Cutting oil use when machining aluminum plate?

[windcrest77]

I'm going to be machining hole patterns to make electronic control panels out of 1/8 in thick (11 gauge aluminum) with a final profile cut...

Should I be squirting cutting oil on the bit occasionally throughout the job when cutting an aluminum panel like this? I figure I'll tell the software to do it in two passes for all holes and the profile (1/16 inch per pass). The size of the finished profile is typically 11 x 11 inches and the number of holes on average is 8 to 12 3/4 inch holes and a few rectangular holes.

I'd like to extend my bit life by a few percent if that means the minor hassle of squirting come cutting oil now and then on the work.

[johnb]

If this is going to be a regular thing (production), you'll likely need to either replace your spoilboards with phenolic or anchor a sheet down on top of them in order to use any water or oil. If you don't, then as the Brits say "You'll end up with a right mess".

[windcrest77]

Jul 5, 2020 7:31:42 GMT -5 johnb said:

If this is going to be a regular thing (production), you'll likely need to either replace your spoilboards with phenolic or anchor a sheet down on top of them in order to use any water or oil. If you don't, then as the Brits say "You'll end up with a right mess".

I have an enormous amount of laminated particle board shelving and old flat pack cabinet sides that I use for spoil boards, left over from when I used to install flat pack cabinets. That stuff is totally flat and waterproof because its laminated. I dont expect oil to ever get to my original Iconic4 machine board, going forward I dont ever expect to ever need to "spoil" the bed of the Iconic ever, even for wood, I've been using up all this laminated board I have. I can set my cut depth to just cut into the laminate a little so my parts are through cut thoroughly, not worrying about cutting up my original board. I've been using the blue masking tape with crazy glue method to cut these aluminum plates, so that I dont need any tabs that I have to saw out manually later. I dont see much chance of oil getting to the original MDF slats.

Since nobody answered here yet with a definite "no dont use oil", I'll assume it cant hurt to go ahead and use cutting oil when working aluminum plate.

[mnwoodbee]

The biggest thing with aluminum is the right type of bit and the yes coolant mister or cutting oil. The oil with help prevent the “gumming up” either in the tool flutes or sticking to the profile of your part. The lubricant helps with the heat build up and chips welding together
You could use a cheap brush and paint oil on in the path of the tool then on the tool bit itself.

[windcrest77]

Jul 5, 2020 20:40:15 GMT -5 mnwoodbee said:

The biggest thing with aluminum is the right type of bit and the yes coolant mister or cutting oil. The oil with help prevent the “gumming up” either in the tool flutes or sticking to the profile of your part. The lubricant helps with the heat build up and chips welding together
You could use a cheap brush and paint oil on in the path of the tool then on the tool bit itself.

Thanks,

I've been doing a lot of youtube research. It seems many are using WD40 in a spray pump bottle (like a window cleaner spray bottle). On my drill press I use regular cutting oil. But knowing first hand how cutting oil behaves with aluminum and regular jobber drill bits on the press. I'm thinking a light spray of WD40 will do better. On the drill press cutting oil gets thick and sticky and the chips can clump. WD40 smells bad but it should work better.

I'm using 3 flute 45 degree helix angle center-cutting end mills for both the milling and the drilling. According to the charts I need to shoot for a chip rate between .05 and .1 (using mm). If I select a bit speed of 3000 RPM Vectric is computing a chip rate of .0988 and a feed rate of 889 mm/min and a plunge rate of 254 mm/min. I'm doing two passes through .125 material, no ramps, all plunged for the profile and pockets. And I'm going to try it with no peck drilling for the drill paths. I would think 1/8 inch aluminum I can do a drill through with no pecks? I'll find out. I decided against twist drills, I think the center-cut end mills may do better.

I'll post back here on if these feeds and speeds worked ok for me, and how the WD40 worked out. After I get my new end mills delivered.

[johnb]

If you detest the smell of WD-40 you might try Marvel Mystery Oil instead. It's about SAE 3 and composed of mineral oil & something akin to Varsol. You might, however also consider that WD-40 has a flash point of 122 degrees (F) whereas MMO has a flash point of about 160 degees (F).

[Axiom Tool Group]

We have machines a large amount of non-ferrous metal...and unless you are pushing the limits for small business production requirements, then lubrication may not be needed at all provided that the correct bit is being used.

O-Flute bits such as those found in the Axiom Aluminum bit set are designed for non-ferrous metal specifically and would not need lubrication if setup correctly.


