Blue chips

[mick70Participant @mick70]

Was told if I want to mill some steel should work to 400rpm for 1″ cutter half that for 2″ and double for 1/2″.
So thought as quiet at work would have go.
12mm 2 flute cutter and some mild steel.
Getting blue chips at 800 rpm.
New cutter so obv operator error.
Where have I gone wrong?
Mill as no makers plate on it but is similar in size to Bridgeport at my old place.
Only taking 1 mm cuts just wanted to make double sided clamp spacer.
On side 20mm other 10mm.

Edited By mick70 on 29/07/2018 04:44:47

[mick70Participant @mick70]

[not done it yetParticipant @notdoneityet]

What is wrong with that? Nothing obviously wrong! What colour chips were you expecting. Just get the job done.

[mick70Participant @mick70]

new to milling and guy who took our 2 day introduction to machinery course at work said blue chips mean damaging cutter.

said they should always be silver coloured chips.

so i was just obv being over cautious if nothing obviously wrong.

do those speeds he gave us sound about right?

[JasonBModerator @jasonb]

When using HSS cutters I tend not to push so hard that the chips come off blue, don't mind it that colour if using carbide.

Speed sounds the high side or rightt, could come down a bit  How fast were you feeding the tool into the work?

Couple of cuts with similar sized cutters but 3 or 4 flute so can be fed a little faster.

 

Edited By JasonB on 29/07/2018 07:59:42

[Anonymous]

Running a 12mm cutter at 800rpm is pretty much spot on in terms of surface speed for low carbon. Even at that speed I wouldn't normally expect to see blue chips, more straw or light brown. But I wouldn't be worried about blue chips. It's called high speed steel for a reason; it can run much hotter than carbon steel without losing its temper. To echo JasonB, what was the feedrate? And what about the cutter; new or old?

Rule 1: Cutters are a consumable item

A cutter is going to start wearing out as soon as one starts to use it. Cutting hard and fast will wear it out more quickly. But conversely running with slow feedrates will also wear the cutter, rather more quickly than running at high feedrates.It's a case of finding the happy medium without wasting time.

Andrew

[colin hawesParticipant @colinhawes85982]

Your 12 mm cutter should be nearer 500 – 600 RPM for general machining of non free-cutting mild steel. Colin

[Mark RandParticipant @markrand96270]

Posted by colin hawes on 29/07/2018 09:17:41:

Your 12 mm cutter should be nearer 500 – 600 RPM for general machining of non free-cutting mild steel. Colin

Possibly for a manganese or chrome or higher carbon steel. but that's very much on the low side for mild steel. 800rpm equates to 100 feet per minute, which is the right cutting speed for HSS in low carbon steels.

[colin hawesParticipant @colinhawes85982]

There is a difference between machining at production rates with a jet of coolant and machining on hobby machines with a low or non existent coolant flow. It is my opinion that many amateurs go for published production rates at the expense of tool and machine life expectancy and machining mild steel with HSS on a hobby machine should not be producing blue chips. Colin

Edited By colin hawes on 29/07/2018 15:41:56

[Anonymous]

Posted by colin hawes on 29/07/2018 15:40:21:

and machining mild steel with HSS on a hobby machine should not be producing blue chips.

Errr, the OP says he's using a Bridgeport size machine so does that mean he's entitled to produce blue chips?

Andrew

[Mark RandParticipant @markrand96270]

100 feet per minute on mild steel with a sharp HSS cutter does not need coolant and won't produce blue chips. So something else is going wrong. Either the cutter has become blunt (unlikely, it was new), The speed setting was mistaken, the feed was excessive or the steel wasn't as mild as was thought.

