Ok, so a slight deviation on the typical theme for a site called “make it from metal”, but it’s close enough, right?
It seems like the occasional request for parts made from plastic is pretty common for your average machinist. Some shops specialize entirely in this kind of work, but it’s something that you can fully expect to encounter even in a general job shop.
In this article, we’ll cover the following topics:
- How to select an appropriate cutter
- How to achieve a good surface finish
- What speeds and feeds are recommended
- How to handle workholding
- Tips and tricks to make the job go smoothly
Effective cutting tools for acrylic are very different from the tools that you’d use for steel.
The cutting edges need to be razor sharp and very aggressive to avoid problems like poor surface finish and material melting. Usually tools that are designed for aluminum can work well for acrylic, although you’ll find better results with tools specifically made for plastics.
The reason for this is that acrylic melts at a very low temperature. Common machining challenges like built up edges and galling are exacerbated ten times over with most plastics. As a general rule, it’s best not to use cutters that have been previously used for metal, since the edges will likely already have some wear.
Cutting edge rake angles of 5 degrees and clearance angles of 2 degrees work really well. If there isn’t enough of a clearance angle, the material will rub and you’ll have a bad day.
Lots of specialized cutters have only one single flute for maximum chip clearance. These work great, but I’ve used endmills with up to 3 flutes very successfully. The main requirement here is that the chips can easily evacuate without getting stuck, melting, and causing undesirable results.
The advantage to having more flutes is that you can use a higher feed rate, the advantage to having less flutes is that there’s less of a risk of catastrophic failure when the chips don’t clear out properly.
Single flute cutters are also good for keeping the plastic cool while cutting; if you’re having issues with the chips welding then try a tool with less flutes.
Another point to consider is that more flutes will mean that the tool will have a thicker core, which means that it will be less prone to vibration. There will be more information on how to effectively use these tools in the section about cutting strategies.
A small corner radius for endmills can also greatly improve the surface finish on floor geometry.
Here’s a summary:
|Less Flutes||More Flutes|
|Lower feed rate||Higher feed rate|
|Less heat||More heat|
|Less rigid tool||More rigid tool|
|Rougher surface finish, more burrs||Better surface finish, less burrs|
Upcut vs Downcut vs Straight Flute
The majority of the time, you’ll find that an upcut endmill will work best. This means that the flutes spiral upwards, like they do for typical metal cutting endmills.
This is because the chips are lifted up and out of the cut, so they don’t have as much risk of being re-cut and being a source of extra heat. Think of an auger – the tool is pulling the chips out as it’s working.
To use an upcut endmill, you need to have rigid clamping so the workpiece isn’t pulling up into the cutter along with the chips. This also means that parts with very thin floors may not be suitable for this style of cutter, since the floor can flex up and be gouged by the endmill.
Downcut is a practical approach for certain applications. If the workholding isn’t very good, this is a safe choice.
For example, if you’re working with flat parts, you might choose to hold them down with tape. This works particularly well for sheet work. Otherwise, it’s best to avoid downcut endmills unless the application justifies it.
Straight flutes don’t really work very well. Acrylic is best cut with a high helix tool; the impact from a straight flute can dislodge the material from your workholding, and the surface finish won’t be nearly as good. The only exception to this is with PCD tools – those are generally sharp enough to justify the lack of helix.
As a general rule of thumb, the higher the helix, the better.
Carbide is definitely the material of choice for cutting tools. While high speed steel will cut acrylic, it generally won’t give a great surface finish. Some shops use diamond-coated cutters, but this is generally better suited for high-production types of jobs. Diamonds ain’t cheap, and most job shops do just fine with plain carbide.
Cutter Coatings and Finishes
In general, uncoated carbide endmills are the most practical for acrylic. This is because coatings tend to leave a slightly rounded cutting edge, making the tool less sharp.
In harder materials, like steel, a slightly rounded cutting edge is an advantage since it makes the edge stronger and less prone to chipping. But for plastics like acrylic, the material is soft and the cutting edge isn’t working as hard. What’s significantly more important is edge sharpness to reduce heat and prevent rubbing.
Overall, the only kind of coating that will usually make sense is a poly-crystalline diamond, or PCD, coating. This can improve tool life for high-production parts since the cutting edge isn’t prone to wear as much as carbide. Even still, though, acrylic isn’t an abrasive plastic so uncoated carbide will generally be a good starting point for most jobs.
