# CNC Machine - for home-building aircraft

Discussion in 'Workshop Tips and Secrets / Tools' started by Rienk, Apr 17, 2015.

### Help Support HomeBuiltAirplanes Forum by donating:

1. Apr 25, 2016

### Rienk

#### Well-Known Member

Joined:
Oct 11, 2008
Messages:
1,364
190
Location:
Santa Maria, CA (SMX)
Yeah. it's a matter of the material being stiff enough to stay down on the table. I'd be worried that as you begin to cut, the tool starts pulling the material up, or it just chatters so that the edge is worthless. The former might be mitigated by using a down feed bit, but I'd definitely have someone experiment a bit before you made such an investment
Some cnc lasers can cut thin aluminum, but I believe the power requirement is at least 250W - and they're expensive.

Fritz, have you tried cutting thin sheet metal? If so, what were the results, and are there tricks that make it work well?

2. Apr 25, 2016

### Algoa

#### Well-Known Member

Joined:
Nov 26, 2008
Messages:
101
18
Location:
Houston, Tx
FWIW: I built my own 4'x8' shop CNC out of ordered parts (not a kit). While I haven't totaled up the entire cost, I would guestimate it at $1000 -$1200 including mistakes. The table and gantry are made from welded steel square tube with parts ordered mostly from Amazon and OpenBuilds.com

Here it is cutting some 040 6061-T6 yesterday.

nucleus likes this.
3. Apr 25, 2016

### Rienk

#### Well-Known Member

Joined:
Oct 11, 2008
Messages:
1,364
190
Location:
Santa Maria, CA (SMX)
Nice!
Can it cut as thin as .016" with no problems?
How much time do you have into building it?

4. Apr 25, 2016

### Algoa

#### Well-Known Member

Joined:
Nov 26, 2008
Messages:
101
18
Location:
Houston, Tx
Yes, it can cut .016. Since I haven't made a vacuum hold-down surface for it yet, I use a down spiral bit instead of the more usual up spiral since the up spiral will try to lift the sheet off the surface as it cuts. I also screw two corners to the MDF sacrificial surface and use a climb cut.

proppastie likes this.
5. Apr 25, 2016

### Rienk

#### Well-Known Member

Joined:
Oct 11, 2008
Messages:
1,364
190
Location:
Santa Maria, CA (SMX)
There you go Don - time to build/buy yourself a CNC!

6. Apr 26, 2016

### proppastie

#### Well-Known Member

Joined:
Feb 19, 2012
Messages:
3,779
1,094
Location:
NJ
double post

7. Apr 26, 2016

### proppastie

#### Well-Known Member

Joined:
Feb 19, 2012
Messages:
3,779
1,094
Location:
NJ
When the aluminum dragon is finished, and refined to such a state that I am looking for another project it sounds like a good possibility. unless something pops up with CAM software close and cheap.

8. Apr 26, 2016

### FritzW

#### Well-Known Member

Joined:
Jan 31, 2011
Messages:
3,627
3,252
Location:
Las Cruces, NM
What are you using for feeds and speeds? I downloaded a calculator but I must be using it wrong. Every time I cut aluminum I have to mess it a bunch to get a clean cut.

You can see on the far edge of this seat pan that the material started melting ( .025 6061 T-6)

9. Apr 26, 2016

### ScaleBirdsScott

#### Well-Known Member

Joined:
Feb 10, 2015
Messages:
1,033
656
Location:
Uncasville, CT
Melting aluminum with a router? That's cray.

I use single flue 1/8" upcut carbide endmills, speed around 40-60ipm at 12000rpm max .03" DOC, and it cuts like a madman even on my dinkbot. Your CNCRP based unit should be able to clobber along at faster feeds.

The main killer of bots is running too slow a feed where the bits can heat up and smoke. After a cut job my bits are cool to the touch. If I'm getting any heat at all with carbide in alum it means rub, and rub is the mill-killer.

