Engraving/machining acrylic

[andy_con]

been trying to engrave some clear acrylic to make an led sign for a friend, but its not been going as well as id like.

first tried a 1mm end mill, 22000rpm, 0.5mm DOC and 500mm/m. acrylic just melted and stick to the cutter and produced a poor finish.

I then tried a 4mm spot drill, 0.25mm DOC, 22000rpm and 300mm/m. started off very well with a perfect finish then after a while the acrylic melted and stick to the spot drill and gave a crap finish.

I then tried an 8mm spot drill, 0.25mm DOC, 22000rpm 300mm/m. went ok for about 30 seconds then acrylic melted and stick to the spot drill.

so decided 4mm spot drill was giving best results and played around with a few different feed rates, I can get good results but then every time after a few mins of cutting the acrylic melts and sticks to the end and causes a shit finish.

anyone got any tips?

[Clive S]

anyone got any tips?
The little bit of acrylic that I have done was using a lot higher feed rate than 300mm/min so I would do some tests at say 2-3 mtr/min. There are people on here that do cut that stuff though and hopefully will chime in.

[cropwell]

I have had reasonable results using lots of air to clear chips and WD40 or Fixt spray to keep the cutter lubricated and cool. A sharp carbide single flute cutter with open architecture (lots of space in the spiral, to allow chips to get out of the way) helps. You also need to make chips that take the heat away, not rub the plastic.

[Boyan Silyavski]

been trying to engrave some clear acrylic to make an led sign for a friend, but its not been going as well as id like.


welcome to the world of plastics :hysterical:


I don't remember right now what machine you had, but plastics melt if machine is not rigid or if you push cutter so it passes some minimum deflection. Plus they need constant air cooling. Or one flute cutters. But could be done without melting if you don't dig deep.

V cutter is not same as spot drill, but anyways. At least it must be very sharp. That's a rule for plastics. New and sharp! Try 0.025mm chip load and 0.1-0.2mm pass. It would help if you file a bit that tip flat. say 0.4- 0.6mm at least. Cause you know there starts the burning. Not digging deep means you could pass without any cooling at all.

[magicniner]

A sharp carbide single flute cutter

+1 to this, also the single flute cutters are easy to sharpen with a little practice.
I made some covers for Theoben airgun magazines in acrylic and flame polished the inside (machined) surface to achieve good transparency,

- Nick

[cropwell]

the single flute cutters are easy to sharpen with a little practice. - Nick
Never had one go blunt, had plenty of the feckers snap though! :culpability:

[andy_con]

thanks for all the info

I have a denford micro router, which is enclosed. I did wonder if things in general were getting hot yesterday, it was a hot day and once I closed the door of the router there is no air movement inside.

how small can you get single flute cutters? I want to engrave so didn't want to go any bigger than 1mm really

[A_Camera]

been trying to engrave some clear acrylic to make an led sign for a friend, but its not been going as well as id like.

first tried a 1mm end mill, 22000rpm, 0.5mm DOC and 500mm/m. acrylic just melted and stick to the cutter and produced a poor finish.

I then tried a 4mm spot drill, 0.25mm DOC, 22000rpm and 300mm/m. started off very well with a perfect finish then after a while the acrylic melted and stick to the spot drill and gave a crap finish.

I then tried an 8mm spot drill, 0.25mm DOC, 22000rpm 300mm/m. went ok for about 30 seconds then acrylic melted and stick to the spot drill.

so decided 4mm spot drill was giving best results and played around with a few different feed rates, I can get good results but then every time after a few mins of cutting the acrylic melts and sticks to the end and causes a shit finish.

anyone got any tips? I use V-bits to engrave, but when I am milling acrylic I am using single flute bits. Feed rate depends on the type and diameter of the mill bit and the DOC. My current crappy DC motor I have as spindle is running at 9000 RPM and the feed rate for engraving with V-bits is normally around 300mm/min. Milling with 2, 3 and 4mm end mills I normally run with 500-900mm/min feed rates.

So my advise for you is to use single flute end mills and V-bits for engraving and reduce the spindle speed by 50% and keep everything as it is. If you still experience melting then reduce the spindle speed even more and find an optimal speed when melting stops. Once you found that you can increase feed rate and spindle speed.

Remember that the 0.25mm DOC is more like shaving than cutting material, the chips are very thin and can not transport away the heat very efficiently. Use a vacuum cleaner to keep the surface clean to avoid milling the already milled material and making even more tinier chips. If you manage to keep the track of the bit clean then you don't need cooling and the edges will be fine. CA good dust/chip extraction is more important than cooling. Blowing air may work, but I found that at least for me, vacuum is much better. It is also more pleasant to use than blowing plastic chips and dust around the room and all over the machine.

What I also experienced problems with is that the protective sheet some times is of a material which melts considerably easier than the acrylic it is protecting, and that is a real problem. You can't run the machine and adjust to the protective sheet, because that will cause problems with milling the acrylic. In those cases I remove the protective sheet before I start milling, because once the protective sheet starts melting it will destroy the work piece as well and will continue melting, taking the acrylic with it and may also destroy your bits.

In my experience, acrylic is a lot of trial and error. What one person is saying is working for him is not always the same that will work for you, unless we would use the same plastic and every other parameter would be the same. There are different material qualities, so just because it is clear acrylic, it is not that all clear acrylics are the same. Especially when you run out of material and need more, you may need to adjust some of the parameters again.

Good luck.

