I'm struggling with aluminum sticking to my 2-flute carbide bit on my Partner MB16

I've been learning how to use the machine, making sure everything is working.
For my first piece, I designed a part that I want to make in aluminum but I'm running into some configuration issues.

I used Fusion 360 to develop 2d adaptive optimum path, but it was way, way too aggressive.
The screenshot is with already adjusted plunge feed rate from 44in/min to 4 (yes 90% reduction).
https://www.cnczone.com/forums/attac...d=451894&stc=1

I slowed down my feeds to 60, then 40, and even 10%, and the bit still gums up.

I've doubled and tripped my programmed RPMs (manual RPM crank handle), and still no luck.
I don't have flood coolant. For now am just using air nozzle that I hold close to cutting edge.
What are you running in terms of SFM, RPMs and cutting bit engagement?

I do not have any cooling, but have been using air to blow ships out.
Some on hobby forums have recommended using Yonico or Amana O-Flute Upcut Spiral End Mill CNC Router Bit, but I'm not sure if that's because most use benchtop style, small machines or not.

I'm never going to be a production shop, so time is NOT money in my case.
I'm not opposed to spending $50-$80 if I have to, but I want to be careful with wasteful spending. For my first set, I'm using HF bit set. My brand new (cheap) 2 flute 1/2" bit. Could that be it? Should I step down in size or go up? I have 10 bits from 3/16" to 3/4. Set came in both 2-flute and 4-flute. I've been reading and most claim that aluminum is better off with 2 vs. 4 flutes.

I went super conservative and got a bit better results, but still issues.
https://www.cnczone.com/forums/attac...d=451898&stc=1https://www.cnczone.com/forums/attac...d=451896&stc=1

I'm running calculators on different websites and mobile apps, but I'm still coming up empty.

What is my problem or problems?
I really want to learn and am open to any and all criticism.
If it's constructive and informative, I'll take it and implement whatever wisdom you're willing to impart.

Thank you.


https://www.cnczone.com/forums/attac...d=451900&stc=1https://www.cnczone.com/forums/attac...d=451902&stc=1

Also, I have been watching a bunch of tutorials and reading a articles/reviews, but it seems that the HASS and Tormacs zip at 10,000, 18,000 or even 24,000 RPMs, so I'm not sure if it's a linear correlation with my old and slow 3,300-4,200 max RPM dog.

What type of aluminum are you machining?

With aluminum you need some type of lubrication to prevent welding. WD-40 or kerosene works very well hand applied with a spray bottle. I would recommend a spray mist system and a good water soluble coolant.

On a few occasions I have milled some really cheap aluminum that was extremely gummy. Even with coolant there was no winning.

That .02 ipt is a good bit high. It should be like .005".

The .0018" though is low.

Build one of these. Its my dad's build that he uses on his Partner 4. You really need some lubrication on there and this has worked well for him. Attachment 451906

Sent from my SM-N960U using Tapatalk

...#1 get a good quality 2 Flute HSS (High Speed Steel) or Carbide endmill. those Harbor Freight endmills have poorly ground flutes causing excess heat. Jim and cbChris Spray Mist suggestion is the way to go if, you dont have flood coolant. 1/2' EM 2000-3000RPM at about 20-30 IPM is in the ball park. 5-10 in Z
https://www.mcmaster.com/spray-miste...-dispensers-7/

And get some Chip Screens ..your going to need them.
Good luck
DJ

Agreed, lubricant and .02 is too much.
Also, have you been chipping the aluminum off the tool after it starts to stick? After it has gummed up once, it will do it more readily the next time around, in my experience.

Those cheap chineseium cutters are worthless. A few good carbide cutters are worth a drawer full of those. I like YG-1 Alu-Power 3 flute 45deg. Practice with 1/4" cutters, they are cheaper when you break them.

Lastly, try a roughing bit.

Just some rules of thumb, run about all the rpm your machine has, mine has 5000, but it's old and tired, so I tend to run 3000 on everything, don't want to overheat my spindle bearings. For feed, you want to run 1% of the cutter diameter per tooth, so a .500 end mill you want .005" per tooth, and use a 2 or 3 flute only on aluminum, no 4 or more unless it's a super light finishing pass. Depth of cut can be deep if you are not slotting and just profiling, but keep your step over at 15% to 25% of the cutter diameter. Use good carbide end mill, I like either the YG-1 or these guys, https://www.carbidetoolsource.com made in the USA and great prices.

You will have to have coolant of some sort, WD40 will work, but it's hard to be consistent with a squirt bottle. I built the MQL system years ago, it's well worth the effort, skip Sparber's version and go direct to my dropbox link: https://www.dropbox.com/s/wsggc0nmez...rayer.pdf?dl=0 I have been using this for years now and for an open machine, it's the only way to go. You will have to buy new mixing valves every year or two, and the clear containers for the coolant housing tend to get opaque from the oil/water mixture (I use Master Chemical Trim Sol) so you'll need one of those on occasion too.

Last but not least, what type of aluminum are you cutting, 6061-T6, 2024-T4, or 7075-T7 will cut great, what you have in your picture there looks like some gummy stuff, stay away from any cast aluminum or "O" condition aluminum, that means it's dead soft and is almost impossible to machine.

Good luck, you will soon get a feel for what speeds and feeds work with your machine.

As others have said once the aluminum is stuck on the tool it will keep sticking, especially with soft aluminum. Try .003-.005ipt and if you can I like mist setups on open machines like that. I use beeswax for drilling when I don't want to deal with coolant, should work for some milling it has a tendency to coat the tool when it melts and it stays lubricated surprisingly long.

