Issues carving 20mm Acrylic

I’m trying to carve a logo out of 20mm acrylic that I previously cut out of 24mm cherry wood.

The wood carve worked flawless.

The acrylic carve however went quite wrong:

I tried using the same grey 1/8" upcut bit I used for the wood. It started out fine but then went off path and started to make pretty unhealthy sounds :smile:

It seems as if it lost track of it’s Y coordinate and tried to carve the bottom cutout too high up. Also the Z axis seemed too deep when I stopped the machine. It’s supposed to use 1mm depth per pass but there it was carving in more like 2-3mm depth.

When I touched the acrylic to take it out it was pretty hot even a couple of minutes after I stopped the machine. So I’m guessing the issue is heat and amount of dirt over time?

But then in a second cutout attempt it stopped/lost track at the very same place. During a 45 degree diagonal motion where both the X and Y coordinates are changing. It never seems to happen on straights where only the X or only the Y coordinates are changing.

I know 20mm acrylic is going to be tough, if at all possible. I also read you’re supposed to cool the bit with water. Which isn’t quite possible in the Carvey since it stops when I open the door. Though there’s probably a way around that.

Does anyone have experience cutting acrylic on the Carvey? Are my assumptions correct? Or is the issue something else?

I first searched the forums and read tips about tensioning the belts. I could try that, however I successfully did another wood carve of the same object after the acrylic failed, so am not sure the machine itself is the issue. More likely something I’m doing wrong here.

If heat is the issue maybe I could pause the cut more often and let the bit cool down.

what depth of cut and linear speed are you using?

The standard Easel recommends for cast acrylic:

This is what it looks and sounds like once the drill gets off path. Before that it’s a monotone humming and then suddenly turns into a stuttering with the bit jumping around in the material.

Sorry for not getting back to you earlier. I am buried in work this weekend.

I would lower your depth to .5mm per pass and test on a scrap . What brand of acrylic sheet are you using?

With acrylic, I like to go shallow on depth per pass and fast on the feed rate.

Lukas,

Definitely want to turn up the speed and lower the DOC. I typically use 1300 mm/min and DOC of 0.5 mm with the X-Carve. You should do some tests to see what works best for you.

What type of acrylic is it? Cast works much better than extruded which is what you typically get from a local hardware store.

Also, as a point of humor, the sound from your video made me think of the Jurassic Park T-Rex roar.

Like a few others, you need to lower the DOC, and speed up the feed rate. Is it possible acrylic bits got into a wheel or belt? Im not sure how the carvey is setup.

The Carvey is relatively well protected against material flying into parts but I’ll remove the bottom cover and check the belts before attempting the next carve.

The material is cast acrylic.

Thanks for the settings! I’ll try with the reduced DOC and increased feed rate. It’ll be next Saturday before I have access to the machine again.

I’ll also do the carve in parts instead of all in one go and let the bit cool down / clean out the chamber after each section.

I’ll update this thread after my next attempt.

Thanks again for all the tips!

I managed to get access to the machine for two hours today already. Unfortunately the new settings (1300mm/0.5mm) didn’t bring any improvement. If anything the result was worse.

For cost reasons I tried with a sheet of blue 3mm cast acrylic instead of the 20mm this time. It seems he lost track of X/Y already while drilling the four mounting holes of the sign. Because right when he started carving the first outline he was in the wrong spot. But also all carving was stuttery from the start. Here’s what he carved before I stopped it.

I honestly don’t even know which part he was trying to carve when he started to mess up around the upper left hole.

This is the work piece in Easel and there’s nothing to carve in the direct vicinity of that hole:

(One tab is in the wrong place, I just quickly threw them in because I didn’t use double sided tape this time)

To make sure it’s not the machine I opened it up and checked the belt tension - which was fine.

I then took the same work piece and swapped the acrylic with some soft foam core material which carved just fine:


Would need some cleanup obviously but the shape is alright and a perfect match when overlaid on the wooden piece.

I’m beginning to think the 1/8th single flute upcut might not be the right bit or maybe I’d need to feed it slower instead of faster. Unfortunately it’s the only one I got that’s long enough for the 20mm acrylic.

Once I’ve got access to the machine again I’ll do some trial and error on the cheap 3mm acrylic sheets with different bits and feed rates.

The brand of acrylic I’m using is called PLEXIGLAS GS from Evonik for the 20mm and PERSPEX for the coloured 3mm sheet.

Lukas, sorry I didn’t realize you were only using a single flute. I typically use a two flute.

Also, I re-watched the video above and maybe its just the viewpoint but it looks like the machine is cutting much more than 1mm DOC. If this is true, that plus a single flute with those settings I can understand why you are getting the results you are.
Can you confirm it’s cutting at the DOC correctly?

Yes I noticed that. Like I wrote in my original post

Also the Z axis seemed too deep when I stopped the machine. It’s supposed to use 1mm depth per pass but there it was carving in more like 2-3mm depth.

This happens because it looses track at a point where it’s already three passes deep into the material. So once it leaves it’s path it’s trying to carve way too much material which makes things even worse. Though I suppose at that point it doesn’t really matter anymore, after it leaves it’s path that is.

