How big is too big?

[Nick WelburnParticipant @nickwelburn]

I’ve been using a Sieg mini mill. I’ve used perhaps an 8mm mill maximum.
I’ve just acquired an Emco Cnc machine and a vast array of end mills.
Emgee and Mike Tull have been giving great support in getting me up and running 🙂

How do you know when the cutter is too big?

[Nick Welburn]

On 27 June 2024 at 21:55 Nick Welburn Said:

How do you know when the cutter is too big?

When the belt slips, the motor stalls or the cutter chatters. Although all of these can be cured by reducing the depth/width of cut.

Also:- When the chips are blue even at the lowest spindle speed.

Lastly:- When the cutter won’t fit into any of the available tool holders.

Might seem light hearted (‘cos they are) but these are genuinely the correct answers.

[Paul LousickParticipant @paullousick59116]

Check your mill specification for maximum recommended cutter size.

A Sieg X2D for example states 16mm end mill and 30mm face milling capacity.

But this depends on type of material and feeds and speeds.

[BazyleParticipant @bazyle]

Also calculate the speed of the tip of the cutter. Most small mills can’t go slow enough for larger cutters.

[JasonBModerator @jasonb]

What is the max spindle speed of the machine.

You want to keep the motor running where it will deliver the most power and on any variable speed machine that will be at its max speed. So you don’t want to put in a cutter that requires a significant drop in spindle speed to avoild running it too fast for the material/cutter combination.

I tend to use 6mm or smaller carbide cutters on my KX3 and run them at the max 5000rpm, only going larger if say I want a full depth finishing cut and the flutes are not long enough on a 6mm or to surface the top of stock.

The amount removed known as the “Metal Removal Rate” will also come into it as you could happily use a 25-40mm dia insert cutter for facing the top of work provided you did not take too much off vertically per pass.

Another factor that you will have to consider is the radius of any internal corners, these will often govern the dia of cutter you can use and should typically be a bit less than twice any radius. So for example use a minimum 3.5mm internal corner radius for a 6mm cutter to avoid a large percentage cutter engagement in any corners what can lead to chatter and poor finish. A half decent CAM package will have a tool library will minimum cutting radii for any given cutter use that as a guide. I now think about this at the design stage and try to avoid having to go at it with two cutters – one to rough out and then a smaller one to get into the corners but sometimes it is the best option.

Tool holders were mentioned above and these can also have an effect but not just on what the max you can actually fit. You will be generating a lot of swarf particularly with aluminium and that needs to be kept out the way and preferably some lubrication added. If you have say a 6mm cutter in an ER32 collet holeder then that will get in the way. You want something more like an ER16 or even a sidelock holder so you can get in with air to clear the swarf so what that size holder can accommodate will be another limiting factor

I’m not sure about small mills not going slow enough for large dia cutters, I run a 50mm dia insert facemill at 2000rpm with little problem in all materials, larger on non ferrous. I have only found Hss Slitting saws to be a problem so running faster than the traditional calculated speeds is needed.

[JasonBModerator @jasonb]

here is a vid I uploaded a couple of days ago, all done* with a 6mm except some deeper cuts around the 6min mark where I used a 10mm dia cutter as I needed 20mm flute length for a full height pass. Plenty of room for the fog buster to get in with the smaller collet holder. If you look at some of my other CNC machining videos you will see most are 6mm or smaller cutters, I’ll often list the speeds and feeds either as captions or in the description.

* drills excepted

 

[derek hall 1Participant @derekhall1]

Once again a great video Jason,

Amazing what can be done with CNC. How long did it take you to machine that component?

I wonder how long it would take if done manually?

A quick question was that a mist coolant nozzle you were using or just compressed air? If it was coolent what were you using? I think I was told many years ago that paraffin was a good coolent for aluminium – not sure if mixed up with compressed air would be good for your health though !

Best wishes

Derek

[JasonBModerator @jasonb]

Thanks Derek, Breaking it down F360 tells me

The feet took 4mins

Each cylinder mounting flange face, bore & drill 34mins

The 5 slots in the front face 10mins

So total of 82mins. Add a couple of tool changes and rotating the R/T plus a slight loss as I use the free version so don’t get rapids although there were not that many and I suppose you are at about 1 1/2hrs.

It is a fog buster (non mist) system where a small amount of lubricant is pumped into the air flow. I did not use it on the slots at the end and also got a couple of air bubbles in the line so you do see my using a brush a couple of times. As the liquid is not atomized like it would be on a mist system you don’t get a mist in the air which would be bad for you. If you watch it on Youtube at full screen it’s easy to see the drops form on the end of the nozzle and then get splatted onto the work. Just enough to lubricate the tool and stop ali sticking, it would need a lot more too cool things. Yes it is Paraffin.

On the cutter size front, this is the draw next to my CNC, just one 8mm and one 10mm in there the rest are 6mm or smaller. Do have 25mm and 50mm insert cutters in another draw or larger in the other workshop.

[Mark Rand]

On Mark Rand Said:

On 27 June 2024 at 21:55 Nick Welburn Said:

How do you know when the cutter is too big?

When the belt slips, the motor stalls or the cutter chatters. Although all of these can be cured by reducing the depth/width of cut.

Also:- When the chips are blue even at the lowest spindle speed.

Lastly:- When the cutter won’t fit into any of the available tool holders.

Might seem light hearted (‘cos they are) but these are genuinely the correct answers.