If you really want something that will work well, consider a polished endmill. The tool’s surface finish will be so smooth that the chips will glide across the flute face, and your machined finish will be noticeably better.
These principles apply the same way for turning tools.
The cutter should be sharp, with aggressive rake angles, lots of clearance, and as smooth as possible.
You should also generally avoid tools with excessive radii (like round inserts) – this can cause rubbing if the feed is too low and then the surface finish will be cloudy. My go-to is a 0.060″ nose rad, since it’s a nice balance between lighter cutting pressure and a good surface finish on turned diameters.
If the nose rad is large, then the high feed rate required to maintain a clear finish might cause the following problems:
- The part cracks because it’s under too much pressure from the cutting tool
- The part dislodges from the workholding
- The workholding leaves blemishes on the part
Just remember that plastic can’t take the same amount of pressure that metal can. If you’re working with large diameter stock, this becomes less of an issue, but it can come up on the small diameter stuff.
Really, though, all you need is something sharp, and the rest you can figure out fairly easily. There are some polished carbide turning inserts that work extremely well.
If you’re in a pinch, use a HSS bit, grind extra relief and a hard rake angle, and use a hone stone to dress the cutting edges for maximum sharpness. It’ll be good enough to get a couple of cloudy parts out the door.
Note: If you really do need a glass finish on the acrylic, a PCD cutter is your best bet. Here’s an example of possible results:
For the most part, holemaking is fairly straightforward with acrylic. However, there are a few things to be aware of:
The old-school 118-degree point jobber drills put a lot of heat into the plastic. You’re better off with a 135-degree split point drill that’s very fresh.
Acrylic can be tapped easily enough, but the material itself isn’t the best for
Work holding needs a lot of surface area, otherwise the part will be prone to cracking or coming loose. Even still, clamping pressure can’t be too high.
Don’t use a facemill on a 4″ x 4″ block that’s held by a vise that’s gripping on to the bottom 0.125″ of the part. It’ll pop out of the vise, and everyone in the shop will hear it.
For parts that are very flat, double-sided tape actually works very well. This is practical for working with acrylic sheets. Here are a few tips for this approach:
- Make sure that the tape that you use is very thin, or the part will vibrate and flex during cutting. This is the stuff that I use, it’s cheap and works great.
- Use smaller diameter tools to reduce cutting pressure. If the tool is too big (like a 1/2″ endmill for a part that’s 2″ square) then it will likely pop the part loose.
- Vacuum plates are an excellent way of holding down sheets precisely and firmly, and often the ideal solution.
Peel milling works really well to minimize cutting forces and keep a clear machined surface on the part. Also, because the actual cut time of each flute is greatly reduced, there’s not a lot of opportunity for the heat from cutting to work its way into the part.
That’s actually one of the key fundamentals of machining plastics like acrylic: get the heat out through the chips as fast as possible.
Acrylic melts at a very low temperature: only 320 F. It’s really not hard to get that hot through friction with industrial machines. Using a higher feed rate reduces the risk of rubbing and gets that heat out through the chips.
There’s another important strategy when it comes to machining acrylic: avoid anything that gives you long and stringy chips.
This applies to both milling and turning.
When milling, avoid plunging engagements in favor of shallow ramping motions. If there’s no way around it, use a pecking cycle to break up the length of the chip.
These chips can build up around the tool and then melt the plastic through friction as it spins against the workpiece. It can also block coolant from reaching your tool.
If you’re having problems with a rat’s nest of chips around your tool, here’s one possible way that you can deal with it:
Retract up to about an inch above your workpiece and throw the spindle into reverse. This is usually enough to toss out the chips.
If you’re programming manually, this is what the code will look like:
G81 X1. Y1. Z-1.0 R1.0 F30.0;
This will retract the tool back up to 1 inch above the workpiece, reverse the spindle, wait for 1 second for the chips to fly out, then flip the spindle back to clockwise rotation.
This is usually my last resort, but it does work.
For turning, this is more challenging. Acrylic is very difficult to cut hard enough for a chip breaker geometry to work; it’s just way too malleable.
Come at the work from the angle with the least amount of material. Depending on your setup, it might make sense to rough the part out using a X-axis plunge.
