What should I change to get a better surface finish on Aluminum

[TTalma]

I have a AXYZ CNC router, It is designed for cutting wood and Aluminum. I am cutting aluminum for the first time with it. The person I bought the machine from demoed it cutting aluminum and his cut edges were beautiful! This was a few years ago and I have no idea what settings or bit he used. My cuts don't look great (See pic).

My biggest issue is probably that I need to cut dry. I spray the bit with rubbing alcohol while its cutting from a spray bottle, and use air to get the chips out of the channel, but that doesn't get them all (about 75 to 80%).

I didn't take a picture, but I am making chips They are little squares, No sign of melting, and after cutting I can touch the bit without burning myself so it doesn't appear to be getting to hot. Cut time is about 7 min for this part.

I am cutting the parts out of a larger piece of stock, so the cuts are a full .25" wide. I am not taking a finishing pass. I used an online feed/speed calculator and believe I have the setting correct.



my machine, and settings details:

Onsrud 65-025 bit (.25" single flute upcut bit, 65-025)
.5" thick 8081 aluminum
6.6 hp spindle
12,000 rpm (This is the Min spindle speed)
40 in/min feedrate
.15" depth of cut
ramp in to cut at 5 degrees

Any suggestions on what to change?

 

[michiganbuck]

A single flute will not run as true because of balance and a longer distance between wacks. .15 is a very heavy cut for such a machine and cutter. You might try a multi-flute spiral flute end mill..A left-hand spiral / right hand cut would help push down the part

 

[IninefingersI]

If you are full slotting with a single flute end mill, I'm surprised your finish is as good as it is.

 

[TTalma]

Would this load the path with chips? causing heat issues?

 

[TTalma]

If you are full slotting with a single flute end mill, I'm surprised your finish is as good as it is.

Should I do a finishing cut with a 4 flute cutter? would .002" be enough?

 

[IninefingersI]

Should I do a finishing cut with a 4 flute cutter? would .002" be enough?

That isn't enough. Your chatter is deeper than that. I'd leave myself .020 - .030 to clean up. I usually use 3-flutes.

 

[mhajicek]

A 3 flute cutter designed for aluminum will leave the best finish. As said above, probably about a .020" to .030" finish cut, but also a skim pass (0.000" stepover) or three to remove deflection. Your finish shows evidence of a very non-rigid machine / setup.

 

[michiganbuck]

Using a down cut multi-flute, having the part raised off the table for space where chips might go, having a raised rail near the machining edge to reduce chatter, perhaps a weight-loaded wheel to ride the part top side.

*A raised part might be set on three points like setting a surface plate, for less chance of the part chattering, perhaps with a weight on top of it.

 

[anthony_industry]

it's dependent on how rigid of your machine, RPM of spindle, Feedrate, and tools. I guess you are using hobbies CNC machine? if that, please increase your spindle up to 24KRPM or maybe higher. and reduce feedrate as well.

 

[TTalma]

That isn't enough. Your chatter is deeper than that. I'd leave myself .020 - .030 to clean up. I usually use 3-flutes.

Thanks I will try that. Any recommendations on cutter? I'm used to suppliers for cnc wood routers. It seems a majority of these only make a single flute bit.

 

[TTalma]

A 3 flute cutter designed for aluminum will leave the best finish. As said above, probably about a .020" to .030" finish cut, but also a skim pass (0.000" stepover) or three to remove deflection. Your finish shows evidence of a very non-rigid machine / setup.

My machine defiantly isn't as ridged as a machine designed for milling steel. But it has very little vibration when performing these cuts. based on the quality the original owner got, it's not the machine it's the person using it!

 

[TTalma]

Using a down cut multi-flute, having the part raised off the table for space where chips might go, having a raised rail near the machining edge to reduce chatter, perhaps a weight-loaded wheel to ride the part top side.

*A raised part might be set on three points like setting a surface plate, for less chance of the part chattering, perhaps with a weight on top of it.

With this part, I can clamp it in place on a support, drill the holes, and mount it to the support then cut the profile out. I am not sure what you mean by weighted wheel. I Think the chatter is because the bit is sticking out about 1.5" if I move it down so only the cutting edge is out of the holder that should help reduce the chatter.

 

[TTalma]

it's dependent on how rigid of your machine, RPM of spindle, Feedrate, and tools. I guess you are using hobbies CNC machine? if that, please increase your spindle up to 24KRPM or maybe higher. and reduce feedrate as well.

This is a commercial machine, although I am just a hobbiest. If I increase the speed and slow the feedrate I am worried heat will become an issue.

 

[CarbideBob]

Climb or conventional cut?
Good pictures of the chips?
Part is fine but what I always want to see is the chips under high magnification as they tell the real story of how they got made.
Unlike the fans of a down cut I be more into two-three flute and high helix the other way if able to hold onto the part.
There is no heat problem here. There is chip weld and then oh-my lots of heat.

You are slotting out of a bigger plate need to cut dry and have 6HP to use?
Bob

 

[IninefingersI]

Thanks I will try that. Any recommendations on cutter? I'm used to suppliers for cnc wood routers. It seems a majority of these only make a single flute bit.

This is my go-to 1/4" for aluminum.
https://www.mscdirect.com/product/details/82976580

If you are just profiling and ramping your entry, you might consider something with a small corner radius. More expensive, but they can keep you from blowing the tips off your flutes. Your break through just needs to be a little deeper. Personal preference.
https://www.mscdirect.com/product/details/70217195

 

[TTalma]

Climb or conventional cut?
Good pictures of the chips?
Part is fine but what I always want to see is the chips under high magnification as they tell the real story of how they got made.
Unlike the fans of a down cut I be more into two-three flute and high helix the other way if able to hold onto the part.
There is no heat problem here. There is chip weld and then oh-my lots of heat.

You are slotting out of a bigger plate need to cut dry and have 6HP to use?
Bob

This is climb cutting, I've tried conventional as well. Surface looks the same but chip clearing is worse. I will take a picture of the chips, But I don't have magnification.

I am slotting out of a larger plate, I am dry cutting (hand misting with rubbing alcohol), blasting with air to clear chips from slot. Running the spindle at 12,000 rpm as according to manufacture (Columbo) this is peak power.

 

[TTalma]

This is my go-to 1/4" for aluminum.
https://www.mscdirect.com/product/details/82976580

If you are just profiling and ramping your entry, you might consider something with a small corner radius. More expensive, but they can keep you from blowing the tips off your flutes. Your break through just needs to be a little deeper. Personal preference.
https://www.mscdirect.com/product/details/70217195

Thanks for the links. I ordered both. Cost is never ignored, but I've found cheap tools end up costing more in the long run.

 

[Mtndew]

I am dry cutting

6061 aluminum or 7075?
7075 you can get away with dry cutting easily.
6061 will gall up on you eventually and destroys the cutter and possible the work piece.
Stub up your cutter as much as you can into the holder, this will help with rigidity and chatter.

 

[michiganbuck]

If you tap the part with a small hammer and find vibration likely that will deter getting a good finish. Some type of hold-down or weight may reduce vibration. A larger diameter and shorter length cutter may help. A pull spring or weight arm to your spindle may help to reduce vibration. If you take handhold to your spindle and find that it wiggles easily..taking up some of that wiggle can help.

Aluminum is about the limit of your machine, way tougher to machine than wood. You may find that a very small stock removal is needed for the best finish. If having a quick set-up you may run finish production/the light cut with using a second operation with a fresh sharp cutter.

You may find that 1/2" (Thickness) is too much for the machine and so run two passes of a 1/4" at +.005 or + .010 and then a light stock removal for the 1/2" finish pass.