Good post. I agree with all of your points. 🙂

[Vic]

On Vic Said:

On Mark Rand Said:

On 27 June 2024 at 21:55 Nick Welburn Said:

How do you know when the cutter is too big?

When the belt slips, the motor stalls or the cutter chatters. Although all of these can be cured by reducing the depth/width of cut.

Also:- When the chips are blue even at the lowest spindle speed.

Lastly:- When the cutter won’t fit into any of the available tool holders.

Might seem light hearted (‘cos they are) but these are genuinely the correct answers.

Good post. I agree with all of your points. 🙂

How I do it too – on a manual mill!  Mine is a WM18 with a 1100W DC motor and 2-speed gearbox.   Although the DC motor maintains torque reasonably well at reduced RPM, it pays to follow Jason’s advice and run the motor fast with a small diameter cutter rather than slow with a large diameter cutter.  Mostly, not always!

But Derek’s question relates to a CNC machine.   Don’t have one myself so could be talking rubbish, but I see CNC as being set up more scientifically than the touchy feely methods that work well on a manual machine.

A stall means the machine is way off, either speed, depth-of-cut, and/or feed-rate.    Reasonable for a quick thinking operator to correct these on a manual machine by feel, but a CNC machine shouldn’t be run experimentally to find the stall point.  A stall only happens if the operator missed an important step in the ‘Numerical Control’ part of CNC.  Someone guessed rather than doing a proper job!

Ideally, a CNC machine is told exactly what to do in advance, working to pre-calculated parameters, that ‘just work’.  The material, cutting operation, removal rate, and other factors are balanced against the machine’s power, torque, and rigidity.  Could be derived experimentally – might even be essential – but in general,  planning is far more likely to pay off.   Getting the control program right allows the machine to accurately cut complex shapes in 3 or more axes, without stoppages.

I suspect the seat of the pants methods I happily use on my manual machines would be time-wasters in a CNC shop.   My feeling is getting the best out of CNC requires different skills, including a better understanding of the power/torque/rigidity relationship.

What do CNC operators think?  Do manual skills transfer directly to CNC, or does CNC require additional planning?

Dave

[JasonBModerator @jasonb]

It certainly helps to have used a manual machine first as it should have given you a basic understanding but having a CNC certainly needs a bit more thought and you will think a lot more about depths of cut and feed rates as you start to use one. You are also likely to have much higher spindle speeds available and the ability to move the table far faster than you could wind a handwheel so best to use them rather than apply your manual thinking. This also applies to the type of cut and what parts of the cutter to use.

This is another good reason for not having a vast range of cutter sizes as you will get to know what works on your particular machine for a given material and type of cut. I tend to know now what works and have those parameters set in the tool library so I can just select the tool for the job and it has my basic known settings there and ready to go or be slightly tweaked depending on the job. The machine could certainly take more aggressive cuts but I’m happy to use the ones I do as a good all round balance of machining time against tool wear, swarf clearance and not putting too much load on the machine.

Most controls have an over ride on the machine so if in doubt to can drop say the feed rate by x % and then if things start off OK then you can click back up to what you originally thought, or even go above that if you think it can take that. Probably a safer approach to start with than picking the supplied rates and then frantically trying to reduce the feed once the cutter starts to friction weld itself into your aluminium part. There is really no feel with a CNC though sound and chip colour can be an indicator so you can’t just ease off on the handwheel even if you did have one.

I’ll also add that of my draw full of cutters there are no screwed shanks to be seen anywhere, nor are any imperial. There is a single HSS one in there that I think got used once when I did not have the size in carbide.

[JasonBModerator @jasonb]

one other factor that comes into play with size of cutter particularly if you are going to make use of carbide is cost.

If your machine is only capable of say taking an adaptive cut of 6mm high by 0.6mm sideways then unless there is a specific need why use a larger cutter as you are going to wear the end 6mm of flute of a 12mm dia just as fast as you wear those of a 6mm cutter but it is a lot cheaper to replace a 6mm one than it is a 12mm one.

Same applies for those early tool crashes, you won’t cry for as long after breaking a 6mm dia as you would a 12mm. Also the 6mm is more likely to break which could save further damage to the machine if something else has to fail when a solid cutter is driven into an even more solid block of metal.

[SillyOldDuffer]

On SillyOldDuffer Said:

Do manual skills transfer directly to CNC, or does CNC require additional planning?

I don’t think skills really transfer. All cutting parameters have to be specified in advance for a CNC mill. That requires a good knowledge of the cutting process and parameters including cutting speed, depth of cut, width of cut and chip load. Judging by questions on here these are sometimes poorly understood. As SoD says it also requires a good knowledge of the characteristics of the mill spindle in terms of torque and power. Another difference is that climb milling is very common on CNC mills, and is often preferred.

Using a CNC mill is not just about the cutter and cutting parameters. The sequence of operations, reference datums, clamping and toolpath type also need to be considered.

Early on when using my CNC mill I learnt that it is better to use smaller cutters running at high speeds and feedrates rather than large cutters running more slowly. The toolpaths and parameters can also have a significant effect, sometimes in ways that are unexpected. I always run my G-code through an independent simulator before running on the CNC mill. There have been times when the G-code did not do what the CAM program simulator said it would.

Most of my basic CNC milling is done with 6mm and 10mm, centre cutting, three flute carbide cutters. Other sizes and shapes are used as needed, but when designing I try and minimise the  tools required.

Andrew

 

[Author]

Posts