Burning out end mills!

[jim_cliff11]

Hi all,

I have a Bridgeport series 1 milling machine running Mach3 with 3 servo controlled axis.... Machine works great, and get ALOT of work.
One of its main jobs is machining out bar. Three pieces of bar sits in a jig and each piece is 50mm wide, 20mm deep and 300mm long. I use a 12mm 2 flute slot drill.
I spiral drill 2 holes into each bar with one at either side (first cut to 20mm diameter, second cut at 27.95mm diameter). After the drilling a radius edge is then machined onto the end of each bar.

I use G-wizard to calculate my machine feeds and speeds.

My problem is.....

I get through one end mill for every three bars. Eventually the end mill melts around the cutting edges and fails. Whether I cut at a 2mm depth or 6mm depth it doesnt matter. I've tried using a 4-flute end mill with the same result. I don't use coolant, but instead a consistent air blast.

The machine is set up as per G-wizard instructions:

12mm end mill
2mm cut depth
12mm slot
1229rpm
130.3mm/min feedrate
65.1mm plunge.

This is annoying and expensive when I'm machining several sets of bars a day.
Pictures attached

Can any of you pro's shed any light on this issue?

Thanks,
Jim

Similar Threads:

• Eprom burning
• Burning Questions
• tool burning
• Burning Out Motors?
• drives burning up

[ToolHIT]

I have a few questions on this JIm: What is the material you are cutting? It looks like you are currently using a 2 Flute Cobalt End Mill, correct? What do you mean by the 65mm plunge?

If you are using a 2 flute cobalt end mill then your parameters aren't too far off for a low to medium carbon steel (I'd start at 900 RPM and 110 mm/min). The slower parameters would help but you still wouldn't see too much of an increase in tool life. The best way to increase tool life would be to either use a coated tool or go with a stronger substrate.

If you would like to stick with a Cobalt End Mill then I'd add either a TIN or TICN coating. Either of these coatings would give you better heat resistance and increase tool life for you. TICN would be my first choice, here's an example (1/2" Diameter instead of 12mm)
https://www.toolhit.com/products/01321cc

If you are looking for the longest tool life possible then I'd go with a Powdered Metal End Mill. This is a much harder substrate with better wear resistance than a Cobalt End Mill giving you long tool life (but it still has great toughness). Here is an example (1/2" Diameter as well)
https://www.toolhit.com/products/e9983032tf

Hopefully this helps Jim,

Mike

[Jim Dawson]

You don't mention what the material is, but why not try carbide. Normally when I am burning up end mills, I slow the spindle down. This may require slowing down the feed rate also, right now you are at about 0.05mm tooth load on a 2 flute. If you went to a 4 flute, and slowed the spindle down to about 600, kept the feed speed the same, then the tooth load would remain the same which is in a reasonable range for a 12mm cutter.

Other than that, I agree with @ToolHIT

[warrenb]

Are you taking that full cut in one pass?

[jim_cliff11]

thqbks for the replies.

I'm cutting mild steel. The end mills cost me about £4.50 each and are a standard HSS steel so that's probably about right tool life wise then? I was thinking of adding a coolent setup which should extend life.

Also I might try the powdered mills and see how I get on.

Taking a 2mm cut over ten passes. But previously took 6mm cuts. No difference between 6 and 2 mill cuts in terms of tool life.

Although what does confuse me is Gwizard recommends practically the same federate for both a 2mm and 6mm cut :/

[Tarzan63]

The feed rate is determined by
(rpm X chipload( I.e.- load per tooth) X number of teeth)
recommended chipload per tooth should be available from the EM manufacturer, or you can just look it up in the machinerys handbook to get a safe starting point.
There is a starting range they give you, say .001- .003 per tooth . You select where you think you will be to start. You need to adjust from there.

Typically the federate will be determined by surface finish and tool wear. Oftentimes you can use the same feedrate for a small range of DOC. , but if the machine is bogging down or the endmill starts to deteriorate rapidly you should probably back the feedrate down a bit, considering that you have the correct rpm already.

Personally, I think your EM is showing that it is getting hot from lack of cooling. I would use a mist system or flood coolant if available.
But as has already been pointed out, there are also coatings that will help with tool life and lubricity also to some extent that make HSS
tools better.
I use carbide for almost everything anymore. The tool life, surface finish and rigidity are all far superior for most materials.

[thaisurplus]

if your hogging hard materials you need more flutes

if your chips are the same color as your part your not taking enough material out and all the heat is going in your tool

if your chips are blue, the chips are taking out the heat.

try a 4 flute

[zero_divide]

You are going too fast for HSS

Here is results from HSMAdvisor for slotting:

Material: 1018 (126 HB)
Tool: 12.000mm 2FL HSS None Solid End Mill
Speed: 26.8 SMM/ 711.8RPM
Feed: 0.0498 mm/tooth 0.0996 mm/rev 70.88 mm/min

Even still. a coated carbide endmill while pricier will last much longer and be much more forgiving with mistakes in calculating speeds and feeds.

Also you should use cutting fluid when using HSS cutters to mill any sort of steel. Carbide should be used dry.

[KH0UJ]

On my opinion a 2mm nose dive of the bit is your problem, even though it`s just mild steel but the heat generated on a 2mm pass will eventually cause the tool bit to change it`s state, if the tempering state of the carbide bit will change then it wont be that hard anymore, a 0.5mm nose dive I think is good enough for mild steel, on my side I can cut all day on a mild steel without worrying my bit getting dull (24K rpm spindle watercooled) because im nose diving my bit lesser than 0.5mm your CAM pass is too aggressive sir. you can also use cooking oil + kerosene to act as a lubricant, a drop on it in every pass will work magic preserving your tool bit to it`s optimum state all day if you like

[brian257]

I would not expect cheap HSS end mills to last. You need coolant and carbide and 4 flute carbide end mills.