using milling cutters

I am really having difficulty understanding the milling operation using end mill cutters & would really appreciate some guidance in simple terms please.

I want to make a couple of clamps as detailed in Harold Hall's website. So the first thing to make are the parts to go in the T slots. So using some old 25 mm square mild steel, I had my first go at machining these with a 2 flute HSS end mill.

It took ages to make a simple rebate on one side & although i tried various RPMs & feed rates & depths of cuts I still felt that I was missing something. You tube does not actually show someone machining something like this in detail. Looking at various tables i get some weird findings. When I run at slow speeds the result is a lot of what I would describe a "knocking" as though it is too slow but tables suggest only 450-650 RPM & I wonder if I am taking enough off too little or too much. I am just hand feeding on the table which is quite slow.

So working on a half inch HSS 2 flute cutter on mild steel in a Warco WM 16 mill may I ask:- (Rather than " how long is a piece of string?"I really need definitive values to start with rather than formulae)

1 ) what RPM would one suggest?

2) How much depth & how much side cut in each pass to form the 12mm * 10mm rebate. in a piece 25mm long ie alternatively how many passes should that take to complete it - should I cut the full 10mm each time & go a certain depth until I get to 12 mm or should i go say 1mm * 1.2 mm each time taking some side & some depth in each cut?

3) As to feed speed how long should it take for the cutter to engage on the end of each cut until it comes off the other end of the 25mm cut?

Are there any links where one can actually see this process being done at the speed one might expect so i can get an idea of what I should be doing that anyone is aware of

Any help gratefully appreciated

Edited By Sam Longley 1 on 23/09/2016 16:22:07

A four flute cutter would help. If you have a sturdy mill, it should be fine.

Hi Sam,

I think the problem you have is probably using a two flute cutter rather than a 4 flute. With a two flute end mill/slot drill you might need to increase the RPM and reduce the feed rate.

I would keep to the high end of the figures you have quoted, do not attempt to climb mill otherwise you could get a grab and end up ruining the work. I would take small depths of cut, say about 1/16", keep the feed steady and around about 4" per minute and limit the step over between cuts to around 1/3d the diameter of the cutter. This is very conservative in terms of feeds and speeds but it should provide you with a starting point without causing too much vibration. .

Get used to it taking a long time, it does, single point lathe tools remove metal continuously whereas milling cutters don't so it will naturally take longer than you would expect.

If you can lay your hands on a 3 or 4 flute cutter give that a try and you will find that it will cut much more smoothly. Don't be tempted to take too big a bite using the flutes as a cutting edge as the cutter will start to chatter and leave an undesirable pattern on the work, especially if the speed is too high.

There are lots of variables and it takes a while to find out what suits your machine, most importantly make sure that the machine gibs are adjusted to take up any play on the x & Y axis particularly.

I'm sure other people will chip in with more tips.

Bob

Hi Sam,

The speed (RPM) for a 12mm dia. end-mill will depend on several factors, one being how hard your steel is. You could try around 350 RPM, if using no coolant. With coolant you can of course go faster, as you can with a free-cutting steel. If 350 RPM works try to go a bit faster, to high a speed will blunt your cutter. A two flute cutter (slot drill) is used to cut slots for keyways, as Bob says, use a 3 or 4 flute cutter.

Thor

Hopefully I won't be criticised for grandmothers and sucking eggs, but;

You could always remove the worst of it with a hacksaw.

Using some low-tech to do the worst of it, will save on the expense of a high-tech cutter. Plus, of course, when you convert all of your material to shavings, the bits you don't need can't be used for something else in future.

With a WM18 at 420rpm with a 12mm 2-flute HSS I just cut a 2mm deep slot across a 25mm mild steel bar in about 20 seconds. It vibrates but not scary badly.

The 2mm deep cut was based on a rule of thumb for HSS suggesting a max depth of cut of no more than 20% of the end-mill's diameter. Another rule of thumb for HSS is rpm = 6000 divided by tool diameter. I can't remember where I got these 'rules' from but they seem about right. Interested to know if they're wrong!

A 0.5mm deep slot across 25mm took me about 10 seconds with very little vibration.

No coolant used.

Cutting rates vary a lot with how hard the metal is and the sharpness of the tool. After a bit you get a feel for what's what's reasonable.

If you're having a lot of trouble I'd suspect a blunt end-mill or a bad lump of metal. If it was Black Mild Steel, the scale can blunt HSS quite quickly.

Cheers,

Dave

It was a brand new cutter

Thanks that gives me something more definite to measure against. i will try that. & see what happens .

'Knocking' might mean that you are trying to 'climb mill' or the table gibs are not well adjusted, or both.

Ideally feed the work against the rotation of the cutter, this avoids the situation of the work being pulled into the cutter as the cutter tries to 'climb' over it in a series of jerks.

Secondly, make sure that the gibs (metal strips that adjust the clearance of the table) are adjusted to get rid of any shake, without being so tight it is hard to move the table. naturally you lubricate the gibs and dovetails of the table with some oil. This is a very condensed description!

