Tips for Cutting Acrylic Parts on the CNC
Detailed, specific advice and explanations for cutting sheet acrylic on CNC equipment. April 21, 2011
Question
I need to know what 3mm router blade to use to achieve a clean cut without furring (melted chip buildup). Is it best to go for 2 or 3 flutes, and what router speed should I cut the material? I'm based in the UK. I normally get my blades from Menlo. The last blades I tried didn't solve the problem at all. They were down cut spiral double flute routers.
Forum Responses
(CNC Forum)
From contributor Y:
I use a 1 flute and do a rough cut with a .01 offset, leaving a skin, then a finish cut all the way through.
From contributor M:
Onsrud 52-700 series spiral O.
From the original questioner:
Also, is a downcut or upcut router blade better?
From contributor V:
Yes, routers usually produce furring problems. To solve this problem, use a milling blade. For cutting flutes, 0-24000 rpm router speed will be better, and router spindle working speed 3000-6000mm/min is nice.
From contributor J:
The goal is to shear a cool chip up and away from the cut. If you are going too slow with a high spindle speed, then the plastic melts onto your blade and remelts the cut together. A single flute O spiral bit will do this cut. If you have a strong vacuum then an up spiral bit is the way to go. I have not done this with a down spiral, so hopefully someone with more experience will chime in. What are you cutting, sign letters?
From contributor G:
Use any of the Onsrud O flutes for plastic. 3/16" or larger. Most important is that the cutter never touches wood. Single pass. 18,000 rpm and 200 - 350 IPM. The larger the diameter, the better.
From the original questioner:
Contributor G, I machine various shapes from a sheet of 3mm acrylic (Perspex). Why should the blade never touch wood? I place the acrylic on top of some MDF.
I'm going to buy a couple of Onsrud bits, but is there any advantage to using a straight plunge router bit compared to a spiral bit? Just wondering as I haven't tried cutting acrylic using a straight bit before.
From contributor Y:
I have a Gerber bit that is made for acrylic. It does a real nice job. I got it from Hyatt's art supply. I ordered on a Sunday and had it on Wednesday. It is the gold series cutter.
From contributor M:
The advantage of an up spiral is just like contributor J says - the goal is to get a cool chip up and away before rewelding. It doesn't mean you can't cut acrylic with a straight flute, but unlike wood, acrylic is homogenous and predictable, so you don't have a serious problem with chipping at the top of the sheet. Use every advantage. Acrylic is also smooth and reasonably rigid so it isn't too hard to keep stuck to the table. If your parts are very small, you may need to sacrifice the advantage of the upshear for a straight flute or downshear, but it will be at the expense of another variable, most likely speed or cut quality.
If you are really paying close attention, the video from Onsrud shows a second pass with a 75-012. Though I haven't tried it, in the catalog it looks like a straight flute with almost no gullet. I imagine that is because you are only removing a very small amount in the second pass and this tool would stay sharper and be very stiff. I like the idea and the method and next time I have an acrylic job I will try it.
From contributor G:
Wood or paper is an abrasive. It will affect the finish on your acrylic. I guess I'm saying avoid wood as much a possible. Your cutter won't be trash if it touches it, but avoid it. We do a lot of cutting in all plastics. Even our saw blades are changed when we cut wood or plastic. Once that blade touches wood, it's just not the same. I've been cutting plastics since 1988 and I've found this is a great practice. When we cut acrylic sheet with paper masking, you can actually see grooves in the cutter where it's cutting through the masking.
I use a straight bit because I find the finish to be better in cutting acrylic. Up spirals tend to lift the part and down spirals shove the material into the spoilboard. I use them all but prefer the straight. I also find less vibration giving a better edge.
From contributor Y:
The cost of the Onsrud 75-000 series bits is expensive. 75-002 is $1840.40 from Onsrud.
From contributor M:
Well, that puts it in a different perspective! I was expecting a tenth the cost. Scratch my last post.
From contributor G:
O flute Onsrud cutters are $20-$25 and they are perfect for cutting 3mm acrylic.
From contributor W:
My technique is to surface my spoil board, then remove the paper from the top surface to save work later. Then set your Z depth to go all the way through the plastic and half way through the paper on the bottom. This way you never lose vacuum and the adhesive on the bottom paper holds the part in place. I use this method to cut fonts and it works perfect.
In addition, if your cutter goes all the way through the paper, you will pull MDF dust up into the plastic and tarnish the edge. For 3 mm I would use a 1/8 inch bit. Also, keep in mind there is a big difference in cutting cast acrylic and extruded plastic
From the original questioner:
Contributor W, I'm not quite understanding what you mean about the paper. The acrylic sheet I purchased has a plastic protective film/sheet on both sides. What is this paper you are talking about?
From contributor G:
Acrylic is available in both paper and film masking. The technique described above is for cutting small parts. Also, use a cutter with the biggest possible diameter. You will get great cuts. It's not very often I use anything less than 1/4". I use 1/2" whenever I can.
From contributor J:
Contributor W, are you spraying a small tack?
From the original questioner:
Regarding the protective paper on the back of the acrylic sheet... What is the thickness of this paper? Is it significantly thicker than the protective plastic film? Just wondering how accurate you need to be on the Z axis.
Contributor G, you mentioned that you use a straight bit. Can you tell me which brand/model?
From contributor W:
Yes, part of this technique applies to small parts. Take a micrometer and measure the protective coating.
Contributor J, I don't understand the question.
From contributor J:
"the adhesive on the bottom paper holds the part in place"
How is it adhered with the paper face still on?
From contributor G:
Onsrud 61-082 1/4" dia and 61-041 for 1/8". The whole 61 series.
Contributor J, he's cutting through the acrylic and not the bottom layer of paper... letting the adhesive on the paper masking hold the part in place. Just like onion skinning. In this technique I usually set my cutter to the spoilboard and cut .004" above that.
From contributor J:
Got it - makes sense. I am cutting 10 sheets of .090 6061 and learning a lot. Making small bolt covers for drink rail legs where fastened to concrete
From the original questioner:
I have just order a product called Vilmill black. It's used to cut out small parts. Anyone have experience with it?
Thanks for all your help guys. I'm now using an Onsrud Super O and it's cutting through the acrylic absolutely perfectly.
From contributor F:
All those Onsrud suggestions were right on. Very interesting in hearing how the Vilmill stuff works. We do a similar technique here, using a few layers of sign masking paper applied to the sheet first, but the Vilmill looks easier (maybe not cheaper).
The comments below were added after this Forum discussion was archived as a Knowledge Base article (add your comment).
Comment from contributor A:
Use a downcut router when the material might be pulled upward by an upcutting router or mill, and only when you have a place below the cutter for the chips to go. For instance, when you have a large piece of material on a milling machine table and don't have a good way of uniformly holding it down the edge of the material hangs slightly over the edge of the table. The downcut router will exert force such that the material you are cutting is held down. Also, whereas the upcut router will drop chips on the part, obscuring your view of the cut, the downcutter won't do that. There's no particular advantage in finish for one over the other. It's just how you're using them.
