Milling steel on a small mill - speeds, feed, doc, step over?

I have a Servo Products mill with limited spindle power. I think it might be close to Sherline for spindle power but a lot heavier and more rigid with ball screws. I mill aluminum with no problem. But my try with steel haven't been good. I think the issue may be speed, feed, and doc. For mild steel with a 0.25" 2 flute end mill what is a reasonable speed, feed, doc and step over for pocketing with carbide end mill? I tried to do some - it ran for a while but ended up stalling the spindle and breaking the oring belt. I don't have all the settings but think I was doing 0.020" doc. Not sure how much step over. I have two sets of pulleys for two speed ranges. I was running 6000 RPM - max in low range. 6 ipm for 0.0005" per tooth. Max collet size is 0.25". In reviewing the numbers that seems pretty conservative so I'm thinking I had a large step over. In looking at this again I am thinking I should cut the rpm to 3000 and keep the feed rate for 0.001" feed per tooth and reduce the stepover to 0.050. Then adjust the depth of cut. Thinking less step over and more depth of cut uses more of the cutter edge so it will last longer.

How do I tell when I am getting near the limit of the belt drive so I don't bust a belt? I have thought of putting a sensor on the spindle to measure drop in speed. I could even put one on the motor pulley too so I would be able to know slip but is there a simpler way?

Can't advise on settings but in terms of watching the rpm these little units are great for the price:
https://www.ebay.co.uk/itm/4-Digital...koB:rk:42:pf:0
Using one on my X2 mill.

Hi,
the spindle speed is determined both by the material the tool is made of and if it is coated.

For a coated carbide end mill in mild steel the approx surface speed is 100m/min. You can go slower without problems but if you
attempt to go faster and most certainly if not using cooling you'll fry the tip of the tool.

Just as a matter of interest the same tool in stainless you'll be down to 50-80 m/min and if in aluminum about 200-300 m/min.

Lets do the calculation:
1/4 inch= 6.35mm
tool circumference = PI X Diameter
= 3.141 X 6.35
=19.94 mm
or approx. =0.02m

desired surface speed = rpm x tool circumference
so rpm=desired surface speed / tool circumference
=100 / 0.02
=5000 rpm

Thus your speed, 6000 rpm is a little bit too quick.
at 1% per tooth per revolution the cutting speed should be about 0.01 x0.02 = 0.2mm per tooth or 0.4mm per revolution for a two flute tool
and at 5000 rpm 5000 X 0.4 mm =2000 mm/min.

The problem is that is going to require a lot more power than you baby spindle has got. Even if you reduce the feed speed it is still likely that the tool
requires more torque than you spindle can deliver and either the tool will stall or you'll break the belt.

Cutting steels and stainless requires low (ish ) rotational speeds but high torque.

That does not sound like the description of your spindle.

Craig

You're probably going to need less of everything.

I machine some hardened steel bearing races on my G0704 and to get a really nice round finish I run like 1800 rpm with a 4 flute .2" end mill at something like 3 ipm. Without doing the math too in depth, that's like 3600 rpm on a 2 flute but still 3 ipm. That's with a small step over, like .040" or less. Keep in mind my mill is stronger than yours, though still not remotely strong. Also, hardened steel is of course harder to cut, but going conservative and dialing back is always better with steel IMO. You aren't doing any big runs with your system anyways.

Joeaverage, your feeds and speeds look like they are for a "real" mill. Clearly those are bigger and nothing I can get close to. Your points on surface speed do apply and I should decrease RPM, probably to less than 5000.

People claim to mill steel on small machines. I am guessing the spindle power (torque) is similar since they are both belt drives. Mine is more rigid than a sherline - a lot more I think - so it should be possible. Likely with small depth of cut, feed per tooth and step over. For pockets on initial plunge I don't see a way to cut less than full width of the cutter. I don't want to take such a small chip that I have rubbing instead of cutting. I am hoping some users of small machines will respond with settings and tips for steel.

Just ran through some speed/torque numbers for both machines from the spec sheets:

Sherline:
Speed ranges: 70 - 2800, 70 -1280 (also have a 10,000 RPM pulley set but lower speeds are standard spindle)
stated power: 60W
Stated torque: 10 oz-in continuous, 30 oz-in intermittent
Motor Max speed 6100 RPM (torques are motor not spindle)
Stated power of 60 W falls somewhere between 10 and 30 oz-in at max speed
Assuming 60W and 1280 RPM the torque is about 63 oz-in.