[andy_con]

^^^
very useful thanks

[A_Camera]

thanks for all the info

I have a denford micro router, which is enclosed. I did wonder if things in general were getting hot yesterday, it was a hot day and once I closed the door of the router there is no air movement inside.

Do you have any dust extractor? In my opinion that is VERY important.


how small can you get single flute cutters? I want to engrave so didn't want to go any bigger than 1mm really
The smallest bit I am using is a 0.5mm but it is a dual flute. Feed rate is EXTREMELY critical, run it just a tiny bit faster and it snaps. But... if you are engraving for LED signs then V-bits are better (http://www.ebay.com/sch/i.html?_from=R40&_trksid=p2054436.m570.l1313.TR0.TRC0.H0.Xcarbide+v-shape.TRS0&_nkw=carbide+v-shape&_sacat=0) unless you need to engrave large letters or remove a lot of material, because those are more rigid. Never the less, if you run it too fast or too deep you will snap off the tip, especially the tiny 10degree 0.1mm are very sensitive.

[andy_con]

yes it has dust extraction which I use.

I'm engraving so v bit would be fine. I have some v bits which I use for engraving on ally, so I could test one of them. ill reduce the speed down also


Do you have any dust extractor? In my opinion that is VERY important.


The smallest bit I am using is a 0.5mm but it is a dual flute. Feed rate is EXTREMELY critical, run it just a tiny bit faster and it snaps. But... if you are engraving for LED signs then V-bits are better (http://www.ebay.com/sch/i.html?_from=R40&_trksid=p2054436.m570.l1313.TR0.TRC0.H0.Xcarbide+v-shape.TRS0&_nkw=carbide+v-shape&_sacat=0) unless you need to engrave large letters or remove a lot of material, because those are more rigid. Never the less, if you run it too fast or too deep you will snap off the tip, especially the tiny 10degree 0.1mm are very sensitive.

[A_Camera]

yes it has dust extraction which I use.

I'm engraving so v bit would be fine. I have some v bits which I use for engraving on ally, so I could test one of them. ill reduce the speed down alsoPlease note that I still don't have my high speed spindle installed om my machine, and my current spindle is maxing at 9000RPM, so perhaps if you spin your V-bits fast enough you can increase feed rate as well. Anyway, 22k RPM and 300mm/min is not a good combo. With 22kRPM I would try at least 6-900mm/min using a 30degree 0.3mm V-bit. You have to watch out for corners, the machine may drop the feed rate speed but the spindle will continue spinning at 22k RPM, so melting can happen when rounding corners and then continue on the straight part or the mass of the melted plastic will snap the tip, whichever comes first.

I think it is easier to master milling and engraving at lower RPM first before speeding up things. Once you know you can do it you at low speeds you can start increasing the speeds and understand better what is going on if something goes wrong.

On a side note... I'd start with a brand new and sharp V-bit because if you use an already used one, especially if used on aluminum, then it might not be as pointy and sharp as needed for plastic. A defective or damaged cutter may cause problems (melting, bad edges, uneven surfaces and so on) or may give you good results which are not valid for a new and sharp one. I think it is best to use good tools, so buy a bunch of those and keep a stock of them. You will need more than one before you are confident enough...

Good luck. Milling and engraving acrylics is fun.

[cropwell]

how small can you get single flute cutters?

http://www.sorotec.de/shop/Cutting-Tools/1-8--Shaft-Mill-Tools/1-Flute/End-Mill-Single-Flute--0-3mm.html

[Fred]

I found that cast acrylic mills fairly well and extruded acrylic tends to melt as you describe. When I first started I had a nice batch of cast and didn't realise until i got some cheaper extruded stuff one day.

Now I save the extruded for the laser. Unfortunately it also smells worse when being laser cut.

[magicniner]

Never had one go blunt, had plenty of the feckers snap though! :culpability:

I use them on brass, bronze and 304 stainless as well as plastics ;-)

[naijin]

Do you have any dust extractor? In my opinion that is VERY important.


The smallest bit I am using is a 0.5mm but it is a dual flute. Feed rate is EXTREMELY critical, run it just a tiny bit faster and it snaps. But... if you are engraving for LED signs then V-bits are better (http://www.ebay.com/sch/i.html?_from=R40&_trksid=p2054436.m570.l1313.TR0.TRC0.H0.Xcarbide+v-shape.TRS0&_nkw=carbide+v-shape&_sacat=0) unless you need to engrave large letters or remove a lot of material, because those are more rigid. Never the less, if you run it too fast or too deep you will snap off the tip, especially the tiny 10degree 0.1mm are very sensitive.

Hi there, I have done about 10 acrylic signs so far, I use a v bit and a 3mm end mill but I only go as high as 7000-9000 rpm and it seem to work ok.

Nick

[andy_con]

Thanks for the advice got speeds and feeds perfect


https://youtu.be/NrIJ1bb44sA

[A_Camera]

Hi there, I have done about 10 acrylic signs so far, I use a v bit and a 3mm end mill but I only go as high as 7000-9000 rpm and it seem to work ok.

Nick


Yes, that's what I am using as well. Have not tried to run faster yet, but will try soon.

[A_Camera]

Thanks for the advice got speeds and feeds perfect


https://youtu.be/NrIJ1bb44sALooks very nice, but I find the LEDs at the bottom disturbing. The sign is though really well made.

[Tom J]

Yes, that's what I am using as well. Have not tried to run faster yet, but will try soon.d

feed..rate?