If you feel like dealing with a bottle of muriatic acid in your shop(keep it away from steel you don't want to rust) you can soak your tools in it and it will remove the aluminum without touching the tool. Lye also works slower but is less of a hassle as muriatic is to store and dispose of. Once you have them clean just try to keep them that way as long as you can.

Here is my design for a mist system. It works well for me and not too difficult to make.

https://grabcad.com/library/mist-coolant-nozzle-1

Guys, you have no idea how much I appreciate the help.
This is all great info.
One of the issues with starting a new hobby, is existing in a vacuum with no local support network. You guys have been great in filling that void.

I started responding as a single post, but as it got long, I'm breaking it up into smaller chunks.

Material used and selection:

I don't know what type of aluminum I got. I got it from a local recycling plant.
In truth, I don't know who to get raw materials from -- yet.

I contacted local metal supply places in Albuquerque and only one (that I found) sells non-ferrous metals and they have a $500 minimum.

As this is a home garage/shop and a developing hobby, I don't yet know what is a common size raw stock to buy.

I'd appreciate suggestions on where to source raw materials from at a reasonable prices.

Since this is a spare time, fun activity, I don't mind ordering from a place that has a longer lead time, or getting 'drops', random pieces. I also don't mind buying things by the pallet if that will make prices much cheaper.
Again, this is not a production shop and this will never be a for profit operation.

Adam (Abom79) likes to use McMaster-Carr. He does it because of a 2-day shipping, which I don't care about, and I'm not sure if those prices are competitive.
Here is a pricing for a 2"x2" 6061: https://www.mcmaster.com/aluminum/sh...ess~2/width~2/

I pulled this from eBay just now. Again, not sure if those are good prices or not: eBay 1 Inch x 6 Inch Aluminum bars

Length	Price	Shipping	Price per inch
72	$189.80	$75.32	$3.68
12	$39.40	$19.83	$4.94
24	$64.80	$24.88	$3.74
18	$45.60	$22.17	$3.77
36	$86.20	$35.65	$3.38
30	$79.40	$29.50	$3.63
48	$131.80	$60.03	$4.00
96	$206.80	$95.66	$3.15
60	$181.60	$67.09	$4.14

Any local or national sources you can recommend would be highly appreciated.

About coolant system.
I have ordered (over the weekend) this setup based on the recommendations from other folks: Mist Coolant Lubrication Spray System
If it doesn't work, I will absolutely build one of the ones recommended here -- thank you for detailed plans and writeups.

I think my machine was setup for flood coolant, but all that's left from it is a disconnected pump and a skimmer.

I'm not even sure if this pump is 120VAC single phase or 3phase.
https://www.cnczone.com/forums/attac...d=451976&stc=1

Skimmer is a straight forward 120VAC NEMA 5-15P Straight Power Cord Plug that I tested and it works.
https://www.cnczone.com/forums/attac...d=451978&stc=1

Also, since the machine is totally open, not sure if it makes sense to try to enclose it or use shower curtain I saw in another post.

I will play with the mist system and see how it goes.

For now, chips are thrown over 12' in every direction, and that will get old soon. :-)

Probably most important thing to discuss is the cutting implements.

First, thank you for the recommendations.

Looking at the cutting tools, I see that most are in the 5/8"-1". How do you deal with stock that's thicker that that?
The part posted ideally would be 1"-1.25" thick.
Obviously I don't expect to cut it in a single pass, but if a 3/8" bit has 1" flutes and a total length of 2.5", how do you profile greater than 1" tall stock? 3/8" Dia x 1" Cut 3FL Square End AlumaCut Carbide End Mill F16
I assume that the 3/8" shaft is the blank diameter and the cutting part has a diameter is equal or smaller than the shaft.

Do you keep different length cutting tools?
Or, just sink the shaft into the collet to minimize stick-out and then keep lengthening it as the depth gets longer? For example on this 3/8" Dia. x 1-1/2" Cut 3FL Square End AlumaCut Carbide End Mill F18

Or do you simply use the roughing bit at full length knowing that you will get some deflection while leaving 0.04" or so stock, and then use finishing tool for final passes?

Google "metal supply house" in ABQ, there are plenty listed, Bralco being one, Metal Mart is another. You can also check onlinemetals.com I order oddball stuff from them on occasion and if you sign up, they send you 15% and 20% coupons all the time.

That mister might work, the MQL version pressurizes the coolant and helps you run a lot lower air pressure and volume to get the desired effect. You will find compressed air is expensive and noisy. The shower curtain machine you saw is probably mine, got tired of cleaning chips up 30' away... still not perfect, but better.

End mill length, there is no one end mill fits all situations, you will need normal length, stub length and regular length. 1/2" diameter ones are commonly available in 1.25" long. If you really have to have smaller diameter with longer length because of radius requirements on inside corners, you can get shorter than needed cut length with an extended shank that is reduced in diameter. You cut say 1/2" deep at a pass but because the shank is solid it's much stiffer than having a long flute length.

With your adaptive tool path make sure your tool engagement is not something crazy like 40-60% try like 10-15% to start. Also try a 3 flute, works much better for aluminum

Quote:

---

Originally Posted by Brian L

Google "metal supply house" in ABQ, there are plenty listed, Bralco being one, Metal Mart is another.

---

Brian, I did that some time ago, but tried it just now again. Most of those places are metal roofing or metal building places.
The only one that sells non-ferrous materials is the Bralco (division of Reliance), and they're the ones that have the $500 minimum. I filled out a form for an account -- perhaps with that, I'll have an option of picking up just what I need.
I am going to look into onlinemetals.com tonight and see if that's a route I can pursue.