View Full Version : Hmm - is it unrealistic to use feed/speed calculators on home built machines?

26-01-2016, 02:55 AM
Hi all. I was machining a bit of 6082 T6 over the weekend and I thought I'd try a new 5mm, 3-flute carbide roughing cutter. I've read a lot about how you shouldn't shy away from using more of the cutting area of the tool and how it actually prolongs tool life by working the tool etc. - I can understand why this ought to be true but somehow I can't see myself getting anywhere near these setting recommendations from FSWizard:


..so that works out at a feed of 16mm/sec for slotting. Here's a vid using the above parameters but feeding at 10mm/sec:



It was doing alright for a while, but shortly after I finished recording it got a bit melty when plunging into a small pocket... I reverted back to conservative settings that work for me - here's an example at 7mm/sec - DOC 1.5 - AIR & WD40 to cool:



Less than half the recommended speed - if you turn off the 'slot/pocket' option in FSW and use a 40% stepover, then the feed jumps to 30-odd mm/sec which just seems mental to me.

So a couple of general questions - are these quick speeds really intended for bigger (pro-level) machines running flood cooling etc (not just the odd squirt of WD40)? Secondly - what about the rule of thumb that you really don't want a depth of cut more than a third of the tool diameter - how true is that in the context of going deep and keeping the tool happy by giving it some work to do?

I like the idea that there's a formula for every eventuality, but much (if not all) of what I cut is by feel. is it unrealistic to expect to be able to use the numbers from tools such as FSW on home-built machines?


26-01-2016, 05:57 AM
So many variables with cuttter quality, material etc and Each machine is different so much of it is trial and error so I don't put much stall in FSW.
I find to get gauge of the tooling and machines capabilty's it's worth sacrificing a cutter or two and some material by running tests at different DOC and Feeds. Your ear and senses along with machine will soon tell you if not happy. Bit of trial error and you'll find the sweet spot for your machine.

Don't be afraid to use larger tooling either I find 8mm works best in ali. Can cut deeper and make bigger chip which lowers chance melting. Reason you got melting with 5mm was chip thinning because didn't cut deep enough. Thin chips heats up melts then sticks to cutter. Thicker chip doesn't melt so easy and heat leaves with chip. Problem with smaller tooling is it's fine line between cutting right and wrong resulting in much easier breakage or gumming. It's also more critical you clear chips but at same time harder to clear chips when cutting deep due to narrow slot so loads of air/lube is needed.

Clearing chips and Lube/Cooling make big difference and looking at your Video you didn't have enough Air/lube to run those higher feeds with narrow tool, could probably gone bit deeper has well for thicker chip.! . . . Keep playing and you'll find the limit.? . . . . It's often much more or deeper than you think.!!

26-01-2016, 01:29 PM
Rightly or wrongly I also cut by experience and feel. If I go past my trusted F&S or DOC I can usually hear the tool loading up and melting is often only a few seconds away. This can happen quite quickly if it goes around a corner or radius.

Pockets especially need a bit of thought - the first ramp into the new material is at full WOC, whereas once a small bit of the pocket has been cut and the current DOC value is reached then the WOC is generally 20-50% (50% is max in Vectric Cut 2D). This means that feeds and speeds are different for the getting started vs the rest of the clearance.

I can backoff F&S so that both situations are OK and you don't get melting, but then the whole job takes much longer. Or what I do is set the feed and speed for the general pocket clearance but manually override (using Mach3 slider bar) the initial ramp and first few passes of the cut to say 30-50% feedrate until it is into the pocket properly when I slide it back up to 100%. Maybe more advanced CAM software can give you options here but Vectric Cut2D does not.

I'm also stuck with 1.5kW spindle on ER11 (so 6.35mm max) which limits tool stiffness. I'm sure 8mm would be much better as Dean says.

When I cut slots (or outline profiles to cut something out) these are most likely to clog up when I'm about 8mm into the part, which is a problem when the part is 20mm thick. WD40 plus clearing the chips helps, along with a lower DOC than the first 8mm.

26-01-2016, 02:24 PM
You can go as fast as your machine allows if you use trochoidal milling:


26-01-2016, 02:30 PM
You can go as fast as your machine allows if you use trochoidal milling:

Nice, but don't be shy - surely you could increase the width of cut there by a fair margin?

Sent from my HTC One M9 using Tapatalk

26-01-2016, 04:13 PM
I like to use this calculator to calculate the Tangential cutting force, that is how hard the machine is pushing the bit sideways through the material. In my experience you can bet any speed/feed/DOC/WOC combination that exceeds a certain amount (you will have to find experimentally on your machine) will pretty much always cause chatter or be bad. The exception is smaller diameter longer cutters will always be worse than shorter fatter ones, but that might be less important on a machine that's not very rigid. Also obviously the smaller the diameter the cutter the more likely it is to snap completely, so watch your tangential cutting force very carefully.


One thing I have to mention, if you where hand coding you would have complete control over the feed rate. So you can make it slower for parts where the WOC increases (inside corners for example) and speed it up for the other parts.

