Machining Polycarbonate

[Tool-n-Around]

Hi all. Been a while but I’ve been busy with cb. I haven’t had to pay very close attention to feed/speed machining foam patterns but not the case here.

Looking for a little feed and speed guidance for machining polycarbonate. I previously made a post about another polycarbonate lid I made, but I’ll be darned if I can find it. Before I post the cb file, thought I’d just start with the piece I machined, and describe some of the issues I had, and see if I can get a nudge in the right direction.

The part is a display lid for an automotive air filter. The stock size is 21”L x 8”w x .5”t.

I’m seeing a lot of chip welding. I don’t have cut data for the bits, but in general they are carbide woodworking bits unless I say otherwise.

First op was the logo. I had machined it before on a previous project (also polycarbonate) with pretty good results. I set the lowest speed on my router (about 14krpm). It’s a single flute .031” ball nose cutter so it can fit through the narrowest regions of the letter pockets. The feed rates are 15in/min. The depth of cut was .020” and final depth .031. I cut a test plaque and thought it looked good. When I cut the logo on the actual part the chips melted/welded around the bit and scarred the surface around the ellipse. I’m thinking I need to back off to a smaller depth increment to help clear the chips and keep compressed air on the cut. The problem is the darn chips tend to hang on the surface edge like a stringy burr so they can’t always be cleared. Not sure which direction I need to go on feed/speed. I’m at low rpm limit. Coolant/mist is not really option.

The ornamental grooves cut pretty well.

The perimeter chamfer (.5”D double flute 90 degree vee). Depth increment was .15” and final depth .2”, 16krpm. It was a total mess with chip welding on the conventional cut side only. I did a .005” clean up climb cut and the chip welding switched to the waste side, and the part finish looked OK.

The filter gland is cut with a .5”D dish cutter. I didnt post a picture and it has some tool marks in part from the piece being inadequately secured (a screw in each corner and two in centrally in the part). I’m not too concerned about this because the gland turns visbly black when the filter element is installed and I'll never achieve optical clarity on my machine or without polishing.

The .25”D double flute spiral end mill perimeter cuts were a mess. The feed rate 60in/min, depth increment was .25”, and .35” cut width, 16krpm, which for sure was too aggressive for my router and probably so for my hobby cnc machine, especially in the initial two-sided plunge cut. I had a final .5" full depth finish cut of .010” which after observing the chamfer cut, I chose to climb cut. I didn’t post pictures because probably same issue here. The perimeter finish is not so great but why does climb cutting seem to be producing a better result?

I can post additional info as needed, but had to break the cb file up for tool changes and made in-process mods to those files so will need to update the consolidated file before I do so. I can probably salvage this part with some elbow grease but looking to do much better on next pieces.

Best,
Kelly

[Tool-n-Around]

I couldnt find any information of cutting speeds for PC....probably not looking in the right place.

Just thinking this through a little bit, if I'm melting the polycarbonate, I'm dwelling and/or not ejecting chips. Since I can't go any lower in rpm, I may need to increase feed rate. If the router cant handle that, then take smaller depth of cut. Also, I have a .25" O-flute carbide bit that is supposed to be for harder plastics. Being single flute seems that it will also help. I can buy 1/32 O-flute flat bottom bits inexpensively.....may do that too just to have them if the .25D O-flute performs well.

Think I just may need to experiment a bit on some test plaques.

Best,
Kelly

[EddyCurrent]

I know you said coolant was not an option and it's the same for me, but, I get far better cutting with a little washing up liquid in water just dribbled on top.

[lloydsp]

Why is coolant not an option?  It's fairly inexpensive and simple to implement.

Lloyd

[airnocker]

One possible reason liquid cooling may not be an option is that not everyone's machine is waterproof or even water splatter-proof.

I'm no expert but have done a lot of polycarbonate engraving and milling, relatively speaking.
If welding is occurring then that is an indication of high friction and heat.  You're on the right path to increase your feed rate if you cannot decrease your spindle rpm.  Also, large diameter mill bits will have a higher angular velocity than a much smaller bit for a given rpm.

[Tool-n-Around]

Why is coolant not an option?  It's fairly inexpensive and simple to implement. Lloyd

Well perhaps not an option is too strong, but at least not a good option for me since most all of my work is dry cutting softer materials and with an mdf bed and waste board, I’d suppose I could just make a collection pan. Would still be a heck of a mess along with the wet chip ejection and prevent vacuum chip collection. If need be and I do enough with polycarb in the future, I probably have a spindle purchase in my future for reasons other than just this, instead of the cheap router, which should afford a bigger speed range if needed. Not yet certain it’s needed…..I thought my sample cut on the logo looked good, but that long stringy burr got woulnd up on the cutter which did not happen on the sample. I have a few things to try. I think it may benefit from more feedrate too but with that small of a pattern the direction changes can get inertially violent.

