cutting thin materials and holding them down.

[knight_toolworks]

I have been cutting a lot of thin materials lately and I thought I would share some of the ways I found to deal with it.
The biggest problems with thin materials is that the vacuum does not really help when they want to lift up.
when I am talking thin I am thing maybe 3/16" and under. the thinner it is the worse the lift up problem. I really had to struggle till I got the hang of it with some .03 plastic.
a downcut bit would help but for plastics they cause the shavings to stick to the edge badly. but for thin woods it is a good choice.
so I am finding for the thinner plastics a 1/8" straight bit works pretty well. it leaves some shavings stuck to the edges but that keeps the part in place. so that lets you get more parts per sheet. you only need a small amount of uncut plastic between parts and they will hold in place.
cut speeds vary with materials of course. I found you can't cut 1/8" acrylic faster then about 60 ipm or the bit will break if your doing a single pass. but I have cut sintra and such faster.
but since changing over to the straight bits I have hardly lost any parts even when cutting a few hundred parts on a sheet like the picture below.
the time saved not having to glue down acrylic is really paying for it's self. you do waste a bit of material to get the spacing but it pays for no lost parts and no prep work.
I have not compared cut quality but it seems ok.
I found even trying to use two passes to cut thin material with a upcut can lift the material off the table on the first pass. Once that happens shavings get under the part and it won't lay back down.
so far I have been cutting at 8k and that seems fine.

http://i154.photobucket.com/albums/s266/knighttoolworks/posting/f08ec900.jpg
http://i154.photobucket.com/albums/s266/knighttoolworks/posting/rings.jpg

[frankwilliams]

I cut a lot of materials for the local sign guy including tons of white polystryrene for stencils. I have found that a miniature envraving or color core v bit works better than anything. No lifting, no pulling, no melting, 3ips no problem. For Sintra and acrylic, I still like the upcuts the best, but thats only if you leave some tabs and space between parts. Turns out to be the best finish and the least cleanup for me. Just 2cents from my experience. (Worst part about all this stuff if the staticly magnetic chips everywhere!)

[khaos]

I cut a lot of materials for the local sign guy including tons of white polystryrene for stencils. I have found that a miniature envraving or color core v bit works better than anything. No lifting, no pulling, no melting, 3ips no problem. For Sintra and acrylic, I still like the upcuts the best, but thats only if you leave some tabs and space between parts. Turns out to be the best finish and the least cleanup for me. Just 2cents from my experience. (Worst part about all this stuff if the staticly magnetic chips everywhere!)

I am interested in creating some stencils. Can you expound on your process maybe with links to specific bits? :)

Thanks,

[knight_toolworks]

the static can really suck. if you wipe the sheet with a bounce sheet it helps a fair amount. I can see using a v bit for the job. myself I don't like using tabs I always miss some and then break edges.

[frankwilliams]

Sorry this has taken so long for me to reply.

Disclaimer: This is all just my opinion based on 3 years of cutting for the local sign shop. I am only telling you what works best for me.

For cutting the polystyrene, I ususally cut the 0.050" thick stuff as it is a bit more rigid.

For bits I have tried vbits to 1/64" endmills and so far the best thing has been a color core engraving bit like the one from centurion tools (the link is too long to post, look at v-bits and choose color core from the side bar). A half round engraving bit works well too. I usually choose a 0.0313" endmill from my tool list in Vcarve/aspire, and then process the toolpath as an inside profile of the letters and I cut 0.010" deeper than the material thickness ( this takes care of any inconsistencies in your spoilboard).

A freshly surfaced table top is not necessary, but will make cutting a lot easier as its harder to break the "seal" around the material. Feed rate of 2.5 - 3.5 ips works well for me, 16000 rpm. You will know when you get the speed right because you will be left with a smooth edge. Too fast and it will be rough, too slow and the plastic will be really rough due to chips melting back to the cut edge. You can clean up any rough bits with your fingernail.

The part that I still have trouble with is that I have yet to be able to cut this stuff without removing the "fingers" from me dust skirt. They always wedge themselves under the material and break the vacuum seal. Doing it this way makes a mess with chips, but I haven't ruined a sheet since.

When designing your stencil, you will have to add "tabs" to your artwork and lettering so as closed letters and objects still have detail, for example you need to put a tab to support the triangle in the middle of a capital A to avoid it looking like an arrow. I usually do this manually in Vcarve by welding and subtracting little "boxes" to the vectors as needed.

Steve is right about the bounce sheets, I've walked in to the shop with one in each hand swinging them like nunchucks and just watched the plastic fall of the machine. Seriously though if you have bits of plastic or foam sticking to the machine, wipe with bounce and then vacuum it up. You do not want this stuff getting into the racks, router intake etc.

Finally always, always, always wear a good respirator. I don't have the scientific proof to back this up, but cutting plastic is nasty, even if you aren't melting it. If even 1/100th of the stuff that ends up on my coveralls got in my lungs, I'd be in serious trouble.

Good luck, hope this helps a bit, and feel free to let me know if I have left anything out.

Frank

[khaos]

Thanks. :)