Successes Carving Metal

X-Carve
1

I am an high school engineering class teacher and my class specializes in robotics. I own an XCarve 500mm setup that I have upgraded with larger stepper motors and have stiffened my carriage with any improvements that came down the pike. Even though I need more working area, I want to keep the frame as stiff as possible. I got my XCarve because I wanted to mill aluminum. Since this was a personal expense, I could not afford to get an industrial mill.

I wanted to report a successful outcome to anyone that has had as many problems milling aluminum as I have had. I have completed the task of cutting the holes and bearing traces for the frames of 4 large robots in 1/8" aluminum bar stock 6" x 18"…

*I created the .stl file in Autodesk Inventor, and created the g-code in MeshCam. I imported the g-code directly into Easel. Since my part was double my work area, I had to develop a standard place to index each piece. I had to flip the part, reindex it and cut the mirror image on the opposite end.

  • Initially, I bought the a kit from www.SuperPID.com to control the speed of my Dewalt 611. It was very good at controlling router speed, but at speeds less than 7000 rpm the router would in 50% of the time go into a high rpm mode. After the first time the brushes failed on my Dewalt 611 spindle, I bought a new Dewalt 611 and did not install the SuperPid on the new spindle. Instead I used the lowest speed setting on the router.

  • My tool settings are: Feedrate 3.0 in, Plunge rate 2.0 in , stepover 0.0120, and step down of 0.01 in.

  • I tried all sorts of bits but a $12 set of bits from Amazon worked the best " Lukcase 1/8 Carbide Flat Nose End Mill 2 Flutes 17mm CNC Router Bits Double Flute Spiral Set Tool" All of the expensive bits had issues with running too hot, but these ran without lubrication or dust collection. I uploaded a time-lapse video.

Lessons Learned: I quickly found out how to change brushes on Dewalt 611 routers. When the LED works but it won’t run, it is the brushes. Using oil for lubrication on the stock made a mess and was not very effective.

Apparently t he upload did not work. I posted it on youtube: - YouTube

1 Like
2

Got a link to the video?

3

Are these with a 1/8" 2F bit? You should be able to significantly speed up your work times, especially with stiffening mods. I’ve added rail stiffeners and beefier belts to my X-Carve, and I run with a 1/8" 2F in aluminum at 0.005" depth per pass and 20 IPM (would be over 3x faster).

4

Dave, I tried everything under the sun. And the biggest problem I had was that the chips were so warm that I had melting. When I went 0.01 it spit out larger chips and theoretically dissipated more heat. This was a huge problem in cutting the bearing traces. In a straight run, I could double the speed without problems. I tried some very fancy, expensive bits and finally settled on the 1/8" 2f bit.

5

What grade aluminium did you work with?

I just watched your video and would like to offer you a couple of suggestions which I hope will improve you machine capability further:

  • Tool stick-out
    The end mills you used have a 17mm cutter length (height) and it looks like you have about 1" of exposed tool length. Any tool will deflect and reducing the tool length to say 1/2" would reduce the deflection by a factor of 4.
    Generally you’d try to seek minimum stick-out, just enough to reach desired depth.

  • Lubrcation
    I have previously used WD40 which work very well but I stopped using that as it left oily residue behind. I have since switched to a mister running air/denatured alcohol. This work very well for two reasons, the air remove chips and the alcohol provide lubrication and dissipate heat as it evaporate. No residue is a bonus.

Stiffness is what it all boils down to.
The stiffer machine the more aggressive one can get because the variation of chip thickness/chip load approach zero
For a 1/8" end mill in aluminium a good starting point for chip thickness (slice) is a thou (0.025mm / tooth)

Machine flexing, tool stick-out, tool deflection, runout and vibrations directly affect the chip thickness

If I were to calculate the ideal settings, as a starting point, for a 1/8" 2F end mill in aluminium this would be my math:
Feed rate = RPM x Chip Thickness x Flutes
FR = 16000RPM x 0.025mm x 2 => 800mm/min (or about 31ipm)
Depth per cut depend on the stiffness of your machine.

There is another important factor to consider, at least in the commercial world, which is cutter speed.
This is the speed the cutter tip it traveling at when bit is rotating and is called SFM aka Surface Speed / Surface Feet per Minute.

For aluminium the Surface Speed is typically 450-500m/min and this is the speed where the cutter is most efficient slicing through the material. For our typical small diameter end mills the SFM-target go beyond the RPM range of our routers as doing the math may suggest 35-60K RPM.
For simplicity we just decide the max RPM we are comfortable with.
The SuperPID and low RPM range dont really help us here since we are already on the low-side of the SFM target.

Say you go with speed setting 3, about 20k RPM.
SFM is now approx 200m/min which is less than half of target speed (450-500) - but we use what we got :slight_smile:
Targeting even lower RPM for this application is counter productive.

