I’m looking at cutting thin polycarbonate sheeting; 1mm-1.5mm
I’ve had a go with a 2.6mm single flute bit with reasonable results, but I feel like there is a bit of flex happening, increasing the cutting speed makes it worse and lowering cutting speed makes the edges gouge a bit.
I’m cutting record blanks so they need to be reasonably circular, my previous attempts are leaving me with blanks that have rough edges and aren’t always circular.
I’m considering trying to cut it was a 2.8w laser, but I’m not sure that’s going to be any better and I’m a bit suspicious about the fumes.
Has anyone else had any experience cutting Polycarbonate?
Polycarb can be laser cut. It just stinks, and the fumes can foul the optics if there’s not enough ventilation. Not sure what the magic recipe is for cutting it with a router though. When I did my acrylic parts I used a trochodial cutting path, and that gave some really good edges.
If you do want to cut it with the CNC make sure to use a down cutting bit on thin material. But that is pretty thin, laser really might be the best tool for the job.
Well, you can cut a 2X4 with a butter knife, just depends on how long you want to wait for it.
Honestly, I’m not sure how well it would cut.
Okay, reading up on it some more, you’ll want to cut it with a router. To cut the clear stuff, you’ll need a higher wattage co2 laser. The little guys most of the folks here are attaching to their mpcncs are blue(uv) lasers and don’t have to power to cut clear polycarb very well.
Curious what Polycarbonate cutting settings are working for your MPCNC / LR3 based CNC builds? Guessing slow low-speed deep trochoidal cuts with 1 flute carbide 1/8" bits, ideally down cut, but up cut can work too for thicker less flexible stock? With great Vac and/or air assist to clear chips.
Currently planning to use my cast acrylic settings (thanks to the Acrylic topic) as a starting point (LR3)…
These are my settings, I think I’m pretty close to the limit - I think I turned them down from 5000mm/m but to be honest, I think that could even be wrong. I’ve had a bit of a nightmare cutting sheets this week - it’s been 28-32 degrees, so I’m not sure if that’s coming into play. Table is also a mess, and I think my belt tension has gone. The SKR is also playing up, but I did cut 30+ sheets at 5000mm/m - I do wonder if it’s true 5000mm/m as I’m only really cutting curves.
The bit I use is a cheap 3.18mm two flute straight cut, I found the upcut bits tend to pull the entire sheet up, the two flute leaves the sheet in place (to an extent) and I clean up the edges on a lathe afterwards - the edges are not very tidy at all.
It does not really matter much as long as there is one big piece still on the table it can suck to. I learned that using tabs makes it easier, even though you might have a vacuum table.
Anyone notice down cut bits causing their LR3 Core to lift rather than fully cut?
Single flute up cut (from V1E) was pulling up Polycarbonate panels, had to blue tape and glue down to prevent lift. Time consuming, so…
Tried new 1/8" down cut trochoidal 20mm/s when space permits. Works great without tape+glue, am just screwing ~2’x4’ panel around perimeter. However…
Noticed for small holes, using non trochoidal, that the holes are not fully drilled. Instead LR3 Core lifts up 0.5 - 1.0mm from the gantry, rather than fully cut down into the 1.5mm polycarb panel. Bearings rotate when Core is moved side to side, so I thought Core was snugged up ok, but seems there’s still enough of a gap somewhere that allows Core movement, slop?
Never notice this with up cut bits that pull into stock.
Like that down cut pins the stock down. Given LR3 Core isn’t fast to swap or print, am concerned about over tightening and cracking the core. Tempted to just create toolpaths that make 1mm extra deep cuts when non trochoidal. Can also slow feedrate to allow more time for sinking/plunge maybe?
In my tries to fix my wobbling core I really, really tightened the bottom and top (the ones you are only to seat… :P) clamps. Nothing bad has happened so far.
I’ve noticed the polycarbonate sheet seems to have some give…
A lot of the time I need the depth of cut to be .25-.5mm greater than the thickness of the 1.2mm sheet, it’s definitely scarring the table, but she the majority of my cuts are the same over and over again it’s not too much of an issue.
The big issue I’m having is with the SD Card not reading correctly - it only reads one I have at the moment, and my cuts seem to be behaving erratically. I’m going to run from an octoprint server and see if that corrects it.
I could have sworn you made a topic somewhere about speeds and feeds, but I can’t find it, so I’ll reply directly to this topic since it’s in regards to cutting polycarbonate sheet.
I’ve just had to recalibrate my accelerations a bit to cut 1.2mm polycarbonate sheet, I should really save the changes in the g-code itself as the cuts are fairly imprecise… but I’ve been cutting today with this settings;
1.5mm DOC (so as to make sure the bit goes all the way through) I’m still scarring the table, but the scars are all repeated, so it’s no biggy.
Taken from the LCD itself;
1000mA Driver current all 5 steppers
Accelerations
100 Print Accel
3000 Retract Accel
1000 Travel Accel (I think this is the only important one in regards to the LR3)
Max Feed Rate
X 10000
Y 10000
z 800
Max Acceleration
X 600
Y 600
Z 800
In ESTLCam I’m cutting at 11000mm/m on the X+Y and 800mm/m on the Z
I’m using a 3.175mm Two Flute bit with a 45° Plunge Angle
Helical drill for my centre holes (7.2mm)
Speed 6 on the RoutER11
it helps having a sharp bit, the first bit I was using was a little blunt and it was popping out of the cut.
and here’s a video;
I’m guessing the 11000mm/m in ESTLCam may not actually be the speed of the cut due to the max speed being set at 10000mm/m in Marlin.
Big changes from last time has been cable/vacuum management, only the stepper motor cable is travelling along the gantry now, the vacuum being set up in the ceiling.
It’s cold here atm, so I’m wondering if the max current will also be temperature/season dependant.
Keep in mind I clean the centre holes out with a drill bit and then tidy the edges on a modified wood lathe, so surface finish and accuracy aren’t at the forefront of these cuts!
this thread popped up a lot in my google searches on the matter of polycarbonate feeds speeds and lowriders so posting it here: just now on my LR3 with kobalt router maxed out on rpm milling 0.177" (~4.5 mm) polycarbonate had perfect first attempt with no melting issues using an O flute single flute upcut from oliver tool on ebay 3.175x25 “upcut single bit” . maybe ryan sells one like this too i haven’t looked yet but they are affordable and possibly worth selling if not. China Customized Single Flute Upcut Bit Manufacturers Suppliers this is the mfr page
1000mm/s and 0.255mm depth of cut. no melting just tiny little 3/4 of a full spiral chips cutting enclosure panels for a 3d printer. might have been able to push it to 0.33mm depth per pass but i was fine with this working so damn well for only my 3rd time milling solids and most expensive material on the lowrider yet. i think even with a bit like this that is sold as wood and plastic cutting with the polycarbonate and a lowrider you probably shouldn’t do too deep per pass… the feed of the bit though needs to remain high from everything ive seen. i used some guidelines from the carbide 3d video about polycarbonate with a bit of the same diameter.
anyway ymmv … or as i say YAYOW. … you are your own warranty.
oh… additionally for anyone who’s a noob like me… make sure your plastic sheet is laying very flat so that an arch in the plastic sheet isn’t sticking up too high. i broke one of my two o flute bits that way. ended up keeping track of the tool path and setting some small plate weights from my rack on the areas where the tool wouldnt be
I learned that using tabs makes it easier, even though you might have a vacuum table.
