1mm bit broke off at start of mill

Hi,
I'm using this setup:

Material: 3mm plywood with 6mm wasteboard.
End mill : 1mm, 2-flute
Pass depth: 0.3mm
Stepover: 0.1mm (10.0%)
Spindle Speed: 15000 r.p.m
Feedrate: 25.0 mm/sec
Plunge Rate: 10 mm/sec

This is part of a 2-toolpath file, but it broke off after a few seconds making a small hole. My passes were 0.3/0.9/1.5/2.1/2.7/3.1, so 6 passes in total for a 3mm thick board.

My Pocket Toolpath was a "Raster, Climb, Last", with all other settings default.

I think there are a few reasons why the break happened:

1 - the plywood was "bending" up a bit because it was being pulled by the bit, and that distorted movements in XY.

2 - some of the settings didn't match the bit capabilities in terms of overload

3 - other reason i'm not thinking of.

Any ideas to determine the reason for the bit breaking off?
It broke off the cutting part of the bit, while the Shank stayed inside the collet..

Thanks!

I guess that your feed rate is too high for tiny 1mm bit.
Check here: FSWizard
For such bit you should ramp into material, not plunge.

Hi,
I use 0.4mm and 0.5mm two flute endmills for making circuit boards.

You need to spin those small endmills as fast as you can, 24000 would be better, 30000 would be better again.

Small endmills are very tender, they have very little cross sectional area and then the two flute are ground into it reducing
the core cross section even more.

I work out my feed rate by assuming a 1% chip load per tooth.

Thus in each rotation I expect the tool to advance ( feed rate) by 1% of the tool diameter per tooth.
with a two flute 1mm diameter tool:

advance/per rev= 1 (mm) x 0.01 ( 1%) x 2 (two teeth)
=0.02 mm/rev

At 15000 rpm
feed rate (mm/min)= 15000 x 0.02
=300 mm/min or 5 mm/second.

Zasto suggests your 25mm/second feed rate is too high, my calculation suggests that also.
Note that if you could spin your tool at 30000 rpm you could double your feed rate as well and that's why I recommend spinning these small
endmills as fast as you can.

Craig

Hi,
Thanks Craig and ZASto for your help!

Since I didn't have another 1mm bit, I switched to a 2mm one, with the following settings:

End mill : 2mm, 2-flute
Pass depth: 1 mm
Stepover: 0.4mm (20.0%)
Spindle Speed: 25000 r.p.m
Feedrate: 10.0 mm/sec
Plunge Rate: 5 mm/sec

It is working fine :)
The feedrate was probably the issue, but I also added a "Ramp Plunge" of 6mm to be safe.

Hi,
if you want small diameter endmills:

https://www.ebay.com/str/carbideplus

They stock Kyocera Tycom, so a quality brand at very good prices. I've bought hundreds of them over the years.

Craig

Follow up question:

If I want to mill a 50mm thick wood piece, with a 'roughing' pass, using an 8mm bit, are these settings okay? :

End mill : 8mm, 2-flute
Pass depth: 4 mm
Stepover: 1.6mm (20.0%)
Spindle Speed: 25000 r.p.m
Feedrate: 25.0 mm/sec
Plunge Rate: 10 mm/sec

Or perhaps the feed rate isn't too accurate here? I don't know how much % chip load to assume in this kind of setup, cause according to a calculation of 1% I can go up easily up to 50mm/sec feedrate...
I don't know what that means in terms of heat on the wood or the bit or any other results...

Would appreciate your insights.
Thanks :)

Hi,
with small diameter tools you want to spin them very fast. Larger diameter tools need to be slower.

What you are trying to do is match the surface speed of the tool to the material.

Surface speed m/min= diameter (m) x PI x RPM
= 0.008 x 3.141 x 25000
=628.2 m/min.

That is probably OK for a carbide tool in wood.
For carbide in aluminum the surface speed will need to be 200-500m/min depending on cooling and chip evacuation. 8000-20000 rpm
The same tool in mild steel the surface speed will need to be 100m/min. 4000rpm

Craig

Hi yafimski,
Try to use FSWizard.
It will give you rough estimates/starting points about your feeds/speeds. You can change almost any parameter in that wizard.
I'm by no means a machinist, but what I've learnt over time is that every material has it's "sweet spot" of surface cutting speed. That is always my starting point in calculations.

Hi,
I liked HSM Advisor so much I bought it.

https://hsmadvisor.com/

Craig