10. Apr 26, 2016

### Algoa

#### Well-Known Member

Joined:
Nov 26, 2008
Messages:
101
18
Location:
Houston, Tx
As I recall, for 040, I am using a feed speed of 23ipm (I didn't say it was fast, just that it is a lot faster and more accurate than me with snips). It might could go faster, but I am happy with the quality I am getting and feel no need to push it to the limit. No heat issues at all. That speed should work for everything thinner. The Bosch Colt router I am using has spindle speeds from 16,000-35,000 rpm and I have it turned up half-way so I am guessing the spindle speed is around 24,000rpm. I didn't start getting consistently good results until I started using the Whiteside RD1600 down-cut spiral bit in a climb cut.

FritzW likes this.
11. Apr 26, 2016

### ScaleBirdsScott

#### Well-Known Member

Joined:
Feb 10, 2015
Messages:
1,033
656
Location:
Uncasville, CT
Interesting that downcut works for you, everytime I try downcut I get nothing but an aluminum heat-death of the universe. The upcut does lift the sheet some but we mitigate that with tape, screws, etc, and the result is chips everywhere, but never any chance of swarf clogging the action.

I go fancy with the OMT Onsrud cutters. They work. If I need bulk I sometimes have gone and gotten the chinese 10 for $20 bits that should fit the bill in theory but are not 100%. They are good for backup when you just need to barrel through a job and its the weekend and even Amazon Prime can't save you, breakage or no. Surpsiringly I also have good enough luck in a pinch going to Home Depot and getting a Diablo 1/4" 2-flute upcut carbide bit for$20 and it's also the type of bit I prefer for cutting MDF sheet so win-win. They seem to be to just be re-branded Freud router bits so they're OK quality-wise tho nothing astounding, and it certainly will do the job; you have to really try to break 1/4 inch bits with this stuff, though I've smoked and smashed my share.

12. Apr 26, 2016

### FritzW

#### Well-Known Member

Joined:
Jan 31, 2011
Messages:
3,627
3,252
Location:
Las Cruces, NM
Why is that crazy? ...it's, by far, the most common problem I've had with cutting aluminum, actually it's the only problem I've ever had cutting aluminum.

I think I'm running too slow. I started at (IIRC) 16,000 rpm at 40 ipm on an 1/8" two flute, low helix, carbide bit using WD-40 as a coolant. I switched to 14,000 rpm at 60 ipm and used aluminum Tap Magic. It finished okay but still not as pretty as I'd hoped.

13. Apr 26, 2016

### ScaleBirdsScott

#### Well-Known Member

Joined:
Feb 10, 2015
Messages:
1,033
656
Location:
Uncasville, CT
The only times I've had bits go bad in aluminum and cause the edge to start going gnarly are when I was trying to get away with non-carbide when they gum up within a foot of cutting; when I've turned the spindle on in reverse like a moron and just caused mayhem, or when the material lifted enough to start just rubbing on non-cutting shank where obviously it just becomes a really terrible friction welder and immediately causes a bad day. And I guess if I try too heavy a depth of cut, (like trying to go .06+ into a chunk of 1/8" plate... yeah, you're gonna have a bad time.)

In normal cutting, into aluminum sheet, I've never had to resort to any kind of coolant or lube or wax. In fact you might find that if you're using WD or similar it could be contributing to heat?

I'd probably drop the RPM down a little from 16000 at 40ipm, I get away with 10-12k, and definitely go to a single flute carbide cutter advertised for aluminum such as this one here so the material engagement is halved from 2-flute, and run it dry to reduce the mess and fuss and potential for it to steam off. With carbide, the chips can easily carry away all the heat from cutting alum sheet.