 

Apropos of the above, the lad has been turning swirly plastic into fountain pens in the shed and making aluminium or steel end pieces for the pens and caps. yesterday he brought me a ruined, almost new,  8mm long series MT1 drill (that he'd bought!) and a bit of bar with a nice shiny OD, a short ploughed-field-finish hole and a slightly blued end. I asked him which bit of steel he'd took off the rack and was told 'The bright finish 15mm bar with the red paint on it'

Verdict:- I need to teach him about material identification and appropriate feeds and speeds. If you grab a bit of stainless, and just tickle it with the drill, it'll work harden on you and eat the drill. The carbide insert had done a beautiful job on the OD, but carbide doesn't worry quite so much about light cuts on most stainless steels. Probably need a lesson on drill sharpening as well .

 

 

Edited By Mark Rand on 29/07/2018 22:40:23

[Mike PooleParticipant @mikepoole82104]

We seem to always be unsure of the correct speed and feed for milling cutters and lathe tools. The data is widely available for cutters and task materials. I understand that some people will find the calculations none to easy but there are websites that can do the calculation for you as long as you know the material you are machining and your cutter material. Speeds and feeds has to be something that we need to be familiar and comfortable with as it is an important thing to get right or at least close to. There are lots of memorable short cut figures to help get close to the correct speed and have been mentioned on various threads many times. 1000 inches a minute sticks in my mind as the cutting speed for mild steel 46 years after I learned it which is slightly odd as my apprenticeship was fully metric so 30 meters a minute would be more relevant. Pi can be 3 for most practical purposes or as many decimal places as you like if you enjoy irrational numbers.

Mike

[mick70Participant @mick70]

looking at jason's second video and speed he is going i might have been trying to go to fast.

will have to watch properly when i get home in morning as no sound on works computer.

but have always been bit heavy handed.

problem is i don't get lot of chance to practice on it.

 

Edited By mick70 on 30/07/2018 03:16:55

[HopperParticipant @hopper]

Cutting speeds and feed rates are rules of thumb. In real life, they vary with cutter, material, machine, the direction the wind is blowing etc. Start with the textbook setting as you have done, then experiment on the job. If you think you were feeding too fast, try slowing the feed down. If that does not work, try dropping cutter speed by one speed. Play with it and see what works for you on that machine with that material and cutter.

Change one thing at a time, in smallish increments. That way you can keep track of what works and what makes what difference. After a while, you will develop a "feel" for these things, which is really no such thing but more like knowledge gained through experience.

[JasonBModerator @jasonb]

The other two things it would be helpful to know is source of the cutter, as a new cheapie may be not better than a part worn decent quality one. Also the type of cut being taken, was it a full width slot as the choice of 2-flute cutter suggests or something else?

[SillyOldDufferModerator @sillyoldduffer]

Posted by mick70 on 30/07/2018 03:15:25:

…as no sound on works computer …

Very often disabled on business computers to stop staff making a nuisance of themselves. However, because training videos and the like need sound, headphone output is typically left on. It's not the law though. Worth a try.

Dave

[SillyOldDufferModerator @sillyoldduffer]

Posted by Hopper on 30/07/2018 03:29:08:

Cutting speeds and feed rates are rules of thumb. In real life, they vary with cutter, material, machine, the direction the wind is blowing etc. Start with the textbook setting as you have done, then experiment on the job. If you think you were feeding too fast, try slowing the feed down. If that does not work, try dropping cutter speed by one speed. Play with it and see what works for you on that machine with that material and cutter.

Change one thing at a time, in smallish increments. That way you can keep track of what works and what makes what difference. After a while, you will develop a "feel" for these things, which is really no such thing but more like knowledge gained through experience.

+1 to that advice.

The appearance of blue chips tells you that the cut is getting hot, between 290 – 320℃.

