I wanted to do some engraving in timber similar to that shown in the attached image. I needed a bit that could create the vertical faces (sides) in the engraving, therefore it had to be a straight bit, and fit through gaps about 0.025" so I purchased a 0.020"end mill that was make to cut metal! which personally I cannot believe

I set it to cut at the recommended speeds and feeds for Thermoplastic as there was nothing for timber in the data sheet, I set it to cut 0.020"with each pass, as you have probably already worked out it ended badly, I wasn't surprised when the bit broke after a short time. I have pondered the causes of this and settled on the accelleration rate that I used and possibly the CV settings.

I was hoping someone had done a similar thing successfully and may be able to share their settings with me before I make another sacrifice to the bit gods.

I have relinquished to some degree, in that I have enlarged the engraving and bought the smallest straight wood bit I could find being a Amana 46229 DOWN CUT 0.031".

Can anyone help?

Hi,
I use 0.02" endmills for making circuit boards. Yes they are tender...if you don't have the cutting conditions right you will break them.

Basically you spin them as fast as you can, I have a 24000 RPM spindle so I spin them at 24000 RPM.

Next is he feed rate. With small diameter tools like this allow 1% per tooth per rev:
Feed Rate = 0.01 (1%) x 0.02 (diameter) x 2 (flutes) x 24000 (RPM)= 9.6 inch/min
Larger diameter tools, say 0.62", you can get away with 2% per tooth per rev. The 1%-2% is a reflection of the strength of the tool, small tools are weaker
than larger tools. If you attempt to cut at even slower rates all you risk doing is giving the material a 'damn good rub' which work hardens metals rather
than cutting it. Not sure how wood responds but assume if you rub it it gets warm rather than cutting. So I wouldn't go below 1% per tooth per rev
and the strength of the tool precludes you going higher than 2% per tooth per rev.

Next issue is engagement, you are taking 0.02" cuts with a 0.02" tool or 100%. With a slotting toolpath 25-30% engagement is recommended, with an open
toolpath 50-100% is OK. The real issue is that the physical force on the tool is highly dependent on the evacuation of chips. I don't know if you have air
blast but would recommend it. I use flood cooling when making circuit boards mainly for chip evacuation. I can get 15-30 min per tool without cooling but
4 hours plus with cooling. Nothing but nothing ups the load on a tool like recutting its own chips, I don't care what material if you can evacuate the chips from
the cut zone you'll get the best from the tool. If you can't then you break small diameter tools...and I've broken hundreds over the years....chip evacuation and
built-up edge are the two killers of small diameter tools.

To be honest I don't think acceleration settings have a huge role to play.

Craig

Thank you for the info. Im surprised how short the bit life span is without flooding, I assume what you are cutting is a thin layer of copper and some fibreglass, are they carbide bits?

Given you have broken so many bits I'm interested to know what you use the PCB for? I built speakers, amps DAC's & Preamps for fun, so Ivé played with a few PCB's but never made any myself, it's so cheap getting the simple PCB's I have designed made in China that I have bothered and to date the quality has been acceptable.

Obviously I wont be using flooding and I haven't installed an air supply yet, I'll put it on the list, it's a long list though.

The Chip Load Per Tooth in the Amana Feeds and Speeds for Plywood is 0.001 - 0.003, if I use 0.001 at 24000rpm it equates to 48" PM! My plan is to slow down the rpm and slow down the cutting while maintaining the 0.001 Chip Load. This is for 1 X Diameter depth but I will reduce the depth to 50% and see how it goes.

If you're up for it I'd still be interested to know what you CV & Accelleration settings are.

Many Thanks
David

Hi,
my PCBs are for various uses. The one which is difficult to make and very very expensive if I were to have it made for me is a heavy copper board,
the copper layer is 420um thick (0.42mm). That is 12 times thicker than normal. You can get them etched but double side boards with heavy vias
can cost $1000 per sq foot.

I have broken a lot of tools trying to make theses boards but am getting the hang of it now. When I go back and count the number of small endmills (16 thou
and 20 thou) I have not in fact broken hundreds, about 60 over three years.

They are carbide tools and the trick is to cut the barest minimum of fiberglass as it dulls tools big time. I use a software tool called Autoleveller to assist cutting
the barest minimum I have to.

Don't slow the tool down, spin it as fast as you can. If you are using inches the .001 (1 thou) chip load is too much.

My post recommends 1% of diameter....0.01 (%)x 0.02 (diameter)=0.0002    read that again...that is two tenths of a thou. What you are proposing (1 thou) is
five times what I'd recommend. You will break it for sure.

For a slotting toolpath the depth of cut should be 25% of the diameter. Slotting is very challenging, if you try to slot full depth in one pass you will break tools
or I certainly did. I also reduce the feed rate to half when slotting and reduce plunging to a quarter.

My wee mill has low lash (less than 2 arc min) planetary reduction boxes on the steppers and so the rapids are slow (1200mm/min) but the accelerations are high
(375mm/sec/sec). Quite frankly CV and accel mean squat when trying to establish the correct conditions for long tool life with these micro tools, its about matching
the chip load to the strength of the tool and clearing chips to reduce the torque drag. About half the breakages I've suffered are due to the spindle twisting the tool
off. The other half is where the feed over runs the cutting ability and snaps it off sideways.

Craig

Craig

I did run your figures and they worked out at approx 11.5" @ 24000 but I am cutting softish wood not copper so I thought it reasonable to follow the conservative side of the Amana recommended S&F and reduce the depth by 50%. My CNC has a 2.2kw spindle and if I dont need to run it flat out I'd rather not.

Thanks for the help.

Hi,
you realize that even at 24000 RPM the surface speed is only 0.02 (diameter) x pi x 24000 (RPM) / 12 (inches to ft)= 125.7 ft/min, ie very low.
There is a reason that commercial machines which run micro tools have air bearing spindles doing 60000-120000 RPM.

Craig

Hi,
just found my speeds and feed calculator (HSM Advisor) recommends 906 ft/min for uncoated carbide tools in softwood,
would require a spindle doing 180,000-190,000 RPM with a 0.02" tool!!!

What surface speed does your database/calculator recommend?

Craig

Hmmm, this is confusing, the Amana data sheet says to calculate SFM you; "To find SFM: 0.262 x diameter of tool x RPM" their data sheet is based on 18000RPM, therefore it's 0.262 x 0.031 x 18000 = 146.196 SFM

But when I enter the the speeds and feeds into Fusion CAM to get 0.001 chipload I end up with 64.9262!

I'll have to admit I have never been certain that I am doing this feeds and speed stuff correctly.

When I changed Fusion S&F to achieve 146 SFM I get a "Feed Per Tooth" of 0.000444444" I have assumed Feed Per Tooth is the same as Chipload?

I'm using cutter 46229 from the attached Amana data sheet


 

Hi,
that formula is the same, they have combined pi and divide by 12 in the constant.

0.262 x 0.02 x 18000 = 94.32 ft/min
pi x 0.02 x 18000 / 12 = 94.25 ft/min

So this is the actual surface speed given the diameter and rpm but not the recommended target surface speed based on material and tool type.
But 94 ft/min is way way slow. What does the database recommend for surface speed with an uncoated carbide tool in various materials?
My database says 906 ft/min for softwood and uncoated carbide, 10 times what you've calculated.

Craig

I dont have a data base only the data sheet I attached