Calculating feed rate, based on 20k RPM (Feed Rate = RPM x ChipT x Flutes):
20000 x 0,025mm x 2F = 1000mm/min (about 40ipm)

Any deficiency within the whole system will skew the acceptable work envelope.

Dislcaimer - these values dont take the actual machine into account, every machine is different. What matters is what work for you :slight_smile:

1 Like
6

Haldor, thank you so much for sharing your information. I started out in CNC when I wore out my 3d printer with student projects. I wanted to build a giant 3d printer and mill the aluminum parts. So my experience has been to directed to certain specific goals. Sort of “hacking” the hardware to meet a particular goal. I would love to have a liquid cooling/cuttings removal system, but that is a project for another time.

You are right. Stiffening the setup would be key. The X axis was not as much of an issue as the Y axis. I had to replace belts in the Y direction frequently and believe that a threaded rod system for moving the X and Y axis would really make a difference. Because you would compress the fame elements with this sort of system, it should also stiffen the frame as a by product. It would be an amazing addition to the XCarve. I recognized that tool stick out was an issue because of deflection. However I did not want to push the cutting features of the tool into the chuck. Buying a more suitable bit would fix that, but maybe I should have tried sacrificing a chuck to get less flex on the bit.

I bought my 6061 1/8" aluminum from McMaster Carr. What I didn’t say was that I had poor success with 1/4" 6061 Aluminum plate. I think the temperature was building as I continued to cut and I would get molten slag on the bit. Rob Grzesek (MeshCAM) advocates low bit speeds and that is the reason why I went with SuperPID. Whenever I pushed the speeds higher I got the molten slag on the bit problem. The bearing traces were my biggest milling problem. Cutting those accurately were a real bear. During one trial, I had so my pressure on the bit that it took a detour and ruined a sheet of aluminum. Going slow was my only answer. .However, the new feature on Easel, the ability to increase the feed rate was helpful if I babysat the project. Don’t know whether you could see on the video, but my plunge rate was extremely slow. In real time, it took several seconds to lower the tool into the stock every time it was removed. However, there was no method to lower the tool quickly to a point just before the stock and then slowly plunging into the stock; so I was stuck with a very slow plunge rate.

Wish I knew of your research before I started on this project, it would have saved me a lot of time. On my next endeavor; I will use your work.

7

You are most likely right. I had a problem with molten slag on the bit and what I read from Rob Grzesek (MeshCAM) was that you wanted to maximize size of cuttings and spin your cutting tool at a very low rpm. I was aiming at 5K and using as much of the bit as possible. In my defense, I had a serious time crunch issue with a class full of teenagers that needed my robot parts. When I found something that worked, I stopped researching and went into production. Thanks for your input and I will try it with my next project.

8

@FrankWood1 - I can relate :wink:

My foray into CNC started about 3 years ago when I wanted to make camera sliders and started searching for mechanics, stumbled upon the Arduino which lead me to the gshield. The dream was born. Started with drawer sliders and Nema17´s… :rofl: Each upgrade from that have exposed a new weak link and evolution continues. It is now a quite capable machine. (not Xcarve)
That was the mechanical aspect of my journey, 3 years ago I didn’t know diddely about CNC´ing either like feeds and speed or such.

One of the major upgrades you may consider for your Xcarve is a better Z-axis. Several forum posters have done this in the past with excellent results. Linear slider/screw rules too.
The other is the mister, it is nothing sophisticated, all you need is some air pressure and coolant reservoir. I just use a coke bottle zipped to the gantry. The mist is “light” enough so there is no flooding at all. (Work space friendly)

If the heat isn’t allowed to escape the billet/sheet will heat up and you are on a downwards spiral for gummed up bits.
Fewer flutes = more space for chip to clear.
Too slow feed rate (read chip thickness too thin) the bit will rub more than cutting. This add to the heating situation.
But, if there isn’t enough rigidity there isn’t much one can do except go with whatever works.
As a side note, you can use caustic soda (lye) to clear the gummed up bits by submerging them in a water solution over nite. (Use proper protective gear as lye is very alkaline and will cause severe skin burns / eye damage if spilled on flesh)

Another aspect that really can skew things up is untrammed Z, as in not truly perpendicular to the X/Y plane.
This can cause all sorts of things, leading up to only two things => great frustration and poor results :wink:
Been there :zipper_mouth_face:

Straight plunge is hard for the bit as it will want to wobble, Easel dont allow for any ramping in/lead-in/out so the key is to take it slow like you did. I dont go fast either, maybe 3-6ipm if I am going straight in. Most of my designs are done in Fusion360 which open up a whole bigger world of tool strategies so if inclined get your feet wet. F360 is free for all unless you make more than $100k/year with it.

Regarding tool stick-out, use a bit with tool length shot enough to do the depth required. For 1/4" stock I´d use a end mill with 1/4" tool length or as close I can get.

BTW - I still haven’t made a camera slider… :rofl: