Feed and Speed Rates for ACM

[treverinterstate]

I'm trying to cut Aluminum Composite Material. I'm using an Onsrud 63-614 bit. It's a small 12"x7.5" mailbox sign I just want to cut out. I called Onsrud and they said do a 12000 RPM and Feed Rate of 54 on the small sign but it just rips the aluminum to pieces, it doesn't cut it clean. I tried 18000RPM and Feed Rate of 85 and 50 with the same results. I tried it on 24000RPM and 85 feed rate and broke the bit. I tried one on conventional and a few on climb. I don't know how to get it to cut it and look good. I had them all set to a smooth ramp of .25" and I tried them in 1, 2, and 3 passes still no luck. My spindle has a mister. I feel defeated as I have no idea how to make it work and I've searched the internet only to find people have made it work with similar settings. I'm attaching the aspire file. Any help is greatly appreciated.

[Adrian]

I've only ever cut ACM once and I used the settings from here - http://cncfaq.us/ufaqs/what-is-the-corr ... -maxmetal/ - which worked well. I expect my machine could have done it faster with a larger pass depth but as, it was a one off (I use the fully plastic laminates mainly), I left it at those settings.

I didn't use the same make of bit but it had the same specs. It was a single flute O spiral from Wealden Tools here in the UK.

I did have one small section that did show a bit of tearing like yours and that was caused by vibration in the piece as it neared the end of the cutout. Might be worth checking that the material is held absolutely rigid and it isn't vibrating at all.

[treverinterstate]

Thank you Adrian! I will try this. I have a vacuum table but it didn't hold the signbond down very well so I screwed it in to the spoilerboard but only in two diagonal corners. Maybe it did vibrate too much. Thanks for your input. You have been very helpful!

[martin54]

what thickness? Guessing 3mm or 1/8 inch, sorry no software on this machine to check file. I cut this quite a bit being a signmaker & never have problems, good hold down is important as Adrian has said, it tends to bow up but a good vac hold down system should hold it ok that is what the larger Sign manufactures use with their machines. I use same spec bits as well single flute but rest is on computer at unit & can't remember. normally use a spiral ramp to cut but my plunge rate for the bit is set at almost the same value as the feed rate.
Make sure you are clearing the chips to prevent re welding

[treverinterstate]

I guess it's considered 3mm. It's .13 inches thick. I tried the settings in the previous reply with no luck. It broke my bit again. So frustrating that I can't figure it out!

[Adrian]

If it's breaking bits at those speeds and depths I would think it has to be vibration/movement causing it. I can snap a 1/8" bit even in 3mm MDF if it vibrates.

[Mobius]

Do you have any down-cut bits? It may help with vibration by pushing the material down against the spoilboard, and help make a cleaner cut on the top surface. For smaller signs like that, I usually use some masking tape and CA glue to help stick it down nice to the spoilboard.

I find both the aluminum and plastic core to be very soft, making it a challenge to cut cleanly.

[treverinterstate]

I think all the bits I have tried are down cut. But they are all 1/8" dia. except one is 3/16" dia.

[Adrian]

The Onsrud 63-614 is an upcut bit.

[martin54]

Bits I use are generally upcut, 3mm diameter most of the time for ACM, single flute with high helix angle, designed for general cutting of materials like aluminium & acrylic.
Think Adrian was probably correct when he said it was most likely down to vibration rather than anything else

[treverinterstate]

Adrian you are right. I had it in my head they were downcut, but they are all upcut... oops. I've secured it pretty good now and its still ripping the top layer apart. I'm guessing a downcut bit would be more sufficient in preserving the top layer of aluminum and maybe like 1/4" in diameter would work better?

[Adrian]

A downcut will give a much better top edge and will help hold the piece down. The downside is that it will build up chips in the slot that could cause problems depending on feed rates, pass depths etc.

There is a really tricky to cut recycled plastic that I use and what I do with that is to do one toolpath to half depth with a downcut then switch to an upcut for the final pass. If you run into problems with a purely downcut approach it might be worth considering that approach. If you've got a compression cutter then you could use that with leads.

[BradyWatson]

You've got a few things going on from what I can see so far...

First, make sure to remove the plastic protective layer from at least the top side. It has a tendency to melt and gum up the bit in some cases. It IS designed to be left in place so the parts don't get marred in transit, but it creates problems for a lot of people. Remove it after you've stuck it down to the table.

You're not holding the material down well enough. Since you probably don't have vacuum, cover the back of the material where you are going to cut with masking tape first, then cover it in carpet tape - it's double sided and has fiberglass mesh running through it. Stick that puppy down to a clean spoilboard. STOP using screws on metal or metal clad sheet goods. It 'dinks' the sheet and causes it to distort no matter how careful you think you are doing it. Vibration MUST be eliminated or all your cuts will be junk - and bits will snap. The masking tape eliminates the need to remove the carpet tape residue on all but the edges...be sure to use it.

You are feeding the tool too slowly - the chipload is way too light. Keep in mind this stuff cuts like butter with regular woodworking tools like a Skilsaw or chop saw etc. It is a bit funky in the sense that it is aluminum skinned, but the bulk of the material is polypropylene. I would suggest using a single flute spiral-O tool (63-614 is fine for this), and set your cut speed to somewhere in the 75-90 IPM range @ 13,000-15,000 RPM. Create a toolpath that cuts it in 2 passes using a spiral ramp just to be sure nothing moves.

Just like any other material, you should be getting CHIPS off of the tool as it cuts & not dust. You're looking for sparkly black soap shavings/curls. Incidentally, 'dust' collection will help cool the bit and keep it from shmearing like your pics show.

[treverinterstate]

I've tried a number of combinations for speeds and feeds with hardly any luck. I've uped the tool size to a 1/4. Tried both upcut and downcut with little luck.

Currently if I cut it twice once on a downcut and come back with the upcut tool I can get it to cut out. It leaves a some metal spurs on the side of the sign but I can take my utility knife and clean it up so that it looks ok. I've attached a picture of the cut out sign. I was just hoping this would cut smoother. All the videos online show that it cuts so smooth. I'm using the Amana tools series specially designed for ACM now. Its a 51502 and 51402. The recommended feed settings for the tool is 18000RPM at 80IPM which didn't cut good either. The same tool with a zinc coating has a recommened setting of 18000RPM at 140IPM so I cranked mine up to 180IPM and 20000RPM and still leaving some spurs but getting it to cut smoother. I was a little scared to go any higher.

Thanks to everyone for all your help!

[treverinterstate]

Figured out the problem. My spindle wasn't spinning. I was literally just dragging the tool thru the material which is why I couldnt get it to to work. Dunno why my spindle quit but I got it working now.