[thecncnewcomer]

Hi,
I need to machine pieces like the one in the picture in acrylic (PMMA, Plexiglass).
http://www.cnczone.com/forums/attach...d=320754&stc=1

In you eperience, which would be the best machining strategy for this piece? Would this piece to requiere a special featured router or would it be possible to make it with common routers? It would be better to use a big router or a desktop router?

How could I avoid...
... the 0.1mm section gets break during routing process (tool, speed, RPM,...)?
... the piece gets warp after routing?

Thank you very much in advance.

[awerby]

If these are just cutouts, you're better off using a CNC laser cutter than a router for this. Lasers cut acrylic really well.

[thecncnewcomer]

Thank you for your reply Andrew! I need to mill first and then cutout each piece. I'd love to be able to do everything with a laser cutter/engraving machine but AFAIK laser machines are not accurate enough in the Z-Axis. However I still keep a little hope with laser cutters/engravers, it seems there's a chance to produce these pieces with laser machines by rastering 0.1mm layers. Do you have any experience doing something similar?

I guess the best bet is to mill the pieces with a CNC router and then to cutout them with a laser cutter.

[gfacer]

I'd use cast acrylic #1, mill to the 1mm depth and then up to the thicker section, so more surrounding material at that thin cut #2, over cut that pocket area and then profile around the final shape.

Even then the 1mm might be tricky, but you need the meat around it to have a chance, too much force on a thin brittle piece otherwise. A million little passes might work too, but I'd try the faster way with heavy cuts first.

Sent from my ASUS_Z00TD using Tapatalk

[Louis_Cannell]

I mill acytlic regularly and get good results, 6000 rpm and 2000mmpm with 6mm 1-2 flut cutter your main problem is holding down thin stock as acrylic tries very hard to lift with any helix in the cutter, if securely held down double sided tape (Difficult to remove) preferably a vacuum I cannot see a problem milling these. May need to set up small vacuum jig to attach vacuum cleaner if nothing else available.

[elfrench]

I'd try using a vacuum first, as the .1mm will be hard to release from tape and the tape may be too soft to get an accurate cut that thin. Another option would be to glue it to a sacrificial piece. You would need a glue that's dissolvable and won't damage the acrylic. Unfortunately, super glue won't work.

[thecncnewcomer]

Thank you very much for your advices. It seems the vacuum table is the way to go. I try it with glue and double face tape and both affected accuracy in the Z-Axis, however I didn't have any issues when removing the pieces. Other alternative would be to make a holding device which keeps pressing everywhere not machining be necessary, avoid cutting with router and doing it later with a laser cutter. What do you think about this solution?

[Louis_Cannell]

cutting contour with laser after machining probably good idea, consider making a vacuum jig route a vacuum jig out of something to hold blanks and use simple vacuum claeaner for suction.

[thecncnewcomer]

cutting contour with laser after machining probably good idea, consider making a vacuum jig route a vacuum jig out of something to hold blanks and use simple vacuum claeaner for suction.

What do you think about this design?
https://dl.dropboxusercontent.com/u/...umtable-1.iges. (2 holes should be drilled on X:200.5mm Y:0.0mm and X=-200.5mm Y:0.0mm for both pressure regulation valve and suction.
https://dl.dropboxusercontent.com/u/...umtable-2.iges. This piece should be glued to the other piece and flattened if necessary. I'd consider a light glue if it will be used as a sacrifice surface for an easy removing in the future.

BTW, if someone use these files please send me a picture.

[thecncnewcomer]

Here's a different model (easier and faster to machine but maybe less effective):
https://dl.dropboxusercontent.com/u/...mtable-2b.iges

[warrenb]

I see what you're doing there... Reeds.

I've made reeds before. Acrylic never worked for my doule reeds. but... Styrene worked quite well (not nearly as good as cane reeds).

Anyway...

For something like that. Rather than try to surface cut your angled tongue put the entire reed at the angle the tongue is suppose to be. That way you only flycut the angle. Experiment with cutters. Sharp sharp sharp. BUT, even then. Use a sanding stone for your final pass if not the whole thing. Save the surface cuts to shape the rest of the reed. You want the tongue as flat as possible. Also. You probably won't have luck cutting them individually. Make a vacume fixture that will hole down a strip, say 200mm. Cut the outlines with tabs then hand finish the tabs.

You're going to need a VERY NICE fixture. Mine is made from aluminum and I use a refrigeration servicing vacuum pump for hold down.

Good luck.

[Louis_Cannell]

One thing I havent mentioned that may be worth a try is simply use a vertical jig, A solid 90 backing and mill the graduation vertically, using climb milling with piece held vertically using whole length of a solid milling cutter, this may work as have seen this done with aluminium to 10thou for a shim.

Solid 90 degree backing 6mm or greater x 20mm flute, and mill from 0.1 cllimbing up object is most stable method for thin cuts in other materials, then trim contour with laser.

[thecncnewcomer]

I see what you're doing there... Reeds.

I've made reeds before. Acrylic never worked for my doule reeds. but... Styrene worked quite well (not nearly as good as cane reeds).

You're right! Acrylic seems to be OK for single reeds. In the link below you'll find an audio clip (me playing on one of my hand finished prototypes):
https://dl.dropboxusercontent.com/u/...120-1M-252.mp3

[thecncnewcomer]

I mill acytlic regularly and get good results, 6000 rpm and 2000mmpm with 6mm 1-2 flut cutter your main problem is holding down thin stock as acrylic tries very hard to lift with any helix in the cutter, if securely held down double sided tape (Difficult to remove) preferably a vacuum I cannot see a problem milling these. May need to set up small vacuum jig to attach vacuum cleaner if nothing else available.

It seems ball cutters would give a better finishing, probably 6mm diameter should be OK. What do you think about to use or not to use layers? How many layers for going from 4mm to 0.1mm?

[Louis_Cannell]

It depends a lot on machine but 0.5 to 1mm would be my starting place, I tried a similar cut just out of interest using side of 6mm end mill almost full length of flute as described in previous post mounted at 90 deg in vice hanging out of the side with solid steel bar backing and got far better result than end milling could manage, using climb milling rather than conventional.