One possible reason liquid cooling may not be an option is that not everyone's machine is waterproof or even water splatter-proof.

That is the case with me at the moment but could probably be managed.

I know you said coolant was not an option and it's the same for me, but, I get far better cutting with a little washing up liquid in water just dribbled on top.

A little puddle or squirt bottle applied spritz would be a possibility on the logo. It’s small so not much of a mess to deal with but enough to handle the perimeter cuts would be a lot more to deal with.

I'm no expert but have done a lot of polycarbonate engraving and milling, relatively speaking.

If welding is occurring then that is an indication of high friction and heat.  You're on the right path to increase your feed rate if you cannot decrease your spindle rpm.  Also, large diameter mill bits will have a higher angular velocity than a much smaller bit for a given rpm.

What cutters and speed did you use?

The .25D cute was a low helix angle spiral which according to the manufacturer is designed for hard plastics, which may be the case but even though its upcut, probably doesn’t eject chips as well, especially on the two sided cut. I have a single O-flute cutter in that .25D which is supposed to be better, and thinking with a little shallower depth increment and more federate may do the trick dry.
The .031 cutter I was using to cut the logo is actually a single O-flute not round nose. I had to look at that thing under high magnification to confirm such.

I’ll do some experimenting tomorrow and report back.

Thanks for the replies and Happy Thanksgiving to the US guys.

Best,
Kelly

[lloydsp]

"...with an mdf bed and waste board, I’d suppose I could just make a collection pan."
--------------
That's why I asked.  Reasons can vary from "the equipment can't stand water" (yours) to "I don't want to" (often heard).  Yours is a good reason.

Would a variable duty-cycle motor driver perhaps permit you to run that router more slowly?

Lloyd

[Tool-n-Around]

Would a variable duty-cycle motor driver perhaps permit you to run that router more slowly? Lloyd

Well, the router already has a dial that varies speed from 14krpm-24krpm, which was kind of handy for experimenting because I can change speed as it cuts and observe the chip and general quality of cuts. I'm not sure what it uses for control, probably PWM or maybe just rheostat given its a brush motor. Not sure I could get away with another such device in series, and they do lose power at lower Rs......not a problem for the small bit bit likely so for the .25D 2-sided cuts.

Best,
Kelly

[dave benson]

There is a vid on Utube where the people from carbide create cut out some polycarbonate
and give the feeds and speeds for various tool diameters.

He does lament that his software doesn’t have a spiral lead in’s, CB does though.
This is important is can help a lot, is for example in your Logo where you are using a
ball end endmill, it’s a good idea to use the leadins as plunging straight down into the material
is not a ball end mill’s superpower, (typically the plunge feed rate is less than a center cutting endmill) and
as this is the start of the cut and if you get chip welding it’s hard to recover from.

From the Sutton manual.

 The two main functions of the cutting fluid are lubrication and cooling. The purpose of lubrication is to reduce friction by lubricating the surfaces tool and work, to facilitate easier sliding of the chips up the flute and to prevent the chips welding to the cutting edges.

I always use dish washing detergent for polycarbonate\Acrylic.
My machine has no mister and sometimes I use a tub that the vice sits in with a small pump
that recirculates the coolant. I use it rarely though.

The trick will be, using Dish washing Liquid is to mix a small amount in a container (I use an old film canister)
I use the concentrate and mix it one to one so that it still has that light oily feel and when
you rub it between your fingers it should want to stick to both of them like gear oil might.
At the start of the job I coat the endmill with a thin film (It takes a surprisingly little amount small to work)
I use a small brush to do this and rub some on the surface to be cut at the start of the cut and
some brush some more on maybe after a few depth increments.

Use climb milling if your machine is happy to do it, this tends to grab the work so make sure
the stock is well secured, a compression or down cutting bit is nice for cutting thin materials
as it doesn’t tend to lift the material off the bed as it cuts.

Without the cutting surface speed for the material or the chipload from the endmills manufacturer data sheet
your feed and speeds cannot be calculated, so it’s a guesstimate at best.
The young man in the video mentions at some point that the surface speed he’s using is 600 sfm
When I had a quick look at some old files my notes said 180 m\mm which is close.
My spindle speed is limited so re-calculated to suit.