I almost feel I should start a movement or protest or something. Maybe I'll make a website, banspeedsandfeeds.com. Speeds and feeds are an artifact left over from the days before CNC. They shouldn't be used in CNC software and someone should really do something about it.... lol

What we should be using is surface speed, that is how fast the tip of the cutting bit is traveling across the surface of the material per minute. Which is tool circumference(Pi*dia) times the spindle RPM, (Pi*dia)*RPM. This is the primary cause of heat and it's obvious why when you think about it. Rub any two things together even smooth things and you get friction, friction means heat, how much heat is directly proportional to how fast your moving them. The frictional coefficient of the material is the thing that effects this so that will dictate your spindle speed.

Then there is chip load per tooth, this is how big a bite each tooth takes. This is important to make as big as possible so your tool lasts as long as possible. Taking a small bite or a big bite makes no difference to the tooth it wears the same either way. So if you take fewer bigger bites your tool will last longer. However there is a limit of course, bigger bites take more power and more force. Power isn't usually the limiting factor, most people have way over powered spindles for what they are doing. Force can be an issue, a tiny little tooth will snap off more easily than a big one. The hardness of the material makes a big difference. You can generally find information from the tool manufacturer on chip load, then you need to do some maths. For example lets say they recommend 0.025mm chip load per tooth, you have a 3 flute cutter. With 3 flutes/teeth you need to travel your chipload distance * 3 every revolution so 0.075mm per revolution. Your surface speed calculation says you need 10,000rpm spindle speed. So your feedrate will be 0.075mm*10000rpm = 750mm/min.

WOC is important but only really in terms of power and force required for a wide cut is obviously more than a thin cut. Same for DOC. Where you get a problem is when you try to do both a wide and deep cut. Then your going to have problems clearing the chips. However it shouldn't really ever come up if you've done your surface speed and chip load calculation correctly because your machine won't have the rigidity and power for both a wide and deep cut. Not on home hobby machines anyway.

In any case you should try to take as deep a cut as possible so that you wear the tool evenly, it's no good buying a 50mm long endmill if you only ever use the first mm of it.

WOC 30% of the diameter is generally considered to be 'safe' from chip clearing problems. You can of course go wider without problems, especially if the cut isn't deep. But again if your really driving the tool as hard as is recommended(chipload) then it's unlikely your machine will have the balls for a wide cut. You might even have to go much smaller on the WOC.

26-01-2016, 04:48 PM
Excellent post Rufe0. Cheers!

26-01-2016, 06:37 PM
You can go as fast as your machine allows if you use trochoidal milling:

Well not exactly there is still limits.! I use I-machineing all the time which is kind of enhanced trochoidal milling and machine speed isn't the limiting factor it's machine strength.

Also you need to let that machine have it's head because that looks kind of slow for Trochoidal milling.!

26-01-2016, 09:58 PM
Agree with you Jazz, not my video though.Just the first one that came up as diy cnc trochoidal, will note that next time. Basicly wanted to show what can be done even with a light frame router.

When I rough i try to get 0.8 mm of axial offest from the total depth and about 0.5mm for finishing sides. 8mm 2-flute or 3 flute is my preferred choice with at least 3mm of step over going at 700mm/min only because i am limited to the rpm on the old KRV.

editing to add a photo of last weeks job

27-01-2016, 07:55 PM
I'll add to the chorus here. Since getting trochoidal/adaptive CAM in Fusion 360 I've all but but given up using slotting in aluminium, even when doing cut out paths.

Although i have yet to run some "tests" to see where the limits of my machine are I'm getting 5mm DoC from a 6mm 3 flute rougher at 2.4mm stepover in 6082 T651 ali and it doesn't seem to be any where near moaning about it. Whereas when slotting I've found that the "window of safety" is small enough that you only need something in the recipe to be inconsistent e.g. a gummy spot in the aluminium or something slightly off with the machine that day and what normally runs well with a good spray of chips the day before, becomes the howling chatter marked cut from hell.

There is of course operator error on my part as well, so a wider margin of error is always welcome :)

28-01-2016, 07:55 AM
Slotting is about the worst cut you can do, especially in Aluminum. The best cutters I use for that are 1 flutes 3mm, they are almost impossible to gum up, because there are so much space for the chip to go.

Using two or more flutes require the cutting flutes to be really wet in order to prevent gummy aluminum chips to stick to the bit. This is the case for my 6040 anyway.

To answer your question, I have found feed and speed calculator to work pretty well. I tried Gwizard, and the calculations put me right into the ballpark when I selected the second least aggressive cut. (You can select between aggressive roughing, roughing, finish or fine finish)

30-01-2016, 08:53 PM
https://www.youtube.com/watch?v=nFygwHfD5D8&list=PLaCDmykyjVw8cABQfqSll18S 65kkfNBN9&index=9

01-02-2016, 09:53 AM
https://www.youtube.com/watch?v=nFygwHfD5D8&list=PLaCDmykyjVw8cABQfqSll18S 65kkfNBN9&index=9

That video puts in mind something very interesting actually. Something that I had forgotten about.

The spindle power.

It seems that the zero divides FSwizard does not account for reduced spindle power. Was looking at doing some facemilling with a 50mm and he was giving me spindle power requirements of 16HP! My poor KRV only has 3 :uncomfortableness:

GWizard did have the power tweek but my subscription ran out and I am not quite ready to renew.