[sooncheng]

I'm new to CNC. Recently I was trying to machine a 1mm, 120mm long with DOC of 0.5mm with a 1mm end mill. I'm running this on a 3-axis VMC.

Tool: 1mm carbide 4 flutes with TiSiN coating (claimed by the seller)
Material: Mild steel

First trial: 3500rpm, 15mm/min and the tool broke halfway. Inspected the end mill and it seems like the speed is too high causing the tool to heat up, the end appears dark and burnt.

Second trial: 2000rpm at 20mm/min, tool looks OK when I paused the machine to inspect but still broke.

Coolant was used on both trials.

I've used G-Wizard to get an idea on the speed and feed, it says that my chip load is too low and may cause rubbing, maybe this is the culprit? or I'm just not dialing the speed and feed correctly.

Thanks

[joeavaerage]

Hi,
I use small (0.4-0.5mm) endmills to make circuit boards. They are tender.

With a coated carbide tool you should be looking at 100m/min surface speed.

1mm x 2 x Pi= 6.3mm (tool circumference)

100m/min =100,000 mm/min
100,000 / 6.3 =15900 rpm

I don't know where you are getting your speeds from but I would be running a 1mm tool at 16000 rpm.
On small tools I allow 1% of tool diameter per flute per revolution as chip load at 10% engagement.
At 0.5mm DOC and full width that works out to 50% engagement so you would decrease the feed rate
by 4/5.

If you are slotting, halve that. Slotting is a difficult task....do you have to slot? Better a 50% step over.

0.01 X 1mm x 4 x 16000 = 640mm/min

To allow for 50% engagement:
640 x 1/5 =128mm/min, and if you have to run a slotting toolpath halve it to 64mm/min.

Cooling s good but more important is to use the coolant to flush the chips out of the cutzone, re-cutting chips is a sure
way to break tools. Flushing chips out of a slot is really tough....try whatever means to avoid a slotting toolpath.

Craig

[sooncheng]

Hi Craig,

Thanks for the information.

First of all, I don't actually prefer coolant because it makes the machine messy and I'm not able to see the progress when machining small parts, I did use coolant mainly too flush off chips, two nozzles pointing directly on the bit should be good enough.

Can I still run at 100m/min on mild steel? I know I should be looking at 100m/min, I've tried it and the result was lots of chatters, heat and vibration (I was using 10mm flat end mill from same vendor, but this tells me that their tool can't run at 100m/min on mild steel, 25m/min instead). So a quick question here, if my tool vendors suggest that I should run 100m/min on a certain material, can I run it lower?

Unfortunately, I'm slotting here and I can't avoid that, I attached a photo of the part I'm working on, I'm trying to machine the three slots and the teeth. Their depth/size can change, 0.2mm~0.5mm for the slots is good.

Also, the maximum spindle speed my machine can run is 10000rpm, what should I do about it?

[burbingus]

Rather than running a straight slot, I feel like you might be better off using a slightly smaller end mill (1/32 in) and doing a high speed trochoidal style tool path. What is your feed per tooth? I think 0.0001 inch per tooth is approximately what you should be aiming for. I wouldn't worry about your spindle RPM directly - I would run it a reasonable speed (~75% of max) and calculate your speed based on your feed per tooth.

[burbingus]

This is a good article by the way on feeds and speeds:

https://www.harveyperformance.com/in...and-feeds-101/

[sooncheng]

Rather than running a straight slot, I feel like you might be better off using a slightly smaller end mill (1/32 in) and doing a high speed trochoidal style tool path. What is your feed per tooth? I think 0.0001 inch per tooth is approximately what you should be aiming for. I wouldn't worry about your spindle RPM directly - I would run it a reasonable speed (~75% of max) and calculate your speed based on your feed per tooth.

Thanks for the reply! It's a good idea to use trochoidal milling. I'm actually not sure about what feed per tooth to use, but now I'm running it on 0.002mm per tooth (0.00008 inches approx). Can I run it at 1000~3000 RPM and adjust the other parameter accordingly? Because that's the speed I'm comfortable with right now.

[joeavaerage]

Hi,
messy or not, use coolant.

Run at max rpm. the feed rate calculation remains the same. 1% of tool diameter per flute per revolution.