14. Apr 26, 2016

### FritzW

#### Well-Known Member

Joined:
Jan 31, 2011
Messages:
3,627
3,252
Location:
Las Cruces, NM
24,000 is about the limit of my spindle. But 24,000 rpm at 3.2 hp is past my comfort limit (this thing gets loud and scary when it's wound up :gig: ) I'll give it a try next time though. ...and 23ipm is a whole lot faster than I can go with tin snips.

Algoa likes this.
15. Apr 26, 2016

### ScaleBirdsScott

#### Well-Known Member

Joined:
Feb 10, 2015
Messages:
1,033
656
Location:
Uncasville, CT
As an FYI for those who havn't seen it yet, most of my successful attempts at routing aluminum can be linked back on this article:

https://blog.cnccookbook.com/2012/03/27/10-tips-for-cnc-router-aluminum-cutting-success/

I have yet to see where the article is flat wrong though there's always the YMMV caveat. According to the article I pushed my travel speeds up, Ripems down, stuck with single-flute coated carbide cutters, and make sure to always have a vac/dust-collector going with a handy brush and air blast for clearing bunches of chips, and all is gold.

16. Apr 26, 2016

### Algoa

#### Well-Known Member

Joined:
Nov 26, 2008
Messages:
101
18
Location:
Houston, Tx
Unlike ScaleBirdScott, I never found anything at Home Depot that would render acceptable results for me. I use a quality 1/8" two-flute, he uses a quality single flute. I use something over 20,000rpm, he uses something just over 10,000rpm. I do good to cut at 24ipm (rigidity issues), he rips along at triple that speed.

The point here I think is that what works for you works for... you. In the black art of getting a CNC table router to cut 6061 you just have to play with your variables and bits until you get something you like. I took a 2x2 square of .040" 6061 and made at least three dozen 6" cuts in it along both the X and Y axis before I found something l liked. It CAN be done, you just gotta find your rig's sweet spot.

17. Apr 26, 2016

### ScaleBirdsScott

#### Well-Known Member

Joined:
Feb 10, 2015
Messages:
1,033
656
Location:
Uncasville, CT
I can concur with that part, for sure. I'm not suggesting that my way is best or applicable to any other machine. I do think that there's some universal things to machining that are sometimes counter-intuitive and where I started slow and conservative, I've run into plenty of broken \$20 bits on the way to good settings. So I've had to try things that felt like they should be wrong only to find things cut great, even when it occasionally sounds pretty bad as I push the rigidity envelope. So I've run slow and been happy with that but found I had better results as I tried going faster as the recommendations were telling me. So yeah, try things multiple ways. See if there's a speed range that works, and trust that maybe ones that don't seem like the 'safe' bet can actually work well. Going fast and taking heavy chipload or going slow and shaving off swarf or somewhere in between, there's only one way to find the right combo for a homebrew machine, and that's to experiment.

Rigidity and stepper power and those things directly influence what speeds are reasonable to feed at, but I will say someone using steel track like the CNCRP-based units, and any sort of decently powered NEMA-24 steppers, should be able to handle cutting passes of 60-120ipm easily. If not, something might be off with the hardware. It should be able to handle more load than my machine at least.

Also the spindle itself may be a factor. I'm using a Chinese spindle with ER-20 collets and it might handle cuts different from using a router tool. (Also my bearings are starting to get blown out so its about time to swap 'em) But that is a factor for sure in terms of rpm selection.

18. Apr 26, 2016

### davedpilot

#### Guest

Hi

I know routers run at very high RPM's, but here are some basic formulas you can use for speed and feed.

If you know the fpm use: N(RPM) = 12*V / PI*D, where V = cutting speed in feet per minute and D = diameter of tool.

example: 2 fpm using ø.125 tool, 12*2 / PI*.125 = 61RPM

If you know the RPM use: V(fpm) = PI*D*N / 12

example: PI*.125*10000 / 12 = 327fpm

These are perfect world formulas and your mileage may vary.

Dave

19. May 5, 2016

Joined:
Oct 11, 2008
Messages:
1,364