Aluminium cutting

[AGTM]

Hi Bush Flyer

I am new here, but I went through the posts. Would you please tell me why you are using a single flute cutter for aluminium?
I have been working aluminium for years, but mostly with 3 flute cutters. You can plunge, slot and side milling with no problems.
Depends of the tool I am running the cutters around 8000 - 10000rpm.
For me is interesting why single flute, why not 2 or 3 flutes?

[JAZZCNC]

For me is interesting why single flute, why not 2 or 3 flutes?

Because of machine stiffness and feedrates at DIY level. With 3 flute you need much higher feed rates at lower DOC and most DIY machines can't cut at those feeds and are not strong enough or have powerful enough spindle to cut at correct DOC for 3 flute cutters.

I agree thou they are better than single flute and give nicer finish if you can use them.

[AGTM]

Hi JazzCNC,

Thanks for the fast reply. Now I understand the situation. OK, here is what I would do if I have to use a single flute cutter for aluminium:
My rule specially for aluminium is Fz=D/100 or for example if you have 6mm diameter cutter your feed rate will be Fz=0.06mm/rev. And if you have available 10000 rpm, your feed rate will be F=600mm/min. I would not go more than DOC=1D
and WOC=1D.
Always helical plunging if it is possible as F=1/2 for the plunging. The single flute should go straight plunge (drilling) with no problems. Finally, It really depends of the carbide grade of the cutter. It might not be suitable for high speeds. Recently, I did a custom order for 3 flute uncoated cutters for aluminium. I made 12mm cutter with 45deg spiral. The tool has 24mm working length and 80mm total length. The carbide material of this cutter is WC25, a grade for stainless steel processing. This cutter works since four weeks, it is still in use and it works with S=10000rpm and F=3800mm/min.
So, if the single flute cutter brakes on the recommended cutting conditions, I am sure we can fix this problem with custom made tool. The good part is that the price is the same as the standard one, but there is a requirement for min 5 cutters.
I have one of those 12mm cutters left. If you want I will send you to try it or to some friend of you.

[JAZZCNC]

Hi AGTM,

Problem most DIY users here wanting to cut Aluminium is spindle power or lack of it.! Most are using router based machines and spindles with high speeds but little torque with typical 2.2Kw.
So DOC=1xd on 6mm cutter with WOC=1xd is mostly impossible with the spindle torque they have available.! Then you have the stiffness of the machine. Again being router based most are flimsy in comparison to even the weakest milling machine so chatter and poor finish dictate using much lower feeds/DOC etc.

I may give your cutters a try but I mostly use smaller 4-8mm cutters. Again due to spindle power but also material saving when nesting parts.
I'm a big believer that when it comes to tooling cheaper cutters are uneconomical as they wear quickly and put more stress on the machine not to mention much poorer finish quality.

Also I feel most people use the wrong tool for the Job, like not using a ripper for roughing.? Often this is down to the fact they don't want to change tools so will use one tool to do the whole job. This again is False economy because with a cerated edge ripper you can cut far deeper and remove far more material in fraction of the time without wearing the tool away or stressing the machine/spindle.
Also they don't actually save time by not changing tools it actually costs them time and money because the smaller tool cutting at lower DOC takes much longer than any tool change. Plus the tool and machine are getting hammered because they are working much harder than they need to.
On top of this Finish quality is lowered because by the time they get to the end of the job the tool cutting edge is so worn finish is poor. They don't realise that by using rippers and then just doing a finish pass they actually save money because time is reduced and tools last much longer as they are cutting efficiently and they get a much better end result.!

That's my take on it. . .

[AGTM]

Hi JAZZCNC,

I agree completely with you about the written above. You mentioned that you use 4-8mm cutters. I want to send you one Speed Tiger AUE to give it a try. Let me know what diameter would you prefer. You can go on the contact us page in my web site and give me your address.
Next week I will start a new thread named "Solid Carbide Cutting Tools - what we know and what we do not know about them"
There will be a few posts as I will start write first about the carbide grade of the tool.

Otherwise it is Friday here, a time for barbeque and beer.

I'll see you next week here.
Have a great weekend. Cheers.

[JAZZCNC]

Otherwise it is Friday here, a time for barbeque and beer.

That's just cruel as it's pee-ing it down here.!!! . . . . But that's ok as it's offset with plenty of the finest Ale in the world. .

[Boyan Silyavski]

I find that Fz=D/100 usually too much. Especially about aluminum. Not talking about roughing bits. Tools 0-2mm is one thing, 3mm is another thing, 4-6 mm another, and so on.

I have Gwizard trial installed but some how this program doesn't engage me, may be the price and subscription put me off.
Just found the free online FSWizard and actually the data it gives is quite near the manufacturer data and very very near at my actual cutting data. So i am quite convinced and maybe even will buy the payed version

The bits i use are mainly Kyocera, razor sharp and polished. Now looking at their data below, some conclusions about how things develop with sizing and type of operation can be drawn. This is quite more realistic than others i have seen.





Vc - cutting speed
f - chip load or feed per tooth
Fr- feed rate mm/min
D- diameter of carbide bit
U- nimber of teeth on cutter
p=3.14


Ae - side removal
Ap - face removal


1.
determine spindle speed rpm/min depending an operation/roughing, slotting, finishing/


RPM=(Vc*1000)/(p*D)


2.


Calculate feed rate mm/min:


Fr=f*U*RPM

[AGTM]

Hi JAZZCNC,

Your samples are on a way already. You should have them in a 4-9 days.

Cheers