New milling motor Proxxon FBS 240/E upgrade to Kress 1050 FME-1

[Davek0974]

And I wouldn't worry about going for the smaller spindle. I doubt that many home-built machines can fully load the bigger spindle and the main reason for choosing the larger size is they usually take ER20 collets which allow up to 1/2" cutter shanks.

I've got a 2.2kw WC spindle coming for a new build, what size cutter could these handle in aluminium??

I have read that torque drops badly at lower speeds but what is the usable range???

[Chaz]

I've got a 2.2kw WC spindle coming for a new build, what size cutter could these handle in aluminium??

I have read that torque drops badly at lower speeds but what is the usable range???

Typically 12 - 24K. Size of cutter all depends on width and depth of cut.

http://zero-divide.net/?page=fswizard get used to using this, it also tells you how much power you need.

[Davek0974]

Typically 12 - 24K. Size of cutter all depends on width and depth of cut.

http://zero-divide.net/?page=fswizard get used to using this, it also tells you how much power you need.

Thanks, looks like small cutters and solid carbide are the way forwards. HP does not really factor until you get up in the 10mm dia range and a 10mm carbide tool is quite spendy. But at that size machine rigidity would be a serious factor so conservatively I would guess that carbide cutters <5mm dia are the order of the day for aluminium.

Good calculator in that link BTW

[Chaz]

Thanks, looks like small cutters and solid carbide are the way forwards. HP does not really factor until you get up in the 10mm dia range and a 10mm carbide tool is quite spendy. But at that size machine rigidity would be a serious factor so conservatively I would guess that carbide cutters <5mm dia are the order of the day for aluminium.

Good calculator in that link BTW

Ye, very good as a starting point.

Stick to 2 flute for alu, my 'favorite' sizes are 8mm roughing, 6 and 10mm for finishing, 4mm for smaller if needed.

[JAZZCNC]

Stick to 2 flute for alu

Not always the best for Alu. It depends on the job and type of cut. If your profiling for instance and not slot cutting then more flutes are better. They allow faster feed rates with higher MRR and give better finish.
I find 3 flutes are best at roughing.? They are Stiffer and more ridged so can cut deeper. Feed rate and MRR is higher. They give a better finish if not roughers because More flutes.
The only thing is they need more attention to chip clearing and chip clearence. So not ideal for Slotting or small pockets and tight corners where tool cuts on two edges. When used with trochoidal tool paths they rock compared to 2 flute and can be run much faster with more DOC.

[Chaz]

Not always the best for Alu. It depends on the job and type of cut. If your profiling for instance and not slot cutting then more flutes are better. They allow faster feed rates with higher MRR and give better finish.
I find 3 flutes are best at roughing.? They are Stiffer and more ridged so can cut deeper. Feed rate and MRR is higher. They give a better finish if not roughers because More flutes.
The only thing is they need more attention to chip clearing and chip clearence. So not ideal for Slotting or small pockets and tight corners where tool cuts on two edges. When used with trochoidal tool paths they rock compared to 2 flute and can be run much faster with more DOC.

Agreed but generally this is good advice. I use 3 flute 8mm corn cob to rough. The rest are 2 flute.

Certainly anything higher than 3 in alu generally is a problem for most.

[Davek0974]

Great, thanks.

Things are simpler on my manual Bridgeport - just throw in a tool, set the speed to the chart and turn the hand wheels at a rate that keeps her happy :) Got a lot to learn - my reason for building a CNC partly.

So i have a g-code file from SheetCam and it was programmed for say a 6mm roughing cut leaving an allowance for finish, do i need to make a second file for the finish cut or do you use the same cutter but just program a final cut for the finish pass??

One job i have in mind has some 3mm holes in it, i would be looking at ramping in with a 2 or 2.5mm tool for them and then do the outside profile with a larger tool maybe - I am lacking knowledge of how you change tool and get back to exactly the right place OR do you use the tool dia offsets in Mach3

As i said, lots to learn;)

[JAZZCNC]

Agreed but generally this is good advice. I use 3 flute 8mm corn cob to rough. The rest are 2 flute.

Certainly anything higher than 3 in alu generally is a problem for most.

No it's not generally good advise because depends on the type of cut and machine, along with several other factors like cooling etc.
Slot cutting is worst case for most because chip clearence is less so people use less flutes to give more clearence. But if the machine is strong enough and cutting parameters are correct then 3 flute will work just fine and give higher MRR. It's generaly only good advise to those that don't know there machines capabiltys.!
Like wise for finishing or cutting with plenty of chip clearence like profiling then multi flute cutters work great provided the machine can handle the higher feed rates. People go wrong by using multiflute cutters is wrong situations or more often much too low feedrate. If run correctly in right places multiflute cutters give a much better finish.

[routercnc]

I sometimes use 6mm 2 flute carbide tools with a 45 degree helix, but they are a little more expensive.

The more standard 30 degree helix also works but the 45 degree angle is supposed to be more tailored to aluminium cutting.

[JAZZCNC]

I've got a 2.2kw WC spindle coming for a new build, what size cutter could these handle in aluminium??

I have read that torque drops badly at lower speeds but what is the usable range???

The usable range is between 5000 and 24000 rpm if the VFD is setup properly. But yes torque does drop at lower speeds so does have limitations.
You can use the full cutter size range upto 13mm in aluminium but it will affect DOC and Feedrate. I cut lots of aluminium and find 8mm with 3 flutes is nice size that allows good DOC and feed rates. If used with trochiodal toolpaths the removal rate is brilliant and shifts large amount of chips.

My 2 most often used cutters are 8mm 3 flute rougher and 6mm 2 flute spiral flute for finishing. When ever possible I use Trochiodal toolpaths.