Cutting .020 Sheet Aluminum on a CNC Router

[Mini-MillX2]

I have a 4'x8' CNC Router. I want to cut parts out of .020 and .024 4'x8' sheets. Can anyone recommend the best hold down method and router bits to use?

I was thinking of making a vacuum hold down table using pin holes like a air hocky table but is anyone using vacuum hold down on materials that you cut completely thur? In this case the bit would have to cut slightly into the hold down table destroying it over time.

As far as the bits go, I would like to use the smallest diameter possible and I would assume I have to use a down cutting bit to prevent lifting?

I just don't know how to get started with this, any help from those who do this for a living would be appreciated.

[in2steam]

Originally Posted by Mini-MillX2 I have a 4'x8' CNC Router. I want to cut parts out of .020 and .024 4'x8' sheets. Can anyone recommend the best hold down method and router bits to use? I was thinking of making a vacuum hold down table using pin holes like a air hocky table but is anyone using vacuum hold down on materials that you cut completely thur? In this case the bit would have to cut slightly into the hold down table destroying it over time. As far as the bits go, I would like to use the smallest diameter possible and I would assume I have to use a down cutting bit to prevent lifting? I just don't know how to get started with this, any help from those who do this for a living would be appreciated.

that would work, some people who do wood use a substrate like mdf, we use a woollike material on out plotter cutters, but I don think that will work. It has to be porous enough(plus maybe drill holes) for the vacuum to work. you can then skim it down as you wear it out.
You may want to ask in the wood router section and see what they say.
As for the bit that depends upon your cuts, and if you are doing very small parts you might not have a lot of luck, just remeber the smaller your bit the faster your spindle needs to go.
chris

[greg b]

I dont know if this will help or not mate,but what i do when making special gaskets out of alluminium or copper is to clamp them between two pieces of mdf or similar material and that works fine for me good luck.greg b

[cut more]

Mini-MillX2,
I cut aluminum on my router, up to 1/4" usnig double-sided tape to my mdf table. as for the bits, I use a 1 flute upshear bit from either Micro100 or Onsrud.
I do not have a vacuum table yet but this is the way to go for parts that are not too small, or you could make the vacuum table to seal around the edge of the part and use a gasket, so when you cut the material-the cut is out side the gaketed area.
The industrial routers like thermwood, motionmaster, use mdf on top of the vacuum plenum and pull right thru the mdf.
Hope this helps,
Cutmore

[Mini-MillX2]

Originally Posted by cut more Mini-MillX2, I cut aluminum on my router, up to 1/4" usnig double-sided tape to my mdf table. as for the bits, I use a 1 flute upshear bit from either Micro100 or Onsrud. I do not have a vacuum table yet but this is the way to go for parts that are not too small, or you could make the vacuum table to seal around the edge of the part and use a gasket, so when you cut the material-the cut is out side the gaketed area. The industrial routers like thermwood, motionmaster, use mdf on top of the vacuum plenum and pull right thru the mdf. Hope this helps, Cutmore

Thanks for the information. What bit size ane RPM do you or would you use for thin materials? I can't believe they can pull vacuum thru MDF, but that's what I thought they were doing.

[cut more]

I use an 1/8" @ 22,000 rpm. If I want a really smooth edge I go ~ 10 IPM. with an 1/8 doc. On thin materials you can travel faster.
I have seen the large routers with vacuum hold down cut mach faster due to no chatter of the material.
What size are your parts?
Cutmore

[Mini-MillX2]

Originally Posted by cut more I use an 1/8" @ 22,000 rpm. If I want a really smooth edge I go ~ 10 IPM. with an 1/8 doc. On thin materials you can travel faster. I have seen the large routers with vacuum hold down cut mach faster due to no chatter of the material. What size are your parts? Cutmore

The parts I want to cut are mostly large parts out of a 4x8 sheet of .020 Aluminum. I don't do any really small parts or artistic type parts.

[Greeves]

Originally Posted by Mini-MillX2 Thanks for the information. What bit size ane RPM do you or would you use for thin materials? I can't believe they can pull vacuum thru MDF, but that's what I thought they were doing.

Look around before buying MDF, you should find some ultra-light MDF, I just went through all this at work, got a new router 3 weeks ago, it's a multicam 3000 series with a 33 HP vacuum, well standard MDF don't work well even with a 33 HP pump, the ultra light works OK on .040 Aluminum or thicker as long as I keep my feeds down under 200 IPM. With my old router, I would use a spray adhesive to glue .020-.125 Aluminum to a sacrificial, I used a product called corex, it's about $10.00 for a 4 x8 sheet. With this setup I would cut with a .125 SF Upcut spiral bit 18,000-20,000 RPM @ 75-100 IPM, .250 SF upcut Spiral bit 18,000 RPM @ 102 IPM. 102 was as fast as the machine would go.

[Mini-MillX2]

Originally Posted by Greeves Look around before buying MDF, you should find some ultra-light MDF, I just went through all this at work, got a new router 3 weeks ago, it's a multicam 3000 series with a 33 HP vacuum, well standard MDF don't work well even with a 33 HP pump, the ultra light works OK on .040 Aluminum or thicker as long as I keep my feeds down under 200 IPM. With my old router, I would use a spray adhesive to glue .020-.125 Aluminum to a sacrificial, I used a product called corex, it's about $10.00 for a 4 x8 sheet. With this setup I would cut with a .125 SF Upcut spiral bit 18,000-20,000 RPM @ 75-100 IPM, .250 SF upcut Spiral bit 18,000 RPM @ 102 IPM. 102 was as fast as the machine would go.

Great information. What adhesive did you use and how difficult was it to separate the parts from the sacrificial? I tried to look for corex on the internet but I didn't find anything. What type of material and thickness is it? I think initially I'm going to have to go this route instead of using a vacuum table.

[Larry83301]

For thin material like that I would use an O-flute cutter. You will find tha it cuts clean and will NOT pck the part up from the table.

[Greeves]

Originally Posted by Mini-MillX2 Great information. What adhesive did you use and how difficult was it to separate the parts from the sacrificial? I tried to look for corex on the internet but I didn't find anything. What type of material and thickness is it? I think initially I'm going to have to go this route instead of using a vacuum table.

Sprayway #55, sometimes I would use 3M #90, removal can be difficult especially with the 90. Corex looks like corugated cardboard only it's plastic, it's used in the sign industry for those cheesy disposable signs that you see stuck into lawns. look for a company that sells sign supplies, Sun supply, montroy supply, Denco.

[Greeves]

Originally Posted by Larry83301 For thin material like that I would use an O-flute cutter. You will find tha it cuts clean and will NOT pck the part up from the table.

I'm guessing that would be a straight cutting bit, I may want to try one for thinner alum to try to get my feed speeds over 200 ipm without flinging parts across the room, its kinda funny this new table with the spindle up moves to the next part at around 1600 ipm and if anything has been lifted by a previous cut it don't hesitate to throw parts around, it moves too fast to try to get you hands in there to get things out of the way. I'm sure I'll get things figures out, hell I've only had the thing for three weeks now