Getting hot is good, except exactly how hot you can allow a cutter to get without damaging it depends on what it's made of. Roughly:

• Carbon steel loses hardness at about 180℃ : blue chips mean you have trashed the cutter. It's so easy to soften carbon tool steels that nowadays they're used only for wood-turning or special purposes. Before 1910, metal-working lathes used carbon steel cutters, and operators were careful to keep them cool, sharp, and hard. Much time wasted maintaining cutters.
• HSS loses hardness at or just below red heat, say 400 – 550℃. When blue chips appear you might have as little as 80℃ between you and a spoilt tool. Once the temper of HSS is destroyed you can't just touch the edge up on a grinder. In practice most HSS is better than that and blue-chips mean you have about 200℃ in hand before the alloy fails. Uncertainty about the exact temperature at the cutting edge is why some aim for blue chips and others choose to back off slightly. A machine fitted with HSS can cut metal about five times faster than the same machine fitted with tool steel, but it needs a bigger motor and heavier construction to take the strain.
• Carbide has much better heat performance than HSS. Tungsten Carbide at 800℃ is harder than HSS at 20℃. Compared with HSS carbide has superior compressive strength, resistance to burning, and heat conductivity. Not exactly best practice, but a carbide cutter can be pushed hard enough on steel to throw red-hot chips. A machine fitted with carbide can cut metal about ten times faster than the same machine fitted with HSS, but carbide needs abundant power and speed to get best results. I don't recommend making red-hot chips at home. Once the novelty has worn off 800℃ chips flying about are more trouble than they're worth. Blue-chips are less unpleasant.
• There are materials like Boron Nitride that outperform carbide. Harder than glass-hard steels, they would easily slice up an HSS cutter. Never seen any mention of them being used in an amateur workshop!

Blue-chips, or not-quite blue-chips, is a sensible way to judge when a cut in steel is 'about right'. More to it than that. It's also valuable to listen to the cut for signs of chatter, vibration or signs of stress, and to check the finish is OK. Although rules of thumb are helpful, they can't cover individual circumstances, like the rigidity of the set-up, or using a tool that's past it's best. Hopper's advice is spot on.

Dave

[Howard LewisParticipant @howardlewis46836]

You ought to set your feed rate on the basis of "feed per tooth". For an End mill this will be of the order of 0.002" (0.05mm) per tooth, maximum. So for a 4 flute End Mill, you are looking at 0.008" (0.20mm) per rev.

For a 1/2" cutter, to run at 100 ft/min cutting speed, the spindle should be rotating at about 760 rpm. With a maximum 0.002" feed / tooth, this would equate to a feed rate of 6" (150mm) / min for a 4 tooth cutter.

Cutting dry, without coolant, would be likely to call for a decrease in this rate.

Difficult to measure when only manual, and no mechanical feed, is available ; but doable, with practice.

Howard

[Mark BarronParticipant @markbarron78673]

I use an App – Guhring Optimising to calculate required cutter RPM. It's directed toward production machine tools, and for milling only gives options for HSCO and Carbide cutters, but it does speed-up calculating the RPM and is well designed.

Mark.

[JasonBModerator @jasonb]

Mick, as a guide the second video is a 2 flute cutter same as you say you were using, steel is 1" think and it looks to be taking 30 from start of cut to when it breaks through so that is 2" per min feed. Bridgeport should be able to remove a bit more than that.

Quick flick through my IG-1 paper catalogue for a basic uncoated HSS 2-flute cutter in mild steel, cutting a slot 900rpm, Feed 110mm per min, gives 0.061mm per tooth.

[I.M. OUTAHEREParticipant @i-m-outahere]

It could also be the composition of the steel you are cutting , " mild steel " could be anything and if it was just a chunk of black steel lying around the workshop it could be some form of alloy steel . I sometimes pick up some scrap from work that comes off the lifting arms of a garbage truck , 25 – 30 mm thick and around 100mm wide with a mill scale finish . This stuff is not the best to machine but hey its free ! I just use carbide tooling and have at it , the chips are always blue or purple and my biggest concern is making sure the chips are not flying at me ! Try slowing your cutter down a couple f hundres rpm , maybe some brush on cutting fluid and see how that goes – you won't kill a cutter by running it slow provided it is feeding fast enough to make it cut and not rub .

[Author]

Posts