CNC machining soft aluminum

Hello,

I am trying to CNC route an aluminum panel. I can't find data on the alloy, it's a Hammond aluminum project box. It's pretty soft. I am currently using a 2 flute, low helix upcut solid carbide bit. It's 1/8" diameter. The aluminum is .0625 thick and I am cutting at .05/pass. I have tried feeds from 60ipm to 200ipm. RPMs from 7000 to 20,000. Pretty much the exact same result at all settings, it's tearing the aluminum pretty badly and leaving a huge ridge on the top. I am becoming convinced that I am using the wrong bit, but I am not sure what bit I should be using. I did try a downcut bit but that balled up and overheated quickly.
Hoping someone can help me get pointed in the right direction! Happy to fill in any missing data I haven't supplied.

Thank you.
James

Hi James - I'd try a bigger bit with 1F. But FS Wizard picks these settings for soft aluminium & 3mm tool. Its metric values so I understand them. 0.05" is 1.27mm so back it down to 0.5mm (0.025" say) to start. You don't want to clog up the tool gullet. Spiral cut down vs plunge. The plunge can immediately clog and your history if the settings are wrong. Ramp down at 2 or 3degs more will clog.

The feed is 1371mm/min or 54in/min and the spindle is at 15500rpm (metric or imperial) This is a mm/tooth of 0.044mm. I'd start at 0.05mm as a guess so I think this is close. Use some metho or kero or WD40 as a lub and make sure your tools sharp. If it has aluminium stuck to it eat it off with caustic soda. If the tool has metal on it it will attract more metal. The cut also relates to how stiff your machine is and how low the tool runout is. If you have high runout one of your teeth is cutting the other is rubbing. Same if the machine has a wobble... That's one reason a 1F tool is good. The other is that it can run faster yet cut slower. Look up tooth load (Fz) to get a feel for this. If you have a small spindle axle you may never cut aluminium they are too wobbly. Peter

also drill out the centre of the hole then plunge down in the hole and spiral out in one cut if your cam has a cycle like that. Use same settings as above. Often its the plunging thats the issue not side cutting.

I think you will find the box is LM24 a diecasting alloy. High in zinc and silicon can be a bit gummy....
https://www.mrt-castings.co.uk/press...nium-lm24.html

Hi James!

The best solution would be to go with a 1 Flute Router Bit as suggested, a Single O Flute will give you the best finishes.

Also, a Downcut will give you a better part finish at the top of your part and would also help if the top finish matters most. Here is a quick breakdown of the cut options out there:
-An Upcut Bit will pull the chips up to help with chip evacuation and it will leave a nice finish at the bottom of the slot but it will not leave a nice finish at the top of the slot as you are experiencing.
-A DownCut Bit will provide downward pressure, which is nice for a Vaccum Table and will leave a better finish at the top of the part (but not as good of a finish at the bottom of the part).
-The other option is a Compression Bit that Combines an Upcut at the End of the Tool that is .205" Length of Cut at 1/8" Diameter with a DownCut Spiral after that. This will give great finishes at the top and bottom of the part and provide great chip evacuation along with downward pressure that is ideal for vacuum tables.

I like the Osborn Routers, but any O Flute Router with a DownCut should help in the application. Here is the DownCut Spiral O Flute Cutter designed for Machining Aluminum Sheets in Routers we would recommend:
https://www.toolhit.com/products/62-...6636eba7&_ss=r

Or if you prefer an Upcut to keep Chip Evacuation good then they do offer a Series for Soft Aluminum
https://www.toolhit.com/products/63-...c45735b1&_ss=r

Here is what the compression looks like (it is 1/8" Diameter x 3/8" LOC x .205" Upcut LOC x 1/4" Shank x 1 Flute):
https://www.toolhit.com/products/60-...e48ab5d3&_ss=r

Run at:
16,000 RPM
.002"-.004" CLPT

Any O Flute will help you. Hopefully this Helps!

Mike

Wow, thank you both! I had suspected that my bit was likely the problem. I pulled my bit out and found that both sides of the chip evacuation channels are full to the top with aluminum that is basically welded in there. I can't get it out!!

I guess I could use a larger bit for the main hole, but the small holes around are only 1/8". My current bit is actually drilling those out really cleanly, only the larger hole is a problem. I tried a ramp and spiral both, but again, the welded aluminum in the bit instantly created a mess.

Mike, your toolhit site is awesome! I've been using CNCCookbook's G-Wizard F&S calculator pretty successfully, but the website is very helpful. I will be ordering some bits from you!

I'll try a single O flute bit next and see how it goes.

Thanks again.
James

Hi James- soak the bit in caustic and it will dissolve the Al off the tool. Good Luck Peter

Hi,
I use flood cooling and it helps with ALL materials, including aluminum.

It's less about cooling but getting the chips out of the cutting zone. If you re-cut chips you will end up with BUE (Built Up Edge), where
the chips weld themselves back into a lump. You might try air-blast, it too could blow the chips out of the way, but flood coolant is still probably the best
overall strategy despite the inconvenience and sometimes mess.

You might also try diboride coated tools, it has especially good lubricity in aluminum. I got some when I was doing some sticky 5000 series marine aluminum, helped
no end.

Craig

Hi,

Quote:

---

Hi James- soak the bit in caustic and it will dissolve the Al off the tool. Good Luck Peter

---

You can always light a match to see if its working. If the hydrogen that is generated by the reaction between aluminum and hydroxide explodes in your face....then you know its working.:nono:


Do this outside with tons of ventilation, a hydrogen fire/explosion is NOT to to be trifled with.

Craig

I don't think the problem is in the cutter, but in the lack of lubricant on the cutter.

I use an air blast to clear the chips and a pulsed misting of 3:1 kero/olive oil. If I see any scruff on the top surface, as shown in the pic, I immediately add some of the mist to the job (an over-ride button). This almost always improves the cut.

Yes, soft aluminium is quite bad for this (eg 1000 series), but a 6000-series metal will go much better, if you can move to it.
Hum - a Hammond Al box - I wonder what alloy that is! I know less about casting alloys, but misting has always worked for me.

Cheers
Roger

Hi Roger- Look at #2 I spec the alloy there. Craig would only be a little POP. If you add detergent to the water it makes nice hydrogen bubbles that pop quite nicely... Peter

Hi,
my brother and I made enough hydrogen with aluminum and hydroxide to fill balloons 1m in diameter. On one occasion we detonated a balloon that had deflated to the extent
that we thought it safe....we were badly shocked and thrown many feet to the walls of the room we were in. NEVER, EVER fool with hydrogen, when it explodes its violent.

Craig

Hi Pete

Ah so - LM24.

Machining practice [for LM24] is similar to that for other Aluminium castings alloys containing Silicon. Whilst there is not the tendency to drag associated with high silicon alloys such as LM6, tool wear is more rapid than in the case of alloys containing relatively small amounts of Silicon. The use of carbide-tipped tools is recommended but a good finish can be obtained with high speed tools. Lower alloy steel tools may be used, provided they are frequently reground to maintain a sharp cutting edge. A cutting lubricant and coolant should be employed.
https://www.mrt-castings.co.uk/press...nium-lm24.html

This suggests some lubricant is needed. Likely.

Cheers
Roger