Servo Products 7405
Speed ranges: 200-4000, 1000-20,000
stated power 1/4 Hp, approx 188W
188W at 4000 RM is 65 oz-in of torque which should be approximately what is available with that belt ratio

The torque numbers come out essentially the same. I suspect the 1/4Hp may not be a continuous rating so the numbers for the Servo Products unit may be a bit lower than I have calculated. I also think the Sherline belt can likely handle more tension so may be able to transmit more torque before slipping. I also noticed that my spindle shaft has very little inertia - if it hits a chip or rough spot more inertia would help to get through. I am guessing the Sherline is fairly similar.

All this is approximation and estimation but I thought it would be useful to compare the two spindles.

Hi,
when I made my mill I selected a 750W German made 24000 rpm spindle.

I had hoped that if I slowed it down (with the VFD) that it would cut steel. If I use a 3mm two flute tool I can slow it down to
about 9000rpm, the slowest effective speed, lower than that and the spindle starts to overheat.

If I take very light cuts (1mm) at slowish feeds (240mm/min) it does cut mild steel. The real problem is if I try to take a larger
cuts the spindle stalls. Once the tool stops rotating and the machine continues feeding the tool snaps. In short the spindle has been
absolutely great for engraving, making PCBs and does a good job in aluminum with up to 6mm tools it is not up to cutting steel.

I decided to make another spindle for steel and stainless steel.

I was lucky to buy a second hand Allen Bradley AC servo and matching drive in New Zealand for $800NZD ($550 USD) including shipping.
I still had to buy cables and I also bought the Allen Bradley setup software. Even still I got a good buy. The servo is 1.8kW, 6.2 Nm continuous,
18 Nm peak and rated 3500rm.

I bought a cylindrical ER25 toolholder from Rego-Fix (Swiss made) and NSK P4 angular contact bearings and made my own direct coupled spindle.
I did the lathe work myself. While its not perfect I am still pretty proud of it. It takes about 15 minutes to swap between the highspeed spindle and
my high torque 'grunter'.

It cuts steel like a DEMON!!!! The problem is that my mill is not really a stiff as I had thought.....but still I can cut as much steel or stainless steel as
I can offer up to the spindle.

I think if you are going to cut steel then you should consider either replacing your existing spindle or swap it for a slower but MUCH higher torque unit.

Craig

I ended up finishing the job on a bigger mill I had access to but no longer do. I ran the numbers through the calculator at
https://www.custompartnet.com/calcul...ing-horsepower

6 IPM
0.1" stepover
0.020" depth of cut
6000 RPM
unit power 2
machine efficiency 80%
Results:
power = 0.030 hp
Torque = 0.252 in-lb

Those seem pretty low so perhaps I have made some mistake.
If those are correct power should be no issue. Torque seems pretty low but I am getting a torque watch to check the static torque for belt slippage. I realize I need to add a substantial margin for running condition. and for peak loads when it may recut a chip.

Given that torque and the 0.125 radius of the cutter, if all the force is in one direction (it isn't so this is worst case) then then side force on spindle will be 0.252/0.125 = approx 2 lb force. This seems pretty low also.

I should use less RPM - if I half the RPM and half the IPM then torque will be the same, power will be half.

I will be doing some more checks. Let me know if these look right or where I made mistakes...

I measured the torque at the spindle when the belt slipped (turning the motor pulley by hand):
High speed - 1.6 in-lbs
Low speed - 4.5 in-lbs

The belt is basically a big oring and stretches quite a bit before slipping. I am thinking I should keep the load at half (or possibly less) of the slip torque. But at that point it is still 10x the calculated torque for the cut. I also had air nozzle on the cutter to remove chips. Perhaps my calculations are off. Still not sure why the belt broke.

Conventional or climb milling?
I'd try 2 things

1. a 4 flute cutter, just because that's whats worked for me in steels - and even though its not a huge difference the cutter tends to be stiffer for the same size and length. You don't need the chip clearance like you do in aluminum. You also get more IPM for the same same SFM (RPM). Helpful when milling steel and its taking a long time
2. Try conventional milling (up-cut). With climb milling any machine backlash can be translated to a suddenly large chipload which can stall the spindle - especially on a small machine. Think that even a 0.0005" backlash movement can double your chip load (i.e torque) if you were running at a chipload of 0.0005"

Mike

An O-ring drive? I would start by replacing that with a 6 mm GT2 belt!

Cheers
Roger