the information. The high speed spindle looks good; I'll have to put it on my wishlist.
 
Best Regards,
 
Andrew
harold16/04/2012 17:13:04
35 forum posts

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

Stub Mandrel16/04/2012 21:31:09
avatar
4318 forum posts
291 photos
1 articles

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

John Stevenson16/04/2012 22:09:41
avatar
5068 forum posts
3 photos
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 cheeky

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. blush

GoCreate17/04/2012 01:55:02
avatar
387 forum posts
119 photos

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

All Topics | Latest Posts

Please login to post a reply.

Magazine Locator

Want the latest issue of Model Engineer or Model Engineers' Workshop? Use our magazine locator links to find your nearest stockist!

Find Model Engineer & Model Engineers' Workshop

Sign up to our Newsletter

Sign up to our newsletter and get a free digital issue.

You can unsubscribe at anytime. View our privacy policy at www.mortons.co.uk/privacy

Latest Forum Posts
Support Our Partners
cowells
Sarik
MERIDIENNE EXHIBITIONS LTD
Shopping Partners
Subscription Offer

Latest "For Sale" Ads
Latest "Wanted" Ads
Get In Touch!

Do you want to contact the Model Engineer and Model Engineers' Workshop team?

You can contact us by phone, mail or email about the magazines including becoming a contributor, submitting reader's letters or making queries about articles. You can also get in touch about this website, advertising or other general issues.

Click THIS LINK for full contact details.

For subscription issues please see THIS LINK.

Digital Back Issues

Social Media online

'Like' us on Facebook
Follow us on Facebook

Follow us on Twitter
 Twitter Logo

Pin us on Pinterest

 

Donate

donate