I've cut a number of parts...namely aftermarket jeep parts including pocketing and drill hole locations.

Regarding pocketing, I generally use the 1/4" O-Flute bit with a DOC of 0.010-0.020", 16k RPM and a feed-rate of 30-70IPM depending on the grade of aluminum.


For thru holes, or drill hole locations...rather than use a split point bit, I prefer to use an O-Flute bit that is smaller than the desired hole. For instance a 0.25" hole scan easily be cut using the 0.125" O-Flute bit with the same DOC of 0.010" using a spiral ramp which allows the machine to gently lower directly through the plate without peck drilling. *Generally would advise keeping the plunge rate lower for this operation (15-30ipm)


*Both scenarios do not require lubricaiton when cutting but it certainly does not hurt. It may actually keep many of the chips from flying as far....but as mentioned, the oil may soak in the spoil boards.


WRT the use of WD-40....Many people ask about using WD-40 on the guides and ball screws, it should be noted that WD-40 isn't actually a true lubricant. WD stands for "water displacing" and its main use is as a solvent or rust dissolver. The lubricant-like properties of WD-40 come not from the substance itself, but from dissolving components.

This can actually damage the grease that is used within the bearings themselves.

[windcrest77]

Jul 13, 2020 7:58:44 GMT -5 Axiom Tool Group said:

For thru holes, or drill hole locations...rather than use a split point bit, I prefer to use an O-Flute bit that is smaller than the desired hole. For instance a 0.25" hole scan easily be cut using the 0.125" O-Flute bit with the same DOC of 0.010" using a spiral ramp which allows the machine to gently lower directly through the plate without peck drilling. *Generally would advise keeping the plunge rate lower for this operation (15-30ipm)

Thanks!

That's an idea, just do all the round holes as a pocket instead of plunge drill.

For 99% of my projects the smallest hole is .125 inch so a 1/16 single or double flute with an Aluminum steep helix should be good too? Also for 99% of my projects I'm machining 6061 aluminum plate that is .125 inch thick.

I'd like to find the sweet spots for a limited set of tools in 6061 aluminum to be more productive. I may have to accept a lot of mistakes to find those sweet spots.

For 1/8 inch material would 3 passes be enough or should I do more? You mentioned a DOC of .02 so that would be about 6 passes.

[windcrest77]

Jul 13, 2020 7:58:44 GMT -5 Axiom Tool Group said:

I've cut a number of parts...namely aftermarket jeep parts including pocketing and drill hole locations.

Regarding pocketing, I generally use the 1/4" O-Flute bit with a DOC of 0.010-0.020", 16k RPM and a feed-rate of 30-70IPM depending on the grade of aluminum.

I'm learning. I downloaded a feeds and speeds program called GWizard which has a profile set up for the Iconic 4. Attached is the recommended feed/speed it gave me for 6061 aluminum, with a 3 flute 45 degree helix end mill (regular HSS) with .5 inch stick out, doing .125 inch material in two passes .0625 each. Of interest is that it recommends NOT using climb milling, but instead "conventional" milling, Vetric likes to default me to climb milling. But of mention is that when I got to 1/4 inch bits GWizard recommended climb milling. I kept all the red lights off as I had to back off the feed rate to not exceed max deflection with .5 inch stick out. GWizard calculated 13796 RPM at 45.36 IPM. This is falling within your recommendation of 16k at 30 to 70 IPM. 6061 is a much stronger aluminum than your typical hardware store angle and flat stock.

Thanks so much. The combination of your numbers and GWizard here and how they jive really raised my confidence level. I just now have to decide which bits to use, I feel I have to get some more bits with less stick out, and run numbers for all those bits in 6061 aluminum. This is starting to move out of being a headache and into enjoyment!

The screen shot of the above described bit in Gwizard with the Iconic 4 and 6061 aluminum is attached if anyone is interested.

[colofan]

I use an o-flute bit but instead of oil I use compressed air that blows off the chips and keeps everything cool.

The picture showing me using the laser with the cooling as well.

[johnb]

Feb 25, 2021 10:29:27 GMT -5 colofan said:

View AttachmentI use an o-flute bit but instead of oil I use compressed air that blows off the chips and keeps everything cool.

The picture showing me using the laser with the cooling as well.

Do you find that the compressed air cooling on the laser burns creates a more consistent line quality and fewer "flares"?

[colofan]

Yes I use a fairly low flow rate and the line retention is very nice.