[WoodSpinner]

Hi, I reciently got interested in making lithophanes, as a start I found some .180"thick white opaque plastic to try using. My first attempt came out impressively, the image is great, no problems with the plastic melting as I cut the litho. However when it came time to cut it out, like an idiot I snagged a .25" downspiral and set to cut at .07" at a time, at 30 ipm it made the first go round impressively, then I tried to increase the feed to 60 and thats when it started. in the end I had to hand plane the edges smoothe again. The plastic had melted and bubbled up around the edges of the piece and I had to stop it before it was done creating even more material to clean up.

I'm looking for suggestions for improving my cutout quality, I wondered about using a smaller straight fluted cutter, and possibly even cutting one go round at a time. should I reduce the speed or increase it, I'm using a pc 690 router at 27000 rpm with no way to reduce the speed.

any and all suggestions would be appreciated.

John

[aarongough]

If you're melting the plastic then your feedrate is too low. 30IPM at 27K RPM is very, very, slow. Whats happening is that the cutting faces of the tool are rubbing against the plastic rather than cutting into it, this creates heat and melts the pastic.

You want to get your 'chipload' higher. The chipload is the amount of material removed by each cutting edge on the tool.

30IPM / (27,000 RPM x 2 flutes) = 0.00055" Chipload

I usually cut plastics at 160IPM @ 16K RPM.

160IPM / (16,000 RPM x 2 flutes) = 0.005" Chipload

So, given that your router is fixed at 27K RPM your feedrate should be something like 300 IPM to get near the same sort of chiploads that I'm using.

Also using a downspiral may cause issues because it will make chips pack in at the bottom of the cut, if the chips are getting pushed around by the endmill then they may eventually melt.

[keebler303]

With a downcut bit you MUST cut all the way through and you MUST have somewhere for the chips to go (like a space under your cut). As it is now, your bit is shoving the chips into the plastic, making them bind and create heat which welds them together. Once that starts, you are done for. Get an upcut bit and feed it as fast as you can go. 27000 is screaming and you need to maintain a good sized chip so you are cutting instead of rubbing. Slowing down the cutter would be better but speeding up the feed will help.

27000 with a 2 flute cutter is 54000 flutes per minute. Divide 30 IPM by 54000 and you get about .0005". You should be at least .005" (300 IPM) and possibly double or triple that depending on conditions.

If you are going to be doing a fair amount of this, get one of the "0" flute Onsrud cutters meant specifically for plastic.

Matt

Edit: Dang it! Too slow!

[aarongough]

With a downcut bit you MUST cut all the way through and you MUST have somewhere for the chips to go (like a space under your cut). As it is now, your bit is shoving the chips into the plastic, making them bind and create heat which welds them together. Once that starts, you are done for. Get an upcut bit and feed it as fast as you can go. 27000 is screaming and you need to maintain a good sized chip so you are cutting instead of rubbing. Slowing down the cutter would be better but speeding up the feed will help.

27000 with a 2 flute cutter is 54000 flutes per minute. Divide 30 IPM by 54000 and you get about .0005". You should be at least .005" (300 IPM) and possibly double or triple that depending on conditions.

If you are going to be doing a fair amount of this, get one of the "0" flute Onsrud cutters meant specifically for plastic.

Matt

Edit: Dang it! Too slow!

Well you added the part about cutting all the way through in a single pass with downspiral bits. I will admit that I haven't used any downspirals on my machine so that was something that I missed!

[aarongough]

As a pointer: this is the type of tooling Matt is referring to when he says O-flute

Solid Carbide Spiral Plastic 'O' Flute -ToolsToday.com- Industrial Quality Solid Carbide Bits

You should buy up-cut bits for the most part.

Dimar also make some at reasonable prices if you have a Dimar stockist nearby.

[WoodSpinner]

Thank you all for the quick and timely responses. I was afraid the proper solution to this issue would end up being out of my reach. My machine used single start 1/2" 10tpi screws and I'm afraid to try cutting any faster than 60 ipm, I'm thinking it would be best if I try using my best straight cutting bit(1/8", biggest I have) and runnning 60 ipm, then I'll manually edit the gcode to do one pass at a time allowing it to cool between passes and see how it goes. I really hope I can find a solution that will be workable within the limits of my machine and on hand tooling, at least until I get the first one sold and can buy an upcut spiral bit.

John

[keebler303]

As a pointer: this is the type of tooling Matt is referring to when he says O-flute

Solid Carbide Spiral Plastic 'O' Flute -ToolsToday.com- Industrial Quality Solid Carbide Bits

You should buy up-cut bits for the most part.