0.01 x 4 x 10,000=400mm/min

Reduce this because you are using 50% engagement and reduce it again because you are slotting.

400 x 1/5 (engagement) x1/2 (slotting)=40mm/min

Craig

[Jim Dawson]

When cutting slots as you show in your drawing, I would use a slitting saw. An endmill would work, but more trouble than it's worth. Normally when I need to use tiny endmills, I install my air spindle and run them at high speed.

[sooncheng]

Hi,
messy or not, use coolant.

Run at max rpm. the feed rate calculation remains the same. 1% of tool diameter per flute per revolution.

0.01 x 4 x 10,000=400mm/min

Reduce this because you are using 50% engagement and reduce it again because you are slotting.

400 x 1/5 (engagement) x1/2 (slotting)=40mm/min

Craig

Max RPM isn't a very comfortable speed for me, can I run it at a lower speed?

[sooncheng]

When cutting slots as you show in your drawing, I would use a slitting saw. An endmill would work, but more trouble than it's worth. Normally when I need to use tiny endmills, I install my air spindle and run them at high speed.

I will consider a slitting saw for this. Thanks.

[joeavaerage]

Hi,

Max RPM isn't a very comfortable speed for me, can I run it at a lower speed?

Yes you can run at lower speed but you will have to reduce feed rate as well otherwise each chip will be too big and you will 'over torque'
your tool and twist it off like a carrot.

You don't like messy...you don't like uncomfortable....are we talking CNC or are we talking sun bathing?

Craig

[sooncheng]

Hi,



Yes you can run at lower speed but you will have to reduce feed rate as well otherwise each chip will be too big and you will 'over torque'
your tool and twist it off like a carrot.

You don't like messy...you don't like uncomfortable....are we talking CNC or are we talking sun bathing?

Craig

I get what you mean, I was running at 1300rpm 15mm/min, 0.003mm/tooth, 0.2mm doc yesterday, do these numbers look good for you? or they are too low. I don't need high speed. Might try 10000rpm at 40mm/min.

Thanks

[number40Fan]

Why does the high speed scare you? I run a 6mm two flute in aluminum at 16k without coolant until the finish pass.

[joeavaerage]

Hi,
high speed...low speed means what exactly?

It really refers to the surface speed, that is to say the speed that a cutting tooth is forced through the material being cut.

Each material has its own properties and each tool has its own properties as well.

As a rule of thumb with a coated carbide tool in mild steel the surface speed should be 100 m/min.
Tough steels like 300 series stainless that reduces to 75m/min.
Titanium and Super alloys it reduces further to 40-50 m/min.

Aluminum can be cut with uncoated carbide tools at 250m/min and if you have di-boride coated carbide that can be pushed out to
500m/min. Copper cuts nicley with uncoated tools at 150-250m/min.

If you use HSS tools then all of the numbers above should be reduced by nearly a half.

Whether you use HSS or carbide, coated or otherwise they all cost. You really should try to get the best from them.

If you run them too fast, lets say you have a really highspeed spindle and you decide to run at 200m/min in steel you'll
turn the tip of the tool red hot within seconds and the tool will be wrecked and no cutting done. It doesn't matter that you take light cuts
it the SURFACE SPEED that determines the rate of heat generated, if you try to go too fast you'll fry the tool. If you try it
in aluminum you'll get 'built up edge' (BUE) and that wrecks the tool and the surface of the job too.

Much of the research into cutting tools and coatings is to increase the surface speed at which a given tool can be used in a particular
material. For instance I would reduce the surface speed to 85m/min with uncoated carbide in ordinary mild steel whereas I would run at
100m/min if the tool were coated. If the steel were free cutting and/or the tool geometry is such that the heat of cutting is carried away with
the chips then you might be able to push it out to 125 or even 150m/min. All of that is big potatoes to manufacturers.

As for going slower, yes that can be done but the tool wear does not reduce linearly as well.

Lets say I get three hours life from a coated tool at 100m/min in steel. If I reduce rotational speed to 50 m/min does the tool last twice as long...
no it does not. It will last longer but for a given amount of material to be turned into chips the rate of tool wear is increased per kg of chips
at slower speeds.