Another thing to keep in mind is that for example if you are using a profile where you are
plunging straight down and then proceed to cut around the periphery of the object, then this for calculations
sake is considered as slotting (equivalent to 100% stepover) so instead of calculating for one diameter
depth, you calculate for 0.5 diameter depth.

Dave

[Bubba]

Happy Thanksgiving to everyone in the US.

When I machine polycarbonate, I always use single flute endmill (have better success with HS .25"EM vs carbide. Use lots of compressed air directed where endmill engages piece. Because I have PID spindle control, run the spindle at 9000 rpm, and high feedrate, and .25 deep. The feedrate most often is set at 45 ipm. Hopefully this will give you idea.. Get scrap piece, set the rpm's to low end and make cuts varying the feed rate. When cuts the best it sound/feel like the endmill will break any moment. That where you will see nice cut. Good luck.

[airnocker]

What cutters and speed did you use?

The .25D cute was a low helix angle spiral which according to the manufacturer is designed for hard plastics, which may be the case but even though its upcut, probably doesn’t eject chips as well, especially on the two sided cut. I have a single O-flute cutter in that .25D which is supposed to be better, and thinking with a little shallower depth increment and more federate may do the trick dry.
The .031 cutter I was using to cut the logo is actually a single O-flute not round nose. I had to look at that thing under high magnification to confirm such.

My Porter Cable router 890 is my "spindle" and is modified to be controlled by a Super-PID speed controller.  I've used this combination now for close to 9 years.  https://www.vhipe.com/product-private/SuperPID-Home.htm. 

My router also originally came with its own "dial" speed control in a similar rpm range like yours and could not go below 14K rpm either.  With this PID controller it can now go down far further, like 5K rpm, under complete control by Mach3.  My acrylic milling/engraving speeds are usually in the 10-12K range, feeds in the 30-45 ips range.  The largest bit I use is a 1 or 2-flute .125".  I've grown to prefer doing parts cut-outs using a .0625" diameter bit just to minimize stock waste, but have also used a .0313" 2-flute.  If waste isn't a concern then I use a .125" 1 flute upcut bit.  But my preference is a .0625" 1 flute, fish-tail with an .125" shank.  I also use the same size in an upcut fish-tail, both with a .25" flute length.  My depths of cuts are usually from half the diameter of the bit and occasionally up to the diameter of the bit.  I buy bits that are expressly optimized for thermoplastics and get them from Think & Tinker, Ltd. in Colorado.  Their website is https://www.precisebits.com/.

My machine is made from polyurethane'd MDO with the waste board made of polyurethane'd MDF, except for the worksurface.  I've added the capability to use small amounts of liquid lubricant by screwing down a piece of HPDE, surfaced so it has about .125" raised edges, for a spoil board that's about 12" x 22".  But for most of my acrylic milling and engraving I've not needed it.

Happy TurkeyDay!

[Tool-n-Around]

There is a vid on Utube where the people from carbide create cut out some polycarbonate
and give the feeds and speeds for various tool diameters.

I always forget YouTube. Upon quick search I see there’s tons there.

He does lament that his software doesn’t have a spiral lead in’s, CB does though.
This is important is can help a lot, is for example in your Logo where you are using a
ball end endmill, it’s a good idea to use the leadins as plunging straight down into the material
is not a ball end mill’s superpower, (typically the plunge feed rate is less than a center cutting endmill) and as this is the start of the cut and if you get chip welding it’s hard to recover from.

My palm is on my forehead. In fact I could see this happening upon the plunge. I will incorporate lead ins.

I always use dish washing detergent for polycarbonate\Acrylic.

Will do so after some more (dry) experimentation.

Without the cutting surface speed for the material or the chipload from the endmills manufacturer data sheet your feed and speeds cannot be calculated, so it’s a guesstimate at best.

Well, I searched my memory, poked around, and low and behold found the O-Flute data. The feederate for the ¼”D bit is making my eyes pop a bit. My router is only 1.25HP and at lowest speed, will be a fraction of that. Will need modest DOC for what the chart suggests. See attached.

When I machine polycarbonate, I always use single flute endmill (have better success with HS .25"EM vs carbide. Use lots of compressed air directed where endmill engages piece. Because I have PID spindle control, run the spindle at 9000 rpm, and high feedrate, and .25 deep. The feedrate most often is set at 45 ipm. Hopefully this will give you idea. Get scrap piece, set the rpm's to low end and make cuts varying the feed rate. When cuts the best it sound/feel like the endmill will break any moment. That where you will see nice cut. Good luck.

