Milling feed/speed question.

[Robin GrahamParticipant @robingraham42208]

[Robin GrahamParticipant @robingraham42208]

I don't like milling, perhaps because I have only a small bench machine (Warco WM14 – about 65kg, roughly equivalent to the Seig SX2) and normally take tiny bites (say ten thou) so things take ages. But in a fit of reckless enthusiasm tonight I did this in one swipe:

The material is CZ121 brass, I pushed in a 10mm 4-flute HSS endmill in sideways to make a 5mm radius, then 'conventionally' milled to the other end.

It worked, nothing broke, but the finish is pretty awful. I'm wondering if that's because I'm working this little machine too hard or I got speed/feed wrong. I was going at about 1200rpm and feeding (at a guesstimate) about 0.7mm per second.

Do I need to buy a bigger mill to do this sort of thing? Please say yes!

Robin

Edited By Robin Graham on 10/01/2019 01:21:16

[Thor 🇳🇴Participant @thor]

Hi Robin,

I have a Sieg X2 and usually take a light finishing cut to get a good finish, and use a higher speed for the finishing cut. For a light finishing cut in free-cutting brass you could probably use 1500 may be 200rpm. There is a speeds calculator here, and see here for feeds.

Thor

[JasonBModerator @jasonb]

Yes a finishing cut would be worth doing, you will have been getting some deflection and vibration taking the deep cut on a light machine which can be seen better at the ends. So take the first cut say 0.25mm short than go back an take a final cut.

[Anonymous]

Classic chatter problem. The feedrate is way too slow; 0.7mm/s is 42mm/min you need to be nearer 150mm/min or more. I'd advocate a finish pass too; climb milling for best finish but that may not be advisable on a small mill. Another issue for the finish pass is that in the corners you're going from a low tool engagement angle to the corner wrapping around a large arc of the tool. That's a classic cause of chatter. On a CNC mill you get around it by using a smaller diameter cutter. Not much one can do about it on a manual mill other than make sure the tool is sharp and everything is as rigid as it can be – short overhangs and unused axes locked etc.

Andrew

[Thor 🇳🇴Participant @thor]

Sorry Robin,

I made a typo in my previous post, should of course read: "….you could probably use 1500 may be 2000rpm."

Thor

[John HaineParticipant @johnhaine32865]

If you normally takes tiny bites and use slow feed then the tool just rubs and gets blunt.

[Ron LadenParticipant @ronladen17547]

Well done Robin thats a bit braver than I have tried so far on my SX2P. I have come to accept that it is a small mill though not weak by any means. I generally take lighter cuts though and I have pushed it a bit more on a couple of occasions and it seemed ok, I always tend to go with a finishing cut.

If I could I would join you on upgrading to a larger mill, I would really like a Sieg SX3 that would do me nicely.

Ron

[John ReeseParticipant @johnreese12848]

Of course you should buy a larger mill. That is what you wanted to hear, isn't it.

[Martin ConnellyParticipant @martinconnelly55370]

I would suggest searching for JasonB's milling for beginners thread. Look at his videos and watch how fast he is turning the feed wheels and at the size of the chips coming off. Chip size is a good guide to correct feed rate. The rpm of the cutter should be similar to what is used for drilling. It is based on the diameter of the cutting tool and the material being cut. You can be too timid as well as too aggressive when cutting like this but the acceptable range is quite wide. Even with CNC where the numbers are programmed in the operator will often increase or decrease feed rates manually during a cutting operation based on how everything is going (all material varies from one batch to the next and even in the same piece sometimes).

Martin C

[John ReeseParticipant @johnreese12848]

The chatter in the radii is a result of too much tool contact. I would plunge the tool vertically into the work to form the radii. End cutting is likely to produce far less chatter than feeding the side of the cutter into the work. After plunging the ends I would conventionally mill out the material between them. Leave a few thou for a finish pass. When doing the finish pass you want to stop a couple thou short of the radius cuts you plunged. If you get full cutter contact in the radius expect chatter.

[VicParticipant @vic]

Milling machines definitely seem to benefit from more mass so yes, get a bigger machine if you can afford/have space for one!

[JasonBModerator @jasonb]

I think the milling for beginners one may be a bit shallow and slow for brass so popped down to the workshop and had a play.

1/4" brass which looks about what Robin is using and similar speed. A couple of different 10mm cutters did not perform that well maybe because 1/2 diameter of a 4-flute cutter is not an ideal combination so popped in a used 3 flute FC-3 type cutter uncoated HSS.

The infeed is where the cutter is working hardest as the cut is widest so took it easier there and even dropped the speed down towards the end, then back up for the actual pass, probably feeding at 2.5-3.0mm per sec. Still a bit much for these light machines so would probably do it in two passes then a clean up.

Photo shows 0.2mm cleanup pass to the red line.