As I posted earlier I use 0.4mm and 0.5mm two flute endmills for prototyping circuit boards. With careful depth control I endeavor to cut
the thin copper layer on top and as little of the underlying fiberglass as I can. I would like to cut at surface speed of 200m/min, but I can't.
Follow the calculation:

Tool diameter, D, =0.5mm
Tool circumference,TC= Pi x D =1.57mm or 0.00157m

To have a surface speed, S, of 200m/min requires:
Revolutions per minute, rpm,= S / TC
=200/0.00157
=127,300 rpm

My spindle can only do 24000 so I have to run the tool sub-optimally. An air bearing spindle that can do 125000 rpm is way out of my league.

OP wants to cut steel with a coated carbide tool so an surface speed of 100m/min is indicated:

D=1mm
TC=3.141mm or 0.00314m
R=100 / 0.00314
=31,850 rpm (please note this calculation is correct, my earlier post where I calculated 15,900 rpm is wrong, its one half of what it should be)
To OP, run your 1mm tool at the highest possible rpm you can, anything less is just wasting your tool life.

If OP wanted to use a 6mm tool (coated in mild steel):

D=6mm
TC=18.84mm=0.01885m
R=100 / 0.01885
=5300 rpm.

Note how sensitive the required rpm is to tool diameter.

number40Fan runs a 6mm tool at 16000 rpm in aluminum:
S= R X TC
= 16000 X 0.006 X PI
= 301m/min which is right in the sweet spot for aluminum, I prefer coolant at that speed but you can get away without it.

This highlights how required rpm is sensitive to the material being cut, soft metals like aluminum, copper and brass can all be cut at 200m/min plus.
Steels at 100 m/min. Stainless at 75m/min. Titanium at 50m/min.

Once you've done the calculation and established the best possible surface speed you can THEN consider the feed rate.

Small diameter tools are weak...they have a very small core and consequently are easy to break by being overloaded.

One strategy is to reduce the feed rate and therefore take very thin chips. This has a draw back, especially in work hardening materials
like stainless, and heaven forbid should you try it in pure nickel, that all that happens is you give the material 'a good rub' and work harden
the surface making it even harder for following teeth to cut.

The key here is to take a reasonable 'bite' at the material, with small tools 1% of tool diameter per revolution per tooth.
For OPs 1mm tool that is 0.01 x 1= 0.01mm, or with four flutes 0.04mm per revolution and at OPs max 10000rpm= 400mm/min
feed rate. That will avoid the problem of 'giving it a good rub' and work hardening the material but now you almost certainly will
overload the tool and so have to take shallow cuts.

Shallow cuts means that the tips of the tool does all the work and when they are blunt you have to throw the tool away despite the rest
of the flanks of the tool not having been touched. Its a compromise, you may reduce the feed rate a bit but take deeper cuts to
get a better result.

For instance when I cut heavy copper board, by heavy I mean a thick, even very thick, for circuit boards, layer of copper 0.42mm thick.
The first slotting pass I take only 0.21mm and get the next 0.21mm in the next pass. Because its a slotting toolpath I have the feed rate
set to only 240mm/min. Thereafter I have a 50% step over, so that is 0.25mm wide cut but full depth of 0.42mm and I take that at 420mm/min.
With coolant to flush away the chips out of the cutzone I can get 8-10 hours cutting from one 0.5mm tool. All in all I find that this fairly
aggressive cutting style is best, a tool should 'work for its living'......babying them seldom works, they seem to get blunt just as fast, and with small
tools it usually as a mistake in tooplath or handling/jogging that breaks them and that happens irrespective of whether you choose an aggressive
cutting plan or not.

Craig

[sooncheng]

Hi,
high speed...low speed means what exactly?

It really refers to the surface speed, that is to say the speed that a cutting tooth is forced through the material being cut.

Each material has its own properties and each tool has its own properties as well.

As a rule of thumb with a coated carbide tool in mild steel the surface speed should be 100 m/min.
Tough steels like 300 series stainless that reduces to 75m/min.
Titanium and Super alloys it reduces further to 40-50 m/min.