If there isn’t a lot to be removed on the diameter, this can be an effective way of preventing the chips from becoming three miles long. Or, if you’re needing to do a facing operation, it might work best to do the rough cut with a Z feed and then leave finishing for a light cut in the X.
Another option is to rough it in sections. For example, if you have a part that’s 10″ long, have 4 roughing operations that each manage 2.5″ segments
Some CAM systems or controllers have an option for a “stutter-feed”. This is a really excellent solution for breaking up chips – similar in concept to a G73 peck drilling cycle.
At the end of the day, if all else fails, just feed it as hard and fast as you can without having the part fly out of the workholding.
Feeds and Speeds
Of course, if you’re buying tools specifically for the job, you’re best off consulting the cutter manufacturer for machining parameters.
But, if you’re like me, you’ll have a pile of aluminum cutters that are just asking to be used. Here’s what I do for speeds and feeds:
Lots of guys just use parameters for aluminum, but generally the feed isn’t high enough to really be efficient.
Typically I’ll actually go a little slower in RPM, but double triple the feed rate. I find that this offers the best chip control and least risk of the material gumming up, since the chips aren’t getting quite as hot with the slightly lower RPM.
For example, if I have a 1/4″ 3-flute uncoated endmill, I’ll start at about 600 SFM with a 0.003″ CPT. This works out to about 9600 RPM and a feed rate of 86.4 IPM.
For turning, I’ll follow a similar principle, but with a rigid setup (like using a chuck and a tailstock on a thick part) you can really crank up the feed rate. Just triple the feedrate that you’d use for aluminum and you have a good starting point.
For finishing, you don’t need to leave too much stock. Even 0.005″ is lots for most applications. By keeping the finished stock to a minimum, the chips from this operation will likely not be large enough to pose a threat.
Lubrication and Coolant
Oil misters and flood coolant are very popular ways of lubricating and cooling acrylic for cutting. Air blast cooling can also work with polished tools or diamond cutters.
One thing that is worth paying attention to though is the chip clearing system. High pressure coolant is great for blasting the chips clear of the cutter, but long and stringy chips can easily jam up the chip auger or belt.
If there’s no way of avoiding stringy chips, then consider turning off your chip removal system and clean it out manually at the end of the shift.
Another consideration is coolant filtration. Fine plastic particles can pass through mesh filters and clog up a coolant line. It might be worth it to use a paper filter.
One more thing to double check if you’re going to use coolant: Make sure that the emulsion won’t react with the plastic, causing it to become cloudy or melt. Usually most coolants will be fine, but not all of them are. If you’re not sure, drop an offcut of the acrylic into a bucket of coolant and let it sit overnight. If it’s fine in the morning, you’re in the clear.
Alternative Finishing Methods
Flame polishing acrylic is one of the most common ways of getting a clear, glossy surface. Here’s a video that illustrates how this is done:
It should be noted though that this has drawbacks. “Crazing” is a possible problem. This happens when there are tensions is a material that is prone to cracking. Essentially, it’s a large amount of microcracking along the surface.
The heating and cooling of the acrylic is what causes this buildup of tension. To counteract this, you need to do some thermal tempering of the part. It’s not a perfect solution, though, since it could easily cause the part to warp and distort. The key here is to not let the acrylic heat up too much, and to ensure that the heating is even.
It can also be tricky to maintain a sharp edge – as the acrylic reaches its melting point on the surface, it will have a tendency to distort slightly.
Polishing by hand is a tedious process at best, and it’s unlikely that you’ll be able to get a clear surface without distorting it. Generally the only way to get a perfectly flat polished surface is by using specialized equipment.
Tips and Tricks
- Avoid using solvents to clean acrylic parts, since they can melt the part or make it turn cloudy. If you’re not sure, test it out on an offcut first.
- Water-based coolant vs oil-based coolant is generally a better choice, since the parts can be rinsed off with water to remove the oily residue.
- Do everything that you can to avoid stringy chips. They are a serious safety concern to both personnel and equipment.
- Use coolant to direct the chip away more so than cool the tool.
- Turning on a manual lathe? Use Dawn dish soap for lubrication.
- Cast acrylic is significantly easier to machine than extruded; it doesn’t gum up nearly as much.
Have your own tricks or questions? That’s what the comments are for.