Before that though it’s using the correct depth. I confirmed that again last night when I had it do the carve of soft core foam. The recommended settings were 0.8mm per pass and I counted the number of rounds it would carve each shape. Everything seems fine as far as the machine is concerned.

It’s most likely an issue with the bit/material/settings.

Indeed, failure point have occured already.
So you need to figure out (with help from us :scream: ) why it failed to begin with.

If you want to share the Easel project I will try it on my Carvey, I don’t have any 20mm acrylic but I have a heap of 3mm and 4mm from old server rack doors to play with.

I just did a mounting plate for a hard disk for a Raspberry Pi with a 3mm 2 flute bit at 500mm/min and 0.5mm DOC and that turned out fine.

Of course, here it is: http://easel.inventables.com/projects/Mc6QAC-zfXCfC8_bfEt7aQ

Which 2 flute bit are you using? Is it one from Inventables?

I had read on the forums here that a single flut upcut works best for acrylic. Though that was an X-Carve user. Not sure how much of a difference that makes.

You can try a 2 flute mill if you like but a single flute upcut bit is really the preferred mill. If the carvey can use a 1/4 in mill and your design allows for it do it. That goes for all cnc cutting really. I cut acrylic for a living. 20mm is a lot of material for an 1/8 in bit. But it doesn’t sound like your getting anywhere near that depth yet. I’m not sure what your issue is but I do think just based on the sound of your cutting an the size and shape of your chips heat being is generated faster than it is being removed. When properly cutting acrylic your chips should be almost granulated sugar like. Not like little grains of rice. That means they are rewelding.

I tried this project the other day and thought I would turn it into an acrylic cutting test of the the bits I have.

I did all the inner cuts at 500mm/min and .5mm DOC.

As the other info is a bit off topic here I’ll start a new thread with the results of the 5 bits I used.

Gary

So the 2 flute didn’t work at all for me. I tried at 500mm/min as well as the recommended 1100mm/min and neither carved the test material properly.

That said today I tested with some white acrylic that, as I later found out was extruded and not cast. So keep that in mind.

In any case, the “default” blue 2 flute 1/16th Carvey drill bit just gunked up and eventually broke.



I then retried with the 1/8th single flute bit (I don’t have a 1/4th but I’ll put in an order at Inventables sometime this week) at 500mm/min with a DOC of 0.2mm. The result was again a gunked up bit however at no point did it lose track of the X/Y coordinates as it did before.

So I figured 0.2mm per pass seemed like a good value but the speed was too low. So I increased it to 1300mm/min and voila it carved the entire logo.

However the build up of material still occurred. It just moved fast enough for the gunk to fly off the drill.

Also at some point it lifted the material in the middle for like one or two mm. The chips weren’t like granulated sugar at all. More like big boogers :scream:

Note how material build up on the bit and then violently flies away.
The very rough shape in the upper left was still from the blue 1/16th bit.

However in the end it finished the carve and the result was quite okay.


I’ll try with cast acrylic next time and will tape down the material instead of just clamping it and using taps.

My general feeling for cutting acrylic with the Carvey so far is, as large as possible single flute bit, very low DOC and high feed rate. At least that’s the settings that worked for me today.

I still want to find the settings that will produce the granulated sugar like chips. Though as I mentioned this was extruded acrylic so maybe that also had something to do with it.

P.S. the drill bit was the same one I used in previous carves, so the losing track of X/Y wasn’t caused by a dull bit. I’ve only used it for these couple of acrylic carves and two wood carves.

I think any and all problems you are having now can be attributed to that being extruded acrylic. That’s being said with the correct bit,speed, and feed you can successfully rout extruded acrylic. After you switch back to cast if your still getting melting/rewelding then your spindle speed and feed rate is wrong. Its all a matter of finding what the machine is capable of. Increase feed rate lower rpm, sounds counter intuitive but that the general idea, just see what works. My machine at work can cut 3/8in acrylic in a single pass at 90 ipm 18000rpm and the finish is flawless. My X-Carve not so much.

1 Like

Lukas, glad you made some progress. I forgot that the Carvey is lower RPM than the X-Carve. The cast can definitely have an impact. I think you’ll notice a big improvement when you get your hands on some.

Also, I know Phil and others have mentioned here and in other posts about cooling flow but I have cut my share of acrylic and haven’t had any issues yet without any cooling other than exhaust from the Dewalt. As they say, results may vary.

1 Like

I’m not a Carvey user so this is likely of no use but I carve acrylic at a feed-rate of 1800mm p/min and 0.25mm depth of cut. I’ve found moving quickly, coupled with good dust collection, avoids chips building up and I’ve never had any melted spoil on the mill end. Your first pictures of the 20mm acrylic appeared to show all was well up to a point, after which things went a little nutty. This may have already been mentioned but could it be that a long slow carve caused a static buildup and then discharge, confusing the Carvey? I’ve had that happen with the x-carve in the past until I sorted my dust collection and grounding.