[Howard LewisParticipant @howardlewis46836]

A good basis for feed rates is "feed per tooth". For an End Mill, think in terms of 0.002"/tooth.

The machine speed is set on the basis of cutter diameter, material, and cutting speed.

From the machine speed and feed per tooth, the feed rate can be calculated.

If in doubt, feed slower rather than faster.

The depth of cut is usually set for an End Mill, on no more than a quarter of the cutter diameter.

And unless your machine has backlash compensation, do not climb mill. Always have the feed direction opposing the direction of rotation of the cutter.

H T H

Howard

[Robin GrahamParticipant @robingraham42208]

Wow, thanks for replies and especially to JasonB for taking the time to pop down to the workshop for a play and showing results. This has been really useful for me – I've not been using the machine to anywhere near its potential. It's actually happier with a a faster feed and higher spindle speed, less vibration and so better finish. Not sure I understand why, but it works.

Robin

[not done it yetParticipant @notdoneityet]

It likely works because you are operating at conditions closer to the recommended surface cutting speeds and feed rates. Simple as that? Recommended surface cutting speeds are for reasonable cutter life, so can be exceeded if shortened cutter life can be tolerated (we don’t normally do this) and lower speeds , within reason, may lead to longer cutter life. Feed rates are important for the same reason -bexcessive means overload and insufficient means excessive cutter wear – potentially not much more than zero cutter life!

[Robin GrahamParticipant @robingraham42208]

Yes, I totally get the thing about what's best for the cutter NDIY. The trouble for me as rank amateur is that I read stuff about optimal feeds/speeds for both lathe and mill work, but there always seems to be an underlying assumption that the rigidity of the machine isn't a problem. For example, I think that there is a rule of thumb that we can take off a cubic inch per minute per horsepower or something in steel. In my dreams! Another example is the calculator here: **LINK**

You don't get asked about the machine, just about power, DOC &c. so I assume the rigidity of the machine is a given – we don't have to worry about that.

What mystified me about upping speed and feed on my little mill was that the machine seemed happier – I didn't seem to have to wind so hard although I was taking metal off faster. Maybe subjective though.

Robin

[Ady1Participant @ady1]

I always found that "sideyways" milling was far easier than using the tip so used it whenever possible

The cuttlng/loading forces seem to be far more stable, even in a rubbish lathe milling scenario

[John HaineParticipant @johnhaine32865]

The late great Sir John often used to point out that you pay for those sharp edges on the flutes of a cutter, so you may as well use them! When I started I used to be far too gentle and found that milling with the side of the cutter using slow feed and small DOC sounded horrible and gave a terrible finish. Once I started to work the cutters harder everything got much easier.

[Anonymous]

Posted by Robin Graham on 13/01/2019 00:20:56:

Yes, I totally get the thing about what's best for the cutter NDIY. The trouble for me as rank amateur is that I read stuff about optimal feeds/speeds for both lathe and mill work, but there always seems to be an underlying assumption that the rigidity of the machine isn't a problem. For example, I think that there is a rule of thumb that we can take off a cubic inch per minute per horsepower or something in steel. In my dreams!

You don't get asked about the machine, just about power, DOC &c. so I assume the rigidity of the machine is a given – we don't have to worry about that.

It's a controversial view but I would expect a machine tool to be designed to cope with the cutting forces generated. Obviously a machine with 25hp would be heavier and more rigid than one with 1hp, but the same principles apply. It's also not just about the mass of metal, but having the metal in the right place.

All machine tools deflect so cutting parameters need to take that into account. It's not obvious but increasing feeds may well be beneficial. If the feed is small and the machine deflects a little, that deflection can be a significant part of the feed; equals chatter. With a higher feedrate the deflection is a smaller proportion so much less chance of chatter.

As well as the rigidity and power available it helps to have a basic understanding of the cutting process. Remember that neither the material nor cutter know whether they're on a small or large mill.

With smaller machines it's better to run small cutters fast rather than large cutters slow. On my CNC mill I run cutters much faster than on the Bridgeport, although both mills are the same horsepower. The rule of thumb of one cubic inch of steel per minute per horsepower works well for me. In theory the power needed per unit metal removal goes down as cutting speeds go up because the metal in the shear zone is hotter and hence softer.

That's enough pot stirring for now; time to go and fly the tug plane.

Andrew

[SillyOldDufferModerator @sillyoldduffer]

Posted by Robin Graham on 13/01/2019 00:20:56:

… The trouble for me as rank amateur is that I read stuff about optimal feeds/speeds for both lathe and mill work, but there always seems to be an underlying assumption that the rigidity of the machine isn't a problem. For example, I think that there is a rule of thumb that we can take off a cubic inch per minute per horsepower or something in steel. In my dreams! …

You don't get asked about the machine, just about power, DOC &c. so I assume the rigidity of the machine is a given – we don't have to worry about that.