Neil

Hi Sam,

As said in the first post, you need to use a 4 flute cutter, (End mill) 2mm deep cuts 6mm wide (1/2 cutter diameter) dependinng on the rigidity of your milling machine. An excessive vibration- reduce the cut. Do not climb mill unless you have a very rigid, substantial milling machine

2 flute cutters are for machining slots with material on both sides of the cutter

Cheers

Viceman

I've never had any issues end-milling with a 2-flute cutter, you just need to halve the feedrate to keep the same tooth load,

Neil

As above a 4 flute cutter is more suited to the job. (but see next post)

There are a couple of option sfor cutting, either do the full width and say 2mm depth each pass or to use more of teh side of the cutter and cut the full depth moving say 2mm sideways per pass.

Speed try about 600rpm and see what it sounds like, feed start with say one turn of the handwheel per second which on an imperial machine would be 6" per min or 120mm per min if a metric machine with 2mm pitch screw again adjust if it sounds liek it is needed, slower is not always teh way to stop chatter.

As an example this is a 4 flute 12mm dia cutter taking a 2.5mm deep cut, full 12mm width in steel, just a dab of soluable oil applied with a brush.

Or 16mm cutter, 6mm wide cut, 2.0mm deep in steel

Now using more of the side, 19mm high, 0.6mm wide per pass, same 16mm cutter

And another using the side, this time in iron with a 10mm rougher, 7.5mm height of cut, 3mm deep per pass

All on an X3 which is about teh same size as yours

Edited By JasonB on 23/09/2016 20:27:15

Edited By JasonB on 23/09/2016 20:33:55

The traditional 2-flute slot drill is usually best kept for slots that need to be to cutter width or the odd bit of drilling. However modern two flute cutters can have their own specific uses particularly where high removal rates of swarf are required such as when machining aluminium and combined with a high helix angle can happily be used on the side of the work.

As an example 35mm high cut, 0.5mm width

Hi Sam,

I completely understand what you mean about some of the advice and instructions. It's either vague, or assumes you know what is normal. I'm just setting up a Sieg X2P and getting used to milling: I've been happy with a lathe for some time, but milling is different and requires a firmer hand I am learning. The 'slow and light will always work and is safe, even if it takes longer' approach on a lathe, does not apply so much to a mill. Bold is beautiful within reason!

It's also worth noting that there are two types ( at least ) of model engineers. Some like to do things the 'correct way' with the perfect tool (whatever the expense) and will tell you that you should really have 'done it with a 61 degree, rather than your standard 60 degree......' The other we'll tell you how they built a replica Bentley using a pen knife and a spinning top for a lathe. Both are exaggerations, but you will recognise what I mean, and it can be hard to tell which direction the advice is coming from.

If you are making T nuts, then any cutter will do the job fine- four flutes is only better than two if you have got both! Find the right speed etc to fit what you have and it will work, and there is great advice above to do that.

But you say knocking: that's not vibrating or shaking or drumming, it's knocking.

A steady thumping vibration is normal, as the cutter edge starts a new pass: too much means too much work is happening and it's uncomfortable. You can hear this thumping in the excellent videos above, and it's fine ( even if you would be very unhappy with this on a lathe). Climb milling is also a thump, but one that sounds a bit aggressive -perhaps more of a punch than a thump- I don't do it the moment, so I've yet to experience the sound of it going bad!

Knocking is a harder metal on metal sound, suggesting part of the machinery or the part you are cutting is moving. Could be the part is not held firmly, so it's is bashing against the vice, or the table. Could be the gibs are loose and the head is knocking the column, or the table moving against the bed. Knocking is nearly always a bad thing, so go round and check all the above as it will only get worse. Gibs are set differently on a mill, tighter to start with, and locked up hard on any slide that isn't required to move when actually doing something ( actually, it's not bad practice on a lathe, but few do it).

So if it's knocking- probably not a cutting feed/speed/flute problem, but a set up issue with the mill.

FS Wizard (well worth downloading free app for iPad/iPhone [Android?]) says for hot rolled steel, 2 flute 12.7 mm dia cutter, max DOC (depth) 23 mm; max WOC 3.8 mm; 1093 rpm feed rate 4.33 ipm (not sure why it gives this in inches!). This will assume coolant. I'd still run the spindle at this speed, it reduces the tooth load for a given feed rate, but reduce the DOC. There is a reason why cutters have teeth on the sides, as you pay for them you may as well use them.

Jason

Thank you for the video which gives a clearer indication of the feed speed & amount of cut. Both are far higher than I have tried. The cutting action is also much quieter with much less vibration. I suspect some of that is down to the 4 flutes. If I made the gibs much tighter the handwheels would be quite difficult to turn.

I do have some 3 flute cutters which I will try tomorrow but I expect that these are low grade chinese so do not expect much.

It may be that a small investment in some better quality tooling might help

You've most probably done all this already Sam, but just in case:

• Lock the two slides that don't need to move before cutting
• Make sure the tapers are clean
• Insert the end-mill into the collet after putting the collet in the chuck, not before.
• The end-mill must be more than hand tight in the collet
• Nip up the drawbar sufficient for the collet chuck to grip the spindle taper firmly
• Move the Mill-Head close to the work rather than extend the quill

Dave

You say you have seen Harold Hall's website. It really would be worth buying his excellent book "Milling: A Complete Course". It is one of the Workshop Practice series so costs about 7 quid delivered to your door. It will take you step by step through all this sort of stuff you need to know in order to make best use of your milling machine.

Unfortunately I see that is No 35 in the series & I had purchased No 49 which is not much help