Noobs' Feeds & Speeds

Hi All,

I want to cut a 50mm diameter cylinder out of a block of 6061 aluminium that is 40mm thick. I have downloaded GWizard to determine the correct feed and speed. My CNC machine is a 6040.

The figures entered into GWizard are:

Material - 6061 aluminium
Tool - Carbide Endmill
Tool Dia - 6mm, 3 flutes and a 'stickout' of 40mm
Cut depth - 4mm
Cut width - 4.6608mm (I don't understand this bit)
KW limit - 0.8kW
RPM Limit - 24000
Min RPM - 1200
Feed Limit - 10160 (2%) (I don't understand this bit either)

The RPM comes out at 14031 RPM and Feedrate 205.3 mm/min

All the reading are now in black but a warning re "Chipload is low, may cause rubbing!" is displayed.

Please can someone check my figutes and what will be the best way to mill this cylinder from the block?

Regards

Gary

Gary,
I'd try a ramped profile cut, experiment with shallower DOC to see what the calculator says.
Any calculator will assume a rigid milling machine though, which few of us have.
See what the calculator says about a single flute cutter, they're great for chip clearance,

- Nick

Hi Gary,

I take it you have filled in the setup page for your machine i.e. use generic gantry router and specify the weight of the gantry etc?

The two settings you don't understand are:

Cutting Width = Step over - what CAM strategy are you using to mill the cylinder? (I assume from a square block) If you are going for a slot cut then you should use 6mm and if using side milling of some sort then use 2.4mm on a 6mm cutter (although a 6040 machine may struggle with this much depending on depth of cut).

Feed Limit = the feed rate of your machine before stalling occurs or the feed rate limit you have setup in the machine control software (MACH3?) (The 2% is the % of the limit the suggested feed rate is running at e.g. GWizard may suggest 1000mm/min for a machine with a limit of 10,000mm/min, which would be 10%).

As Nick suggests I would try a single flute cutter for aluminium, unless you are going to side mill the block inwards to the cylinder using something like adaptive clearing or a similar strategy and then I would say your feeds for a 3 flute cutter are too low.

Hi Nick and Washout,

Thanks for the explanations and ideas. I entered various values into GWizard and selected 'Fine Finish'. Here are the final figures calculated:

1 flute 6mm carbide endmill
50mm stickout (Bottom of collet to tip of endmill). The block of Aluminium is 40mm thick.
1mm depth of cut
15671 rpms
2.76 mm/sec (165.5 mm/min)
Fine Finish

Any higher and the deflection is too much, so now to buy a good endmill :)

To use a 3 flute, I would need a spindle speed of 36,000rpm. My 6040's max is 24000rpm. I don't know the weight of my gantry. I didn't think to check that before assembly. I have purchased a 'clock micrometer' to check the alignment of the gantry to the bed.

"using something like adaptive clearing". OK, I need to read some tutorials.

Cheers

Gary

Gary,
Have you tried a shallower cut with faster feed with the 3 flute? You ought to be able to get enough advance per flute that way, you'll need air to clear chips and cutting lubricant (WD-40 or a 30/70-20/80 engine oil/paraffin mix) to reduce chip adhesion to the cutter, a quick squirt into the cut once every pass or two is usually adequate,

- Nick

Hi Nick,

OK, back to GWizard to try new numbers. I have an aerosol of cutting oil and a small air compressor and gun. As this will get messy (I was hoping to make dry cuts) I need to find/make a large perspex cabinet/cover. Yet another project, O Joy!

Cheers

Gary

Hi Gary, my 6040 are not too fond of deep (long stickout) cuts with any 2 flute cutters. 1 flute seem to be much more in harmony with the rigidity, on my machine at least. The cutters I prefer, are from sorotec.de, 1 flute alu end mills. They stay sharp forever, and dont break easy.

Just my thought on what have worked best for me.

Quote:

---

Originally Posted by sinnsvak

Hi Gary, my 6040 are not too fond of deep (long stickout) cuts with any 2 flute cutters. 1 flute seem to be much more in harmony with the rigidity, on my machine at least. The cutters I prefer, are from sorotec.de, 1 flute alu end mills. They stay sharp forever, and dont break easy.

Just my thought on what have worked best for me.

---

Hi sinnsvak,

Many thanks for that information. I was having problems finding 1 flute endmills. I'll purchase one from Sorotec.

Regards

Gary

Hsmadvisor....

much better than gwizard imo.

HSMAdvisor here too.

Input your data and then set the cutter engagement slider to minimum performance for this machine.

Oh, and will definitely need lubricant on that - WD40 is good, paraffin too, maybe air-blast to clear the chips, chip recutting is a major tool-killer.

4mm pass depth with that machine is ...:boxing:

3 fluted mills are ok, i don't know what the hassle with that one flute mills? I do absolutely perfect cuts in plastic wood and aluminum with 3 fluted mills.


Calculators are superb though. But without any calculator i will tell you that 3mm pass, 12k rpm and 25-35 ipm will work on any machine similar to yours with good result and without coolant. Though you have to stay there to blow chips out from pocket otherwise it would rub them between cutter and material and here the bit brakes...

My one will push a 5mm single-flute carbide at 19,000rpm and 900mm/min or 35ipm and 2.5mm pass depth, its a fairly heavy cut and will fling hot chips at you ;)

It has a 2.2kw water-cooled spindle on it and was built to cut aluminium.