What mystified me about upping speed and feed on my little mill was that the machine seemed happier – I didn't seem to have to wind so hard although I was taking metal off faster. Maybe subjective though.

Robin

 

Don't worry too much – being self-taught is learning the hard way! Not having a feel for the ability of your machine is likely to be a problem for newcomers.

I did exactly the same as you and was far too genteel in the workshop. Apart from excessive delicacy taking far too long to complete jobs, it also tends to blunt tools rapidly, further reducing confidence. Add to that the possibility that a beginner might practice on vile lumps of difficult to machine scrap, and you might well end up underestimating your machine – I did.

One consolation, assuming a lightly built hobby mill can cut like a Bridgeport is far worse. Heavy-handed beginners get inaccurate cuts and poor finish because the machine flexes. They also risk breaking something. Far from unknown for beginners to wear out brushes, fry their electronics, strip gears, or even burn out motors. One solution for heavy handed hobbyists is to buy an industrial machine, the other is to develop the extra skills needed to work with a lightweight.

On small machines there's a sweet-spot much less than the theoretically preferred cutting rate. It varies with the material, the cutter, lubrication, and the type of cut. Some people are naturals at finding it, others not. It's about sound and feel rather than theory.

The best way to learn is to watch an expert and ask him questions. Watching YouTube is helpful, and reading magazines/books/looking up tables will put you in the right ballpark. I've learned much from the forum – in particular Andrew's advice 'don't pussyfoot', plus hints from many others. However, I had to experiment because only experience can tell you what your particular machine will do. On my WM18 I've found: RPM should be set as close to the theoretical value as possible but the depth of cut and feed-rate both have to be reduced. There's a balance between depth of cut and feed-rate. In my case I was taking suitably deep cuts but had the feed-rate too low. I fixed most of my problems by increasing the DOC & feed-rate until the machine is heard to be working just short of sounding distressed, and when I can feel some resistance when pushing the cutter through metal. (Let the tool do the work rather than force it.) Basically you want the motor delivering no more than its rated power into cutting metal without applying enough force to bend the machine. Work the mill moderately hard but don't thrash it.

Dave

 

Edited By SillyOldDuffer on 13/01/2019 11:43:15

[JasonBModerator @jasonb]

The other factor to bear in mind with the 1inch/HP comment is that is was more than likely based on older machines that had a mechanical means of adjusting the speed be that belt or gear which meant that the motor was always at it's optimum speed.

The modern variable speed machine won't have the same grunt at lower speeds that it does at high speed yet the motor has not changed. I'm sure if Andrew had a big heavy casting in his lathe or was swinging a large dia boring head that wanted to turn at 50rpm he would be more likely to select 54rpm on his gearbox and run the motor at around 50hz rather than select 2000 rpm from the gearbox and have the motor just ticking over.

[Anonymous]

Posted by SillyOldDuffer on 13/01/2019 11:41:09:

I did exactly the same as you and was far too genteel in the workshop. Apart from excessive delicacy taking far too long to complete jobs, it also tends to blunt tools rapidly, further reducing confidence. Add to that the possibility that a beginner might practice on vile lumps of difficult to machine scrap, and you might well end up underestimating your machine – I did.

Been there, done all that!

When I first started with my lathe I bought some 2" steel bar from a tool shop in Cambridge. Had all sorts of issues with finish; smooth for an inch and then suddenly tearing, and then back to smooth. After much experimentation I got nowhere. Starting thinking about taking up knitting instead, even bought an embroidery kit! Then I talked to a professional machine shop who were making some boxes I'd designed. They said we don't buy from that company; their steel is carp. I bought some more steel from a professional stockholder and suddenly I was getting good, and consistent, finishes.

It also took me a while to work out that the way to stop chatter on the Bridgeport was to up the feedrate, sometimes quite considerably.

You live and learn; just wish I was a bit quicker on the uptake.

Andrew

[Anonymous]

Posted by JasonB on 13/01/2019 13:14:57:

The other factor to bear in mind with the 1inch/HP comment is that is was more than likely based on older machines that had a mechanical means of adjusting the speed be that belt or gear which meant that the motor was always at it's optimum speed.

A mechanical speed adjuster allows the motor runs at its design speed, aka base speed. It's the speed at which the rate applied voltage is just sufficient to drive enough current through the windings to give the rated power. It also means that constant power is delivered to the spindle across all speed ranges unlike a VFD.

My CNC mill has two belt ranges within which the speed is varied with a VFD. I know what spindle rpm corresponds to base speed on the motor and I try and stay above that so the motor is always running at constant power. It's one reason I moved to running small cutters at high rpm and feedrates compared to the Bridgeport.

Andrew

[Author]

Posts