[matttargett4]

Hi,,
Im not sure if im posting in the right section but hopefully people can help anyway.

I have built a diy mill, working area 700mm x 400mm x 250mm with a mini mill spiindle from lms, a belt drive to it and a 1kw servo motor as a spindle motor, max rpms about 1500 at the moment. The machine is about 200kg, uses linear rails and ballscrews and servos.

Today i got my first real attempt at cutting metal, i was just playing around with a piece of 15mm mild steel, trouble is i dont have loads of machining experience so im not really sure if its going great or hopeless!!

I used the feeds and speeds wizard in mach as a start off and a middle of the road chip load from a table that was posted here, i was running a 4mm end mill at max rpms, 75mm/min depth of cut was about0.5mm, a 6mm end mill at 1500rpm, 125mm/min feed at around 1mm doc 8mm end mill very similar settings and a 10mm end mill at 1200rpm around 150mm/min. all of the mills are 4 flute centre cutting tin coated hss.

The 4mm was pretty quiet but i was getting quite a lot of clicking noise from it, i guessed it was too slow?

6mm seemed best, was quietest, you could talk comfortably next to it, didnt seems to get too hot etc etc

8mm worked good too, was louder, you had to talk reasonably loud and the ground seemed to be starting to shake, in deeper cuts, approaching 2mm the chips were thinking about going blue, a little cutting oil made a slight difference to the noise but not much.

10mm sounded bumpy by comparison to the others, like it was slow, but i was thinking 1200 was getting on for 10mm, the ground was definately shaking more.

Surface finish looked great with all of them, there was no difference between climb or conventional milling in terms of noise, the conventional cut looked slightly deeper against the climb cut, so the pattern always showed a complete spiral for the conventional cut and a half for the climb cut, but there was no ridge to feel between them, i think this may be flex in the machine, the deep cut is where the machine is pushing the head so dipping the front and the shallow is where it is pulling the head.
there was a point where when turning on the end of a cut the tool would go quiet, according to the feedrate in mach it wasnt because the tool was momentarily stationary, i was using 30% stepover in all cases.

What does all of this mean, am i somewhere on the right track? I realise that my machine well never be as quiet as a 3t brideport but whats normal? I wouldnt have said that the tols were chattering, with your hand on the head there was just a distant vibration.

Thanks for any help
Matt

[SCzEngrgGroup]

Start with SFPM - Surface feet per minute:

SFPM = ToolDiameter * Pi * RPM / 12 or:

RPM = SFPM * 12 / ToolDiameter * Pi which can be approximated a:

RPM = SFPM * 4 / ToolDiameter

ToolDiameter in inches, obviously.

SFPM, using HSS tooling, should be 80-100 for mild steel, 300-400 for aluminum. Double or triple these if using carbide (which, given your very low spindle speed, would be a waste of money....).

So, for a 1/2" endmill in mild steel:

RPM = 100 * 4 / 0.5 = 800 RPM.

Next pick a chipload. For tools over about 1/8", you can assume about 0.010"/inch of tool diameter, progressively less for tools under 1/8". So, a 1/2" tool would be 0.005-0.006" chipload.

Feedrate is then:

Feed = RPM * chipload * #Flutes

So, for a 1/2" 4-flute endmill at 800 RPM:

Feed = 800 * 0.005 * 4 = 16 IPM

Plunge cuts should plunge at 1/3-1/2 the calculated feedrate.

This will give you a starting point. Make a shallow cut (the definition of "shallow" depends on how rigid your machine is....), and see how it behaves. It it's happy, then go a little deeper, and keep going until surface finish starts to degrade, the machine starts shaking, the spindle bogs down, etc. At some depth, you'll need to start backing off on feedrate and/or to avoid the spindle bogging down, or the tool loading up.

When you've got it right, there will be no shaking, no squealing, no strange noises. Just a nice, even "humming" sound. Every machine will be different, and parameters that work perfectly on one machine, may work horribly on another supposedly identical machine. You MUST learn how to "read" the cut to get the most out of your machine.

Contrary to intuition, increasing RPM and/or decreasing feed in an attempt to "go easy" on the machine or tool is the WORST thing you can do, and will lead to ruined cutters. When you've got it right, the chips will be coming off very hot, and the tool will remain cool, and a single tool will last an unbelievably long time - I've got endmills I've used for months on end, and they still cut perfectly. If your tool is getting hot, or loading up with chips, then reduce RPM, and/or increase feed. You'll get the maximum removal rate when your running right on the edge of breaking the tool, but that's also where it will be the happiest.

Regards,
Ray L.

[maker of things]

Ray,
I was just looking for the same info. That was very helpful.

[UUU]

Your clicking noise might be the cutter eating its own chips. If these come off hot and hard then it's not good for the cutter to be swimming in them. If you can blow them away you may find your clicking disappears.