Thanks Bubba, wont be able to get quite that low rpm but have been in that 45 ipm range. Only carbide at the moment, but anxious to try the single O-Flute. The chart I posted seems to suggest 150-200ipm…..dont know that I’ll have the courage.

My router also originally came with its own "dial" speed control in a similar rpm range like yours and could not go below 14K rpm either.  With this PID controller it can now go down far further, like 5K rpm, under complete control by Mach3.  My acrylic milling/engraving speeds are usually in the 10-12K range, feeds in the 30-45 ips range. .......Their website is https://www.precisebits.com/.

Thanks for that airnocker and for the source. Similar to other feedrates mentioned but cant quite dial that low rpm. May need a little more feedrate and less DOC.

Thanks for replies guys.

Best,
Kelly

[pixelmaker]

Hello
sawing and milling polycarbonate is daily work for me.

All I can see from the pictures is that the cutter is not suitable for polycarbonate. It is not sharp enough.
You can already see this with the holes, the hole is not straight and throws up the edge on the top.
The fact that you can see the individual depth increments also shows that the milling cutter is bent away here.
By the way, spiral drilling is the better choice.
Polycarbonate must be processed as cold as possible.
The chips must cool the cut. Therefore, one mills with extremely sharp polished cutters with one flute. Good straight cutters for PMMA with one cutting edge are necessary for milling. We mostly use the ACRYLIC SINGLE FLUTE ROUTING TOOLS GENERATION 2 from crown-norge.no For diameters over 6mm we use the BALANCED single flute routing tools.
Radius or ball cutters have hardly any cutting edge towards the tip. More frictional heat is generated there, which cannot be removed due to the lack of chip size.
For such drawings you need very expensive ballnose cutters with only one flute and and a shank with reduced diameter.
However, the cut is not clean at the top. So you only cut radii with it and clear pockets with straight cutters.

A little explanation.
Polycarbonate is an extremely impact-resistant thermoplastic. Cold, the material does not break, it deforms, because of the impact strength, the material is difficult to cut and mill.
If the material becomes warm, it softens abruptly. With a very small margin, the material then becomes white and foamy, also due to the high water absorption. This is why polycarbonate is better formed cold and not under heat, as is the case with PMMA.
The small margin of heat tolerance goes together with the high water absorption. It is 12 times higher than PMMA. The material must be dried if it is to be processed hot. The material gets a white surface when it gets hot because it is milled with blunt cutters.

For all these reasons, PC is not well suited for such milling work.
Cooling with mist can only assist, as with all thermoplastics. But if the tool is not right, it will not help.
Cutting under water is also not a solution because of the high water absorption. The material will be damaged. Only if you can dry it professionally afterwards (12 hours at 105°C) would you think about it.
Since the light transmission is much lower than PMMA, PC always has gray edges. Polishing is also difficult with PC as it also generates heat.

If the impact strength is the reason for the material, use impact resistant PMMA.

ralf

[Chip Owner]

The chips must cool the cut. Therefore, one mills with extremely sharp polished cutters with one flute. Good straight cutters for PMMA with one cutting edge are necessary for milling. We mostly use the ACRYLIC SINGLE FLUTE ROUTING TOOLS GENERATION 2 from crown-norge.no For diameters over 6mm we use the BALANCED single flute routing tools.


ralf

Can't speak for polycarbonate but on any plastic I cut, these are the same bits I use and would be reluctant to swap for anything else. I source them in the uk from LKHtools, slightly more expensive than most from the big online stores, but typically better value than many popular named brands. The latest GEN2 type is brilliant.

[dave benson]

This has been an interesting and informative thread.
I made this test to demonstrate what a bit of lube can do. (Mainly for my on edification).

I found a piece of material (a cover from an old machine bought at auction).
I did not machine the securing holes or pocket.
It has crazing on both the top and bottom faces, and the holes and pocket are opaque.

I did everything wrong to make an acceptable cut.

Wrong speeds and feeds.
Crappy work holding (sitting on parallels in the vice) so no support at all.
Wrong type of endmill (it was a well-used one for cutting AL, four flute).
No air blast.
Short of spinning the endmill in reverse, I could not think of anything else
to do wrong.

The only thing I did was lubricate the cut with straight dish washing liquid at
the start of the cut with my finger.

Tooling marks aside, the piece came out optically clear, I can see straight through it
(40 mm) to the woodgrain of the table.
I can even see the crazing from the top and bottom faces reflected in the side face I milled.
This is why it was hard to get a decent pic.

I’m not suggesting that you use the dish washing liquid, just that if you are still struggling
to get an optically clear surface to your satisfaction, after taking all of the above
advice (which is good) then it’s well worth considering.

Dave