Dimar also make some at reasonable prices if you have a Dimar stockist nearby.

Those are the ones!

[aarongough]

Thank you all for the quick and timely responses. I was afraid the proper solution to this issue would end up being out of my reach. My machine used single start 1/2" 10tpi screws and I'm afraid to try cutting any faster than 60 ipm, I'm thinking it would be best if I try using my best straight cutting bit(1/8", biggest I have) and runnning 60 ipm, then I'll manually edit the gcode to do one pass at a time allowing it to cool between passes and see how it goes. I really hope I can find a solution that will be workable within the limits of my machine and on hand tooling, at least until I get the first one sold and can buy an upcut spiral bit.

John

Hey John!

Can your machine rapid at 160IPM or so? If so you should be ok to cut at that speed, you may just have to reduce the depth of cut to compensate. When cutting aluminum I feed at 120IPM, but only take a cut of 0.010"

Even when cutting wood you'll want to be able to use feedrates of 100+ IPM. My machine also has 1/2-10 Leadscrews and I am able to cut at 160IPM with no problems (It's a Probotix Fireball V90). If you can't hit those sorts of feedrates you might want to look at changing the leadscrews in your machine to multi-start screws as you will often want higher feedrates than 60IPM.

[aarongough]

Thank you all for the quick and timely responses. I was afraid the proper solution to this issue would end up being out of my reach. My machine used single start 1/2" 10tpi screws and I'm afraid to try cutting any faster than 60 ipm, I'm thinking it would be best if I try using my best straight cutting bit(1/8", biggest I have) and runnning 60 ipm, then I'll manually edit the gcode to do one pass at a time allowing it to cool between passes and see how it goes. I really hope I can find a solution that will be workable within the limits of my machine and on hand tooling, at least until I get the first one sold and can buy an upcut spiral bit.

John

Lastly, if you really can't get your machine to feed above 60IPM then there's still some things you can do.

1) Use only single-flute tooling. Like the O-flute tooling Matt mentioned and that I linked to.

2) Get a variable speed router or use something like the SuperPID to control your current router.

I use a Dewalt DWP611 router and really recommend it. It has an electronic spped control that maintains constant spindle speed under load, and it goes down to 16K RPM. On your machine that's still only 0.003" chipload, but that's miles better than what you have now.

[tatinc2000]

You coul always use a router speed control. I use one on my router table. They are only $30 from mlcs. http://www.mlcswoodworking.com/shops...d_control.html

[tatinc2000]

You coul always use a router speed control. I use one on my router table. They are only $30 from mlcs. http://www.mlcswoodworking.com/shops...d_control.html

[aarongough]

You coul always use a router speed control. I use one on my router table. They are only $30 from mlcs. MLCS Router Speed Control and Billy Pedal Foot Switches

That's a really good cheap option too. One thing to note is that you will lose torque at low speeds, however this should not really be an issue if you're only taking cuts 0.07" deep.

[louieatienza]

I try and use single flute bits anything 1/8" or smaller if I can. Downcut spiral is probably not a good option on plastic because you have nowhere for the chips to go (unless you cut full depth and you have a fixture that allows chips to go down.) Even a single edge straight flute would be better, but your leadscrews are what limit you in terms of speed.

What you COULD do is make sure you're climb cutting; as this tends to move chips back and away. Use compressed air to clear chips away. If you're doing four passes to cut, you can make your first pass say .060" away from your cut line. Then make two passes .040" from the cut line. Then three passes at .020". And finally four passes at the cut line. This will give your bit clearance for the chips, as it won't rub on one side. If your spindle is strong enough you can just do one pass each, stepping down AND in with each pass. So your first pass would be .060" away and .045" doc, then your second would be .040" away and .090" doc, and so forth. You'd have to either hand-code this or use the offsets in your CAM or just simply draw four boxes and make toolpaths for each. You can keep them all separate so that you can do a chip cleanup between each pass.

There's a guy on eBay named drillman1 who sells 10-packs and singles of Kyocera 1/8" 1-flute spiral-O bits, for like $4.00 each or 10 for $35. There well worth it and I use them on both plastics and aluminum.

[ger21]

There's a guy on eBay named drillman1 who sells 10-packs and singles of Kyocera 1/8" 1-flute spiral-O bits, for like $4.00 each or 10 for $35. There well worth it and I use them on both plastics and aluminum.

1/8"(.1250") single flute carbide endmills for plastic | eBay

then I'll manually edit the gcode to do one pass at a time allowing it to cool between passes and see how it goes

That won't help at all, as the melting happens instantly, and has nothing to do with heat from the previous pass.
What I would do, is but the bit I linked to above. Then, cut a profile pass .05" oversize, but not quite all the way through. Don't worry about melting.
Then go back and profile the actual size with a climb cut, and you shouldn't have any issues.