Aluminum can be cut with uncoated carbide tools at 250m/min and if you have di-boride coated carbide that can be pushed out to
500m/min. Copper cuts nicley with uncoated tools at 150-250m/min.

If you use HSS tools then all of the numbers above should be reduced by nearly a half.

Whether you use HSS or carbide, coated or otherwise they all cost. You really should try to get the best from them.

If you run them too fast, lets say you have a really highspeed spindle and you decide to run at 200m/min in steel you'll
turn the tip of the tool red hot within seconds and the tool will be wrecked and no cutting done. It doesn't matter that you take light cuts
it the SURFACE SPEED that determines the rate of heat generated, if you try to go too fast you'll fry the tool. If you try it
in aluminum you'll get 'built up edge' (BUE) and that wrecks the tool and the surface of the job too.

Much of the research into cutting tools and coatings is to increase the surface speed at which a given tool can be used in a particular
material. For instance I would reduce the surface speed to 85m/min with uncoated carbide in ordinary mild steel whereas I would run at
100m/min if the tool were coated. If the steel were free cutting and/or the tool geometry is such that the heat of cutting is carried away with
the chips then you might be able to push it out to 125 or even 150m/min. All of that is big potatoes to manufacturers.

As for going slower, yes that can be done but the tool wear does not reduce linearly as well.

Lets say I get three hours life from a coated tool at 100m/min in steel. If I reduce rotational speed to 50 m/min does the tool last twice as long...
no it does not. It will last longer but for a given amount of material to be turned into chips the rate of tool wear is increased per kg of chips
at slower speeds.

As I posted earlier I use 0.4mm and 0.5mm two flute endmills for prototyping circuit boards. With careful depth control I endeavor to cut
the thin copper layer on top and as little of the underlying fiberglass as I can. I would like to cut at surface speed of 200m/min, but I can't.
Follow the calculation:

Tool diameter, D, =0.5mm
Tool circumference,TC= Pi x D =1.57mm or 0.00157m

To have a surface speed, S, of 200m/min requires:
Revolutions per minute, rpm,= S / TC
=200/0.00157
=127,300 rpm

My spindle can only do 24000 so I have to run the tool sub-optimally. An air bearing spindle that can do 125000 rpm is way out of my league.

OP wants to cut steel with a coated carbide tool so an surface speed of 100m/min is indicated:

D=1mm
TC=3.141mm or 0.00314m
R=100 / 0.00314
=31,850 rpm (please note this calculation is correct, my earlier post where I calculated 15,900 rpm is wrong, its one half of what it should be)
To OP, run your 1mm tool at the highest possible rpm you can, anything less is just wasting your tool life.

If OP wanted to use a 6mm tool (coated in mild steel):

D=6mm
TC=18.84mm=0.01885m
R=100 / 0.01885
=5300 rpm.

Note how sensitive the required rpm is to tool diameter.

number40Fan runs a 6mm tool at 16000 rpm in aluminum:
S= R X TC
= 16000 X 0.006 X PI
= 301m/min which is right in the sweet spot for aluminum, I prefer coolant at that speed but you can get away without it.

This highlights how required rpm is sensitive to the material being cut, soft metals like aluminum, copper and brass can all be cut at 200m/min plus.
Steels at 100 m/min. Stainless at 75m/min. Titanium at 50m/min.

Once you've done the calculation and established the best possible surface speed you can THEN consider the feed rate.

Small diameter tools are weak...they have a very small core and consequently are easy to break by being overloaded.

One strategy is to reduce the feed rate and therefore take very thin chips. This has a draw back, especially in work hardening materials
like stainless, and heaven forbid should you try it in pure nickel, that all that happens is you give the material 'a good rub' and work harden
the surface making it even harder for following teeth to cut.

The key here is to take a reasonable 'bite' at the material, with small tools 1% of tool diameter per revolution per tooth.
For OPs 1mm tool that is 0.01 x 1= 0.01mm, or with four flutes 0.04mm per revolution and at OPs max 10000rpm= 400mm/min
feed rate. That will avoid the problem of 'giving it a good rub' and work hardening the material but now you almost certainly will
overload the tool and so have to take shallow cuts.

