[samy0515]

Hi, I am completely new in machining, and I am hoping to ask some questions.

Currently, I am trying to do a profile cut on a thin plate of plastic (70x30x2.5mm). Originally, we were using laser cutters to cut the piece, but this no longer became an option. Sending it to a machinist was too expensive as we need to make 100~200 cuts throughout the year.

Fortunately, the university I work at had a CNC milling machine that nobody was using, so I am hoping to use it to make these cuts.

The mechanical property of the material is close to acrylic. I am trying to cut tensile test samples for research.

What kind of endmills (or any other bits) are recommend? Also, is there anything specific that I should keep in mind? I have maybe ~2 hour of machining experience from my undergrad days, so any tips will help.

[joeavaerage]

Hi,
I machine small parts out of plastics regularly. Acteal is my preferred material as it forms chips. Surprisingly Teflon cuts nicely too, it is soft, but forms chips rather than strings
and leaves a silky-smooth finish....just the ticket for epoxy molds.

ABS and polyethylene are probably the worst. ABS for its heat sensitivity and polyethylene because it forms long strings rather than chips.

Acrylic is heat sensitive, but it does form chips so is overall not too bad. I use flood cooling, and I think you will have to as well. Any heat build up
in the material or tool or chips will see the chips weld themselves to the tool and wreck the job. You must absolutely flush the chips out of the cut zone the moment they are formed
otherwise you will get Built-Up-Edge.

I use small tools, typically 0.5mm two flute, up to 3mm four flute, almost all of them are Kyocera Tycom.

Truth is that you don't really need coated tools, just well ground plain carbide is quite adequate. Once you have used the same tool in metals or fiberglass its usually sufficiently dull
that while it will still cut acrylic you get a poor finish. With a new Kyocera Tycom tool, I can get a near optically transparent finish.

https://www.ebay.com/str/carbideplus....m47492.l74602

I aim for 225m/min surface speed, but with small tools that means really high speeds (1.5mm spins at 47krpm for 225m/min) and yet my spindle is tapped out at 35krpm.
Feed rate is determined by the strength of the tool. 0.5mm tools are very tender, and you must go fairly slow or you'll snap it. Yesterday I engraved some lettering in cast
aluminum with a slotting toolpath DOC of 0.25mm with a 0.5mm two flute tool at 30krpm under coolant. I chose to be conservative so called for 100mm/min and 50mm/min plunge.
Turned out very nicely and could probably be a lot more aggressive with feeds....but then again I've still got the tool for another day, I did not break it, and that is an all too frequent occurrence
with 0.5mm tools.

Craig

[joeavaerage]

Hi,
in small diameter tools, 3mm and smaller I prefer four flute, as the core of the tool is stronger. You can get four flute down into very small sizes but the price goes through the roof.

My budget allows for four flute at 0.8mm, 1.0mm, 1.5mm and above, but below that I get two flute. Note that it is at the smallest sizes that core strength is most important, so
it may be that my budget-mindedness is counting against me.

This is typical for a two flute 0.5mm tool; $4.50USD This seller had them on special about three-four years ago for $2.65USD each and so I bought 30 of them. Still using them, down to 16 left,
including the one in the tool holder.

https://www.ebay.com/itm/151724700078

Whereas this one is only fractionally bigger (0.533mm) but four flute (coated) but the same manufacturer (Kyocera Tycom) but see how the price has doubled:

https://www.ebay.com/itm/385393957722

I suppose if you get twice the life from the four flute tool it makes sense, but otherwise the increase in cost makes my anus pucker!!!
Really tool life in these small diameter tools is about when you break them rather than when you wear them out. I have over the years gotten better at not breaking them, but still do not get
to actually 'wear them out' as often as I would like.

If you are through cutting the I'd suggest 1.5mm four flute tools, leaves a small fairly small kerf. Do not get over long tools, they flex and break. Try these:

https://www.ebay.com/itm/155071505135

I buy 30 to 40 of these a year. They get used on plastics, brass, aluminum and even steel. They are long enough (5mm flute length) to be useful and yet short enough and four flute
to be reasonably rugged. I've literally used hundreds of these things!

Manufacturers terminology changes but by in large stub length means 1.5X where X is the tool diameter. Thus a 1.5mm stub length tool will have a flute length of 2.25mm. Whereas
standard length tools are 3X to 5X (4.5mm to 7.5mm) and long tools are 10X and higher. The shorter the tool the stronger and more forgiving it is.

Craig

[awerby]

I prefer single or 2-flute cutters for plastics and other soft materials, because they clear chips better than 4-flute cutters, which I use for things like steel. If you're cutting thin sheets, I'd suggest a down-cut spiral, since it has less tendency to lift the material. For heat-sensitive plastics, consider an air chiller, like the Vortex: https://www.exair.com/products/cold-...t-systems.html

[joeavaerage]

Hi,
the problem with down-cut tools is that they exhaust chips into the bottom of the cut where they are highly likely to be re-cut.

Single and two flute is fine for tools say 3mm and above, but at small diameters the cost of core strength is too high relative to the better chip clearance.
What the point a of a single flute 1mm tool that breaks as soon as you look at it verses a four flute tool that lasts for many months other than by breakage?

Craig

[unitedmetallaser]

Hi there! Welcome to machining—great to see you diving into CNC work.

For plastics similar to acrylic:
- Single-flute endmills are ideal to minimize heat buildup.
- Use sharp cutting edges designed for plastics to avoid melting.
- Keep spindle speeds low and feed rates high to prevent heat issues.

Secure the material well, and use compressed air to clear chips and keep the cut cool. Testing on scrap first is always a good idea.

If laser cutting becomes an option again, check out United Metal Laser in Malaga—they offer precise, cost-effective services for projects like yours.

Explore more on our website: https://www.unitedmetalslaser.com.au/

Good luck, and feel free to ask more questions!