Aluminum chatter I believe

[darkclown]

I was hoping someone here could help me with my problem. I have been making wooden Fidget Spinners for awhile now but have decided to try and make some out of 6061 aluminum. The problem I'm having is I believe called chatter on the piece. I included some pics so can see what is going on. I don't know if I need to slow the feed rate down or maybe slow the rpm down.

I'm using a 4mm carbide single flute endmill and I'm profiling through 1/4" 6061 aluminum.

I'm using compressed air as a coolant no fluids.

doc .2mm
feed 540 mm/min
rpm 27000
stick out 15mm
These are the settings I used that I got from G-Wizard.
Any help would be greatly appreciated.

Thanks


Similar Threads:

• chatter
• Newbie- chatter only in x+ and y+
• Aluminum shaft chatter
• Need Help!- Chatter
• Problem- chatter

[dharmic]

For something like that I usually try and go full depth rather than in shallow passes and with a twin flute 6mm. Helix into the centre of each hole and the entry point to the outside perimeter and then profile the full depth in shallow sideways steps to get the chip load right. With a twin flute I'm running about 1200mm/min so your feed rate on a single is probably about right. Then I go in with a 4, 3 or 2mm to finish off. The 6mm seems to make a big difference in deflection.

That might be worth a try.

Using lube of any kind? I run a misted 20/80 mix of methylated spirits and water and it improves the finish and tool life enormously without gunking up my machine with coolant, just blow it off with the air duster at the end and let it evaporate in the tray.

This is all assuming it's the tooling that is deflecting and causing the chatter.

I also tweak the speed on the fly to make the machine as quiet as possible. You may be hitting some magic resonant frequency and pushing the feeds up or down by 10% may make all the difference in the world.

[darkclown]

For something like that I usually try and go full depth rather than in shallow passes and with a twin flute 6mm. Helix into the centre of each hole and the entry point to the outside perimeter and then profile the full depth in shallow sideways steps to get the chip load right. With a twin flute I'm running about 1200mm/min so your feed rate on a single is probably about right. Then I go in with a 4, 3 or 2mm to finish off. The 6mm seems to make a big difference in deflection.

That might be worth a try.

Using lube of any kind? I run a misted 20/80 mix of methylated spirits and water and it improves the finish and tool life enormously without gunking up my machine with coolant, just blow it off with the air duster at the end and let it evaporate in the tray.

This is all assuming it's the tooling that is deflecting and causing the chatter.

I also tweak the speed on the fly to make the machine as quiet as possible. You may be hitting some magic resonant frequency and pushing the feeds up or down by 10% may make all the difference in the world.

Ok I'm a little new at this so forgive if this sounds newbish. I'm cutting these spinners from 4" x 14" x 1/4" single piece of aluminum.
I use fusion 360 to design the spinners then I import it into aspire so I can set it up to cut out 5 of them at a time then export the g-code.

I guess what I'm trying to get at is I don't quite understand what you mean by helix down and then profile at full depth if I'm cutting them out on one piece of aluminum.
I don't even know if aspire has a helix option I'll have to check.
Thanks again for your help.

[dharmic]

At the moment you're taking baby steps down into the sheet and repeating the whole pattern. What I'm suggesting is you ramp in a helix or, if you can't do that, just plunge down slowly (100mm/min maybe) into the middle of each hole so the cutter's full depth, then spiral outwards taking a thin slice of the wall each pass until you reach the full diameter of the hole. Thinking about it you'll probably need to do your current approach for the external wall, especially if you're leaving tabs to keep the thing in place with clamping and whatnot.

Which means back to square one or looking at the other things. Sorry, red herring. Try lubrication if you aren't already, and try tweaking the feed rate multiplier to make the machine as quiet as possible through the cutting process.

[CNCMAN172]

Darkclown,
I have seen this on my setup as well. Several things can happen, one the rigidity of the machine is really critical when cutting aluminum. Second while most of us can not take deep cuts in aluminum with home built machines you can take other approaches. First I normally have to take .020 to .030 steps for DOC, driven by rigidity of my machine. Second you can get a much better finish if you do the first pass say .010 to .015 too small, so you have to do a finish pass. On the finish pass you will take the cutter to full depth and slow the feed down a little and most of the chatter type marks will disappear. This typically takes a little longer due to the finish pass but the result usually improve significantly. I have seen commercial machines use high quality tooling and cut .25" passes and two passes for 1/2" aluminum is amazing and their finish is amazing. Again, they are extremely rigid and have way more power than home machines and they use carbide cutters designed for aluminum and get amazing results.
Russ

[darkclown]

At the moment you're taking baby steps down into the sheet and repeating the whole pattern. What I'm suggesting is you ramp in a helix or, if you can't do that, just plunge down slowly (100mm/min maybe) into the middle of each hole so the cutter's full depth, then spiral outwards taking a thin slice of the wall each pass until you reach the full diameter of the hole. Thinking about it you'll probably need to do your current approach for the external wall, especially if you're leaving tabs to keep the thing in place with clamping and whatnot.

Which means back to square one or looking at the other things. Sorry, red herring. Try lubrication if you aren't already, and try tweaking the feed rate multiplier to make the machine as quiet as possible through the cutting process.

Yeah that was one of the things I was hoping somebody had a better way to do it on the profile cut out instead of just going down in tiny increments.
I appreciate your guy's help.

[sim2]

Machine insides.
Machine outside leaving material for cleanup pass....01-.02 or so all around.

Make a fixture using your layout from CAM program. Keep it simple, small piece of alum, hog out face leaving bosses that the I'd of your part fits snug on...drill n tap someplace inside to secure part to fixture.
Now put your part on fixture, secure and run your profile.
Parts secure, chips have someplace to go and a good finish should follow...also try 3 flute...single flute is great to pull chips out...not great for finish.