A cheap speed control will also help immensely. If you want no melting at all, you need to get down to around 8,000 rpm with your 60ipm feedrate, and you'll still need a 1 flute bit.

[louieatienza]

That won't help at all, as the melting happens instantly, and has nothing to do with heat from the previous pass.
What I would do, is but the bit I linked to above. Then, cut a profile pass .05" oversize, but not quite all the way through. Don't worry about melting.
Then go back and profile the actual size with a climb cut, and you shouldn't have any issues.

The reason for stepping down and in was for ensuring that (except for the first shallow pass) the bit is only touching one side of the kerf, which will prevent rubbing,heat buildup in the bit, and chip melting.

Doing it separately allows one to totally clear any chips without the router in the way blowing them around. From my experience I've never seen a bit just instantly heat up and melt plastic. The bit just gets hotter and hotter till it reaches the melting point of the plastic. Then everything goes downhill fast. But if all particles are removed from the kerf, and a method is in place for removing subsequent particles and reducing bit rubbing, the bit will heat up less.

Admittedly, I rarely have this problem, using a dust shoe with the climb cut passes gets the chips out well; and I have speed control.

[WoodSpinner]

Thanks again for all the information. Starting off, I'd like to say that my machine has been morphing ever since I first built it from plywood, 1x2s and roller skate bearings.

Here is a link to a video of it after the first morph, you will see that the z axis has been built from 1/2"aluminum, steel box beam and angle iron. Oh and of course my first bought part, a k2cnc router mount.

My3DCNC.mp4 video by woodspinner1 - Photobucket

dont forget to turn down the volume before playing it.

While it was in this state, I started making wooden boxes with sports logos on them to make extra money to spend on it and started buying parts from CNCRP, and some steel and built a gantry beam with proper z stage on it. I didnt have enough money to buy multi start screws so went with the ebay el cheapos.

I since have read up on copyrite laws and figured it wasnt worth the risk I shut that product line down.

If I can interest enough people in these lithophanes and light boxes, I'll be continuing the upgrades, but until then, I dont even have money to buy proper bits or a speed controller(drooling for a spid). I do however have them in the wish/someday list.

here is a link to a pic of my first lithophane w/light box

http://i338.photobucket.com/albums/n...1/IMG_0150.jpg

I made that as a gift to the lady that runs our local coffee shop, she has had it on display ever since and I'm starting to get requests for them. Here is a link to a shot of the one I cut today, havent built the box for it yet.

http://i338.photobucket.com/albums/n...IMG_0003-1.jpg

So once this one is complete and delivered, I'll go to ebay and get some decent bits to make this at least bearable.

btw, I did the cut out in two passes with a down spiral(I know bad choice)fishtail bit stopping after first pass to dig out all the bits of loose plastic, was very suppprised to see that the melting stuck mainly to the outside and left my part alone. It only took a razor blade to remove the onion skin that was left.

Thanks again for all the help, feel free to keep it coming, I'm always wanting to learn more.

John

[WoodSpinner]

Thanks again to everyone for all the good info. I sold that first one, and ordered a few single edged o-flut cutters for my cutouts. Next one I sell will buy me a speed control in the hopes that it will improve my cuts.

I was suprised how much it melts doing a cutout but I dont have that problem with my single edged 1/8th" round nose bit.

Just to see if it will improve the clarity of the result, I ordered a 1/16th" ballnose em from bitsbits.com .

John

[keebler303]

From my experience I've never seen a bit just instantly heat up and melt plastic.

Try using a downcut bit at 27000 RPM. The plastic is not melting from the heat of the bit, it is melting from the chips being shoved into the bottom of the kerf by the bit. This will give you near instant melting. If you're doing it right, the cutter and the workpiece will stay relatively cool, with most of the heat leaving in the chips.

Matt

[WoodSpinner]

Try using a downcut bit at 27000 RPM. The plastic is not melting from the heat of the bit, it is melting from the chips being shoved into the bottom of the kerf by the bit. This will give you near instant melting. If you're doing it right, the cutter and the workpiece will stay relatively cool, with most of the heat leaving in the chips.

Matt

my new cutters came in today, so I'll be trying an upcut 2flute this time. I also just ordered a router speed controller, its not an spid but I dont think these cuts require all of the torque this router puts out anyway.

John

[keebler303]

John, just keep an eye on the temperature of the router. It is designed to have it's cooling fan running at full speed. At low speeds the air flow is significantly reduced so it may overheat if you go too slow or try to get too much out of it.

Matt