Facing Aluminum on the S03

Talk about all things CNC
Post Reply
heathenx
Posts: 114
Joined: Thu Apr 02, 2015 10:59 am

Facing Aluminum on the S03

Post by heathenx » Tue Sep 01, 2015 4:40 pm

So...I have been playing around with facing aluminum on my S03. First I tried my micro flycutter from Micro-Mark. I don't really have a proper way to grind the cutter prior to use so I did my best. With wood, it cuts great. Leaves a level surface with no burrs. Feels like I sanded the top. However, when I tried this on aluminum I got heavy swirl marks and it was quite rough. I think I need a rounded tip on the cutter and I ground it to a point.

Next up I tried just a 1/4" flat end mill. Ran my settings at about 20k rpm, 10in/min feed, .20" stepover with a .008" stepdown. I ended up with ridges or burrs on the surface that I could feel with my fingernail. I also cut both ways, Y and -Y.

Next up I tried a rounded 1/4" flat end mill with a .06" radius. I ran it at 20k rpm, 10in/min feed, .008" step down, .12" stepover and this time tried conventional milling instead of back and forth cutting. All the cutting started from the left side and rpid fed back to the left after a pass. I got quite satisfactory results. Finish was very smooth with no rough pass burs. I could still feel slight humps when I walked my finger nail across the surface but it was very very minor. I almost don't feel it at all. This appears to be my best cut and it's what I will use going forward until I can come up with something better.

Questions for the aluminum people out there: Any tips and tricks for facing? What cutter are you using? Speeds and feeds?
Attachments
face2.jpg
HSM Express
face2.jpg (210.57 KiB) Viewed 1490 times
face.jpg
Scrap material
face.jpg (287.73 KiB) Viewed 1490 times
Shapeoko 3, #405 / Dewalt 611 w/Super PIDv2, limit switches

TomDChi
Posts: 184
Joined: Wed Mar 18, 2015 2:36 pm

Re: Facing Aluminum on the S03

Post by TomDChi » Tue Sep 01, 2015 5:38 pm

Is that this endmill:

https://www.engman-taylor.com/Engman-Ta ... 3/P1070820

What is the thinking on radiused vs. straight mills for facing in this type of setup? (I could imagine arguments either way.)

Is it realistic that this small vise mounted on MDF may be flexing on each pass, resulting in the minor surface imperfections you're seeing? I wonder if sandwiching a larger steel or aluminum plate between the vise and the wasteboard would spread out the force/give a longer lever arm and thereby reduce any flex?

I have a bigger vise and a ZrN coated, straight endmill. I'll add facing and trying your options to my "to do" list.

chamnit
Posts: 376
Joined: Tue Aug 12, 2014 2:16 pm
Location: Albuquerque NM, USA
Contact:

Re: Facing Aluminum on the S03

Post by chamnit » Tue Sep 01, 2015 5:56 pm

It's probably a combination of the MDF base, the cutter tool path, tool deflection/rubbing, and the stiffness of the SO3 (belts, wheels, etc). Any small vibrations in the machine will translate to noticeable surface finish flaws. A good tool path will also help with lessening vibrations because the tool is cutting the material efficiently, rather than rubbing against it. You may actually need to go at a faster feed rate, since your RPMs are so high. I typically use FSWizard to calculate speeds and feeds, but be careful. It assumes you have a very-stiff production mill. I'd always look at the cutter force output and make sure it's below something like 2-3lbs for a SO3 and you have at least 0.001" per tooth chip load. And start out very conservative.

That said, it's pretty hard to get a perfect surface finish when milling metals. A fingernail can feel imperfections down to 0.0001" or a few microns.

If you are wanting to a facing operation in a traditional sense, the best way to do it is with a fly cutter. It usually gives the nicest surface finish in the least amount of time, since you are machining a wide path.

heathenx
Posts: 114
Joined: Thu Apr 02, 2015 10:59 am

Re: Facing Aluminum on the S03

Post by heathenx » Tue Sep 01, 2015 6:20 pm

TomDChi wrote:Is that this endmill:

https://www.engman-taylor.com/Engman-Ta ... 3/P1070820

What is the thinking on radiused vs. straight mills for facing in this type of setup? (I could imagine arguments either way.)

Is it realistic that this small vise mounted on MDF may be flexing on each pass, resulting in the minor surface imperfections you're seeing? I wonder if sandwiching a larger steel or aluminum plate between the vise and the wasteboard would spread out the force/give a longer lever arm and thereby reduce any flex?

I have a bigger vise and a ZrN coated, straight endmill. I'll add facing and trying your options to my "to do" list.
That endmill looks to be about the same thing that I have. My endmill is actually from Kodiak Cutting Tools (http://www.kodiakcuttingtools.com/produ ... ght=151083). I actually bought this endmill for something else. I thought since it had a radiused edge that it might clean up the surface a little better. It did at the cost of a lower stepover.

The vice could be flexing, I suppose. I hadn't thought of that.
chamnit wrote:It's probably a combination of the MDF base, the cutter tool path, tool deflection/rubbing, and the stiffness of the SO3 (belts, wheels, etc). Any small vibrations in the machine will translate to noticeable surface finish flaws. A good tool path will also help