Shallow cuts means that the tips of the tool does all the work and when they are blunt you have to throw the tool away despite the rest
of the flanks of the tool not having been touched. Its a compromise, you may reduce the feed rate a bit but take deeper cuts to
get a better result.

For instance when I cut heavy copper board, by heavy I mean a thick, even very thick, for circuit boards, layer of copper 0.42mm thick.
The first slotting pass I take only 0.21mm and get the next 0.21mm in the next pass. Because its a slotting toolpath I have the feed rate
set to only 240mm/min. Thereafter I have a 50% step over, so that is 0.25mm wide cut but full depth of 0.42mm and I take that at 420mm/min.
With coolant to flush away the chips out of the cutzone I can get 8-10 hours cutting from one 0.5mm tool. All in all I find that this fairly
aggressive cutting style is best, a tool should 'work for its living'......babying them seldom works, they seem to get blunt just as fast, and with small
tools it usually as a mistake in tooplath or handling/jogging that breaks them and that happens irrespective of whether you choose an aggressive
cutting plan or not.

Craig

Thanks for the detailed explanation. I broke my last 1mm end mill couple days ago by accident, they are very fragile. I will update here when they arrive.

[hpappsguy]

Forgive me if this was already mentioned, but your toolholder runout needs to be absolutely precise for that tool, in that cut, to improve life. Your target is 0.0001" (.00254mm) TIR at 4 x Diameeter. We see this in small diameter tools all the time. Going from 0.0006" (0.01524mm) runout to 0.00254mm is the equivantel of 45-60% tool life decrease.

Also, that tool has virtually no cross-sectional strength to withstand tool deflection so you shipload is extremely critical. joaverage calculates the circumference incorrectly. Circumference = 2(Pi)r, not 2(Pi). Therefore his RPM recommendation, all things being equal, is off by 1/2. Your 24K spindle should be maxed out. and your feed should be adjusted. I do agree with joeaverage that you should be backing off all your parameters by 20-25% on account that this is a full slot, and under normal conditions, 1% of diameter feed per tooth will get you in the ballpark (less 20-25%)

Finally, how much tool projection do you have sticking out? you could be incorporating unnecessary length, which yield catastrophic deflection in the tool, especially as it dulls, and can't keep up with the feed. That tool should be sticking out of the holders no more than is required for the spindle to clear any obstacle. If there is no obstacle, then you should be running with a tool projection as short was the tool shank will allow.

[hpappsguy]

I just referenced our job history. I'm in the US, so I am not current of your steel grade references, but in "low carbon" steel (1018, 1020, 4140 here in the US) we run that with a 4-flute tool, with modern coating, at:

75 - 107 M/Min Surface speed (stay on the low end here since I don't know what geometry)
75M/min = 23854 RPM
Feed per Tooth: 0.00044mm PER TOOTH (don't go above 0.005 mm/PT, and don't start below 0.0040mm PT
Feed per minute = 458.016 mm/min (assuming 0.0048mmPT, 74 M/min)

The feed has bee pre-adjusted for slotting conditions.

Again, runout and tool project are very important here. As short as possible, as concentric as possible.

You were rubbing the tool to death in your first 2 attempts, almost certainly. When your chip load is too low, not only will you build up heat, but your cutting edge will push off the material rather than bitting, so your effective shipload was actually much less than what you programmed. As you feed into the part, the end mill gradually falls behind and can't keep up, causing the carbide to break from excess deflection.

[annlia]

<a href="https://www.google.com">hai</a>
https://www.google.com
www.google.com
<a href="https://www.google.com">hai</a>
https://www.google.com
www.google.com
nice!
"hai":https://www.google.com
[create debates!](http://createdebate.com)

[sooncheng]

I used cheap ER32 collet with BT40 holder, TIR was around .05mm haha will using smaller collet and holder gives better runout (like ER16 collet, I prefer collet system because I have to change my tools quite often)

I think I had around 12mm stick out which was the minimum I can get before clamping on the coated surface of the tool (can I actually clamp on the coated part of the tool?)

Cheng

[joeavaerage]

Hi,

Circumference = 2(Pi)r, not 2(Pi)

circumference = 2 x PI x r r=radius
circumference = PI x d d=diameter

tool diameter =1mm therefore circumference = 1.0 X PI=3.141mm

Craig