Looking for some help with speeds and feeds and end mill selection for milling 1/4ā soft aluminium- guessing it is 3003.
Thx.
The only thing I can find at sienci is the good old fns datasheet for the longmill.
Donāt know if using a router table or a drill press works with this data sheet, but it at least is something to work with. I would advice against using a milling bit in a band saw though. It will probably fly off or jam your machine.
Hope you have some use for this datasheet in combination with your mystery machine.
Please be careful!
Usual preface, Iām with PreciseBits. So while I try to only post general information take everything I say with the understanding that I have a bias.
Without knowing the grade I would try no less than a 0.0015" chipload. Without knowing the grade AND tool Iād stick to around 600 SFM. What that means in actual cutting is ~9,000 RPM (RPM = (3.82 * SFM) / Diameter) and a MINIMUM of 27 IPM for a 2 flute cutter (Feed = RPM * Chipload * Flutes). Cut your pass depth down to something ridiculous to start out at (<1/4 tool diameter). You can increase this as you go but it buys you a lot of forgiveness.
The reason for this is that you are probably more likely to have issues with melting and choking the tool than anything else. In fact if you have the machine and tool rigidity itās actually much easier to cut harder grades of aluminum.
Some other general things.
Make sure that the tool you are using has as short a cutting length as possible as you need the tool rigidity.
Do NOT use something like double sided tape to hold down the material. You need something rigid so the material canāt float back and forth while cutting.
Any runout thatās a significant portion of that chipload with probably screw you. It will make some of the cuts actually take a smaller chipload that will again melt the material. You can bias that by increasing the chipload (feed) to cover for it as long as the tool and machine can resist the larger cutting forces.
Not knowing the grade makes the whole thing a āat your own riskā scenario. You could have something with lead or bismuth in it (free machining). Those want even more chipload or they will melt.
I hope that marginally useful. Let me know if thereās something I can help with.
3 Likes
I have an altmill 4x4 with 1.5kw spindle, and i will be attempting to cut soft aluminum also. 3003 with an h14 hardness. I am going to be cutting through .080 sheet with o-flute bits, 1/4 and 1/8. From what i can tell, an rpm around 12000, a feed of 50 ipm, and depth per pass of .030 may not ruin my bits lol. I purchased an amana "soft aluminum " o flute but info is limited.
I actually checked on the amana bit, and their chart mentioned 80ipm with .008 chipload.
Do you think i could do this in one pass?
Thatās about half as hard and twice as āstickyā as 6061-T6 (I use that as a base as thereās the most info about it).
A lot of the rest of what Iām going to say depends on the tool. One of the big things here is what your flute length and stickout is on these. Ideally for metal cutting they would be stub length (1.5x diameter). However, Iām going to assume for standard length (4x diameter). If they are longer than that youāre going to need to reduce pass or feed to account for the cutting forces. Iām also assuming slotting. If thatās not the case than you have a lot more forgiveness. In all cases choke the tool up as far as you can into the spindle without bottoming out the tool or inserting a ground portion into the collet.
That RPM will probably be okay on the 1/4". On the 1/8" I would up it to at least 18,334 RPM to hit 600 SFM. This will help with shear on the softer aluminums. You should be safe up to at least 800 SFM. They say on their sheet up to 1000. 800 would be 12,223 RPM and 1000 would be 15,278 RPM on the 1/4". 1/8" would be double the 1/4"
Feed wiseā¦ Forget about feed and think only in chipload. If I was going to start with this Iād probably shoot at 0.003" chipload. So that would be 36 IPM for the 1/4 at 12KRPM" and 55 IPM for the 1/8" at ~18KRPM. That should be enough to keep most issues with a soft metal at a minimum. At the same time you have to account for cutting forces and their effects on deflection (see below). Otherwise you could use a higher chipload.
To be clear Iām biasing all of this to a high chipload lower pass depth as thatās typically safer with soft metal and unknown (to me) tool geometry.
Could you? Maybe, if itās a real short tool on the 1/4". The real issue here is this is the best place to reduce cutting forces on the tool. Ideally I like to limit the deflection to under 0.0003" for these as that will modify you chipload in the next flute pass. So if these are standard length or more, I would split the pass in half for the 1/4" tool (0.040"). For the 1/8" tool thereās much less mass in it so I would go with 0.020". Both of those should limit the tool deflection to under 0.0003".
Regardless, if you are splitting the passes up try to keep them even. With the example that you gave of 0.030" that would mean that you have 2 passes at you 0.030" and then a pass at 0.020" to finish cutting through your material. That will cause the last pass to deflect less and as a result it will take a very light cut on the climb side of your first 2 passes. In a worse case that will melt that material and cause issues.
You can go a lot more aggressive than this depending on the tool, hold down, etc. Iām just giving some base data to work with that should be okay in most application with at least ādecentā everything and assuming no major issues.
One thing to watch for though is that Iām guessing you donāt know what your runout is. That is partially mitigated by using single flute tools. However, itās still potentially an issue with plunging. So if possible Iād ramp into the cut to further mitigate it.
It would also help a lot if you could use a oil based cutting fluid with this grade of aluminum. Thereās a real risk of building up an edge on this depending on the artwork (direction changes, small segments). Oil based cutting fluids buy a lot of forgiveness here even if itās just brushed or sprayed on by hand.
No matter what CLEAR THE CHIPS as you are cutting. Even more of an issue if you are not able to use a cutting fluid. This will straight up break tooling in general with metal working. But especially with soft metal. If those chips are in the slot as the tool is trying to cut it will recut them too. Those recut chips will not be at your chipload and can cause major issues.
Hope that helps. Let me know if you want more on something.
1 Like
I ran a program yesterday on .062 aluminum with .250 o flute. CL was .62, rpm 14000 and ipm 60, pass depth of .035. Chip load was around .0045 and it seemed to do fine. There was one point chatter was horrible and pulled material instead of cutting cleanly. I sprayed some lubricant on it and it cleared and finished the project without issue. I am guessing a chip stuck on bit, but must have came loose. Iām sure it can be improved but it was successful, so i will take it.