1mm Ball End Mill Speed's

[ahooper]

I am trying to make a couple of Dies that will allow me to stamp a logo in to copper however the largest mill bit I can use is 1mm. I have purchased a 1mm TI coated Carbide bit however am a little confused as to the manufacturers specs and how to work out the feed/plunge speed as well as the RPM.

My mill is a converted Sieg SX2 and has a top speed of 2500RPM. I have reconfigured the steppers to allow me to run at really low XYZ speeds.

I am using a heat treatable steel somewhere in the 900 to 1200 N/mm2
The manufacturers recommendation is as follows..
Speed in m/min: 50
feed (mm/tooth) 1-6: 0,01-0,025
and I can exceed these by 20% if the cutter is coated.

I would appreciate any suggestions as to how to work the feeds adn speeds out and hopefully something i can apply to other bits.

Regards
Andrew

[txcncman]

This is actually very simple math that people that claim they want to be machinists continue to refuse to learn. For metric values, the formula is: RPM = ( Desired cutter speed expressed m/min X 1000 mm/m ) / ( Pi X Diameter mm ). Be sure to do the math operations with the correct Order of Operations.

In your case, you are limited in RPM by your machine. So, take your maximum RPM and calculate the feed rate with: Feed = RPM X # of teeth X desired chip per tooth.

[ahooper]

Thank you for that. That's a simple formula.

Just be be sure I am not missing something.
RPM = The speed that my cutter will rotate.
Desired cutter speed expressed m/min = Surface speed of the cutter
Diameter = outer diameter of the ball or cutter.

Based on this the max surface speed for my machine and a 1mm ball end mill is
7.85mm/m with an RPM of 2498.73.

Where does the chip out come in to play? and would this be the same speed for the plunge rate? or should the plunge be slower?

Thanks heaps for that, everything I have read previously seems a lot more complex.

[txcncman]

I would program the plunge at about 1/4 of the linear feed rate. I do not think you mentioned the number of flutes on your cutter.

[ahooper]

The 1mm ball mill is a 2 flute however I have a couple of others that I think are 4 flute and an engraving bit that really only has 1 flute.

[txcncman]

You gave a range of chip per tooth as 0.01 to 0.025 mm per tooth. For 2498.73 RPM (round to 2499 RPM) X 2 X 0.01 = 49.98 mm/min feed.

[txcncman]

Plunge at 1/4 X 49.98 mm/min = 12.5 mm/min.

This is with the lower recommended chip per tooth number. You can go up to the higher number, or any range between at your own risk.

[ahooper]

Wow that's heaps faster than what I had it set to.

I made up a spreadsheet so I can calculate all of the mill bits I have and keep a list of them.

My initial settings were 1800 RPM, feed of 9.8mm/min plunge of 6.5mm/min
I broke one of the bits at this speed but am not sure if this was due to the cutting fluid having stopped flowing or something else..

So according to the calculations I should be able to run the RPM up to 2500 with a feed rate (surface speed) or 49.97mm/min and a plunge rate of 12.49mm/min.

How about the depth of cut? or is this the 1/2 the depth of the ball?

I really appreciate the assistance, much prefer being able to learn and understand the calculations and reasons for them

[txcncman]

Recommended axle DOC and radial is usually 1/2 of tool diameter at maximum RPM and feed. If you find you are cutting harder material or having chatter problems or such, reducing the DOC is recommended.

[ahooper]

Well here is a spreadsheet i created to save some headaches calculating these speeds and feed rates.

I have no idea as to how accurate it is and the calculations may be way off so use at your own risk...
you can change any of the white fields to give you the answer..

Something I am a little confused about is the Desired Speed. I am amusing that this is the speed that I want the mill to move in the X/Y axis however I am not sure as to why the actual feed rate is much higher than the desired.

Or is this figure based on the rate per tooth per rpm...

Anyway i would love some feedback on the spreadsheet if anyone has the chance to take a look and check it.

Regards
Andrew

[Astonlee]

For these tools to work get rid of the coolant and use an air to remove the chips, otherwise the coating cannot do it job. With a 1mm dia tool you need to use the maximum rpm you have to generate heat that the coating needs to form a ceramic coating on the tool.
It your programming software will allow you: rough from the top down, but finish from the bottom up, you will be amazed at the difference.

[ahooper]

Thanks, I will try that as all I need to do is remove the fluid and up the air pressure in the spray system.

My mill has a top speed of 2500RPM and with the specs on the new cutters that arrived today they have a much shorter flute length. The specs say that HRC60 speed(mm-1) is 20000 Feed mm/min 200
I am guessing that the mm-1 refers to the speed per tooth and this gives me a chip load of 0.005.
that should mean 25mm/min feed and 6.25mm/min plunge.

The logo I am milling is all one level and only .3mm deep.

Regards
Andrew Hooper