Can somebody help me, on how to calculate the right feedrate in mm pr.

diycnc-discuss
gplus
(Jørgen Vendorf) #1

Can somebody help me, on how to calculate the right feedrate in mm pr. min?
I know it is only a guide number.

I have a 2 flute end mill at 3 mm.
I run my router at 15000 rpm
Cutting depth is 0.1mm
I`m cutting hard alumimium.
My max feedrate is 1000 mm/min.
The table i use for chip load says 0.05 for hard aluminium.
Router is 2 HP, 3500 - 30000 rpm

From the sound of the cutting, the ideal feedrate is around 300 mm/min. But my calculations says 1500 mm/min.

(Max Kalin) #2

I never calculate anything, I just try.
So maybe 1-2mm/1sec? If the flute works well then raise the speed?
I usually start from low and go up.

(Eugenio Villaverde) #3

i have any videos cutting 1,5mm aluminium sheet with 1 flute at 18000rpm with 600mm/minute… for 2 flutes i think about 10000 rpm and 500mm/min feedrate but the most important is the cooler of the tool i think oil or some oil spray or pulverized water with a bit of soap… deep about 1,5mm to cut

(Alan M) #4

does your machine have a lot of deflection?
@300mm/min is only 0.01mm per tooth

1500mm/min sounds right at 0.05mm per tooth.
you could go lower, around 0.025mm per tooth which would be 750mm/min

(Henrik Larsen) #5

Using http://zero-divide.net/?page=fswizard, i get about 500mm/min at recommended 10000RPM, from what you gave of info. Try yourself.

(Max Kalin) #6

@Henrik_Larsen thank you for the website. I didn’t know it existed.

(Jørgen Vendorf) #7

Thanks, that wiz gives me a much better result.

(Henrik Larsen) #8

Giving your tried speed of 15000 @ 300 compared to 10000 @ 500, then your ears was quite right in fact. Yours and the calculated would result in about the same chipload. But the little higher feedrate and lower RPM will probably reduce tool wear though.

(Henrik Larsen) #9

Usually when working aluminum you would use spirit as tool grease. Just spraying it by hand. This is because aluminum and spirit work well together just like iron and oil.

(Jørgen Vendorf) #10

I use Spirit with a few drops of oil on Aluminium. Currently applied with a small brush.
For acrylic I use a water with soap solution.

(ArtClip3D Software) #11

I use Empiric formula like those:

(1000 x CS) / Pi x D = N

N is the Spindle Speed (RPM)
D is the diameter of the tool in mm
Pi = 3.14
CS is the Cutting Speed of the material (mm/mn)

For Hard Aluminium you can read an average of 400 m/mn (http://www.kennametal.com/content/dam/kennametal/kennametal/common/ATI%20Metals/Stellram/Catalogs-Literature/Turning%20pdfs/Stellram_turning_cutting_speeds_inch.pdf)

So N will be 1000 x 400 / Pi x 3 = 42465 RPM

From N you can compute F which is the Feed rate.

F = N x Z x Zf
Where N is the RPM previously computed.
Z the number of teeth/flute
Zf the feed per tooth (given by your tool supplier: mm/tooth )

F = 42465 x 2 x 0.03 = 2547 mm/mn or 2.5 m/mn

Hope this helps!

(Michael Jacobsen) #12

Does the type of end mill matter? Belive i’ve seen some end mills that are made for cutting alu at high speed and no coolant (coolant actually make them work worse) … ?

(Kyle Kerr) #13

@Michael_Jacobsen sure it does. High speed steel is different from carbide.

(Max Kalin) #14

@Michael_Jacobsen As far as I know, coolant is used to the chips would not stick to the bit. Otherwise you will end up with a chunk of material on your bit. But since you’ve seen, can you post it? I’m interested what kind of bits they are.

(Michael Jacobsen) #15

This one doesn’t seem to use any coolant/vapor: http://www.youtube.com/watch?v=9DhcAiV5U34&spfreload=10%20Message%3A%20JSON%20Parse%20error%3A%20Unexpected%20EOF%20(url%3A%20http%3A%2F%2Fwww.youtube.com%2Fwatch%3Fv%3D9DhcAiV5U34)

(Michael Jacobsen) #16

This is also impressive: http://www.youtube.com/watch?v=aeH-joXOUb0&spfreload=10%20Message%3A%20JSON%20Parse%20error%3A%20Unexpected%20EOF%20(url%3A%20http%3A%2F%2Fwww.youtube.com%2Fwatch%3Fv%3DaeH-joXOUb0)

(Emmanuel Robert) #17

the N=1000Vc/Pi/D is not an empiric formula : it is the required formula.
F = N x Z x Zf is too.
Pb : it doesn’t give the required power for the spindle. Such a power formula exists : it requires to calculate the Force of the spindle on the material.
If you reduce speed because spindle cannot turn theses speeds, you must adjust the F formula according to your real spindle speed.
Be aware that there are 2 kind of cutting techniques : classic with low speed and high forces (high power required) and high speeds with low forces. Spindle are part of this last one. The 2 techniques don’t overlap. So you should be aware that you need to run at high speeds (>7000rpm) with your spindle.
Good luck

(Emmanuel Robert) #18

PS coolant may not be necessay at high speed because temperature (energy) is supposed to go with shavings because they are very small.

(Jørgen Vendorf) #19

Thanks alot for all the nice responses. I think I have the grasp of it now and will try some cutting.

(Michael Jacobsen) #20

@Jorgen_Vendorf , @Henrik_Larsen : Think we’re in the same country. Where do you buy stock material, e.g. Alu? Any tips?