Aluminum sheet edge burr

[ChrisSledziona]

I recently tried cutting profiles in aluminum sheet on our PRS standard w/ HSD spindle. I'm getting a burr along both sides of the cut. I played with my feeds and speeds until I broke a bit. Here are my settings:

material: .050 3003-H14 aluminum [spray glued to spoil board for hold-down]
Bit: 3/16" single flue

24355

10,000 rpm
30 IPM
.032 pass depth [2 passes]

calculated chip load: .003

climb-cut
ramped into material

Here's the result:
24356

Any thoughts on how to eliminate the burr?

[Brady Watson]

My plan of attack would be to use a spiral-O made for routing aluminum. I am not familiar with the tool you show. The rake is different for metals compared to aluminum etc.

However...Cold worked (H14) 3003 resides in the 'poor' column when it comes to machinability - so there isn't much you are going to be able to do about those burrs on 3003. Better hold down always helps and, reverse the cut direction from Climb to Conventional. You can see the scrap looks better in the pic...

My numbers for most AL alloys are 1.2,0.7 inches per second @ 13,000-15,000 RPM with a single flue spiral-O (with short CEL) from Onsrud. Don't know the exact number off the top, but I think it is a 63-series. Look online or contact Gary Beckwith (http://www.beckwithdecor.com/index_files/ONS4.htm) (a member here & good guy) - he is an Onsrud dealer.

-B

[Simops]

I find that the grade of aluminium makes a big difference. I'll get burning like yours then change aluminium with same settings and get none.....damn frustrating at times.
Good luck....

[donek]

I find that the grade of aluminium makes a big difference. I'll get burning like yours then change aluminium with same settings and get none.....damn frustrating at times.
Good luck....

Material being cut is just as important as the cutter, feeds, and speeds. I tried cutting a 5000 grade aluminum once and the result was horrible and it broke the cutter. I only cut 6061 and 7075 on my machine. I know nothing about this series aluminum, but would suggest trying 6061.

The only other comment I have is your feed speed seems way too low. I rough 6061 at 2ips (120ipm) and finish cut at 1.2ips (72ipm) with a 1/4in cutter and 0.05in depth of cut. The best way to get gummy cut results in aluminum is to let the bit sit in one spot and generate heat (ie travel too slow).

[ChrisSledziona]

Thanks for your help guys! The goal here is to cut out a shape in AL, then do some simple bending. I choose 3003 AL based on it being suitable for cold-forming. I didn't realize it would be impossible to machine.

I tried some different feeds and speeds but the cut quality was worse with each experiment.

The bit I show in the first post is supposedly designed for cutting soft aluminum. I changed to the more standard Spiral 'O' Flute bit with no better results.

I'm going to try 6061-t6 and see how that goes.

[knight_toolworks]

I found the soft stuff you need to keep the depth of cut at around .01 per pass then it seems to cut ok of course it takes forever but it does work.

[ChrisSledziona]

I found the soft stuff you need to keep the depth of cut at around .01 per pass then it seems to cut ok of course it takes forever but it does work.

Good Point. I did notice that there was no burr when ramping down into the cut. Maybe I'll try that.

Also. Is there a spoil board material that the aluminum cutters prefer? I feel like MDF is not ideal.

[MogulTx]

Definitely need to ramp into ALL Aluminum cuts. On soft stuff, I usually ramp, use conventional cut, and a very shallow pass. Ramping and shallow passes add time to your cut, but you won't get the burrs that you are getting. And if it is heating up, it is going to defeat your spray glue. I try to have screw holes outside my cut area to hold the material. If you go slowly and use a couple screws plus your spray glue, the piece you are cutting out of the middle may not heat and warp and pull away from your glue. Otherwise you will need some other form of holding scheme. Maybe make yourself a mini vacuum platen or something...

For reference: Brady's speeds are a great place to begin. He is also correct about 63-series cutters from Onsrud (being for aluminum), and Gary Beckwith sent me a few in 1/8 and 1/4 recently... Work really well in aluminum... RAMPING is important!

[shoeshine]

this stuff is magic http://www.findtape.com/product190/Permacel-P-02-Double-Coated-Kraft-Paper-Tape.aspx?idx=10&tid=25&info=permacel

I use a piece of aluminum toolplate screwed to the spoilboard then tape between the metals. after it grabs, smack it with a rubber mallet to ensure adhesion (its pressure activated)

[garyb]

Just seen this post
The tool looks like a copy of the Onsrud 63-400 series which is designed to cut soft Aluminum of 3003 grade.
your problem is your feed rate is too low for that soft of AL 80IPM and 10,000rpm is the recommended for the 63-420 3/16" tool.
you will find the 63-400 series listed on the bottom of this page with feeds and speed http://beckwithdecor.com/index_files/ONS27.htm
When cutting small parts like you have we use 3m hi tac and glue the alum sheet to 3/16 tempered Masonite.
Gary

[garyb]

sorry poor choice of words, should have said looks similar to 63-400 series (edit time was up)
Gary

[sean_adams]

Gary
How do find separating the Masonite and aluminum afterwards, is there any residue left on the aluminum? If so how hard is it to clean up? Also are you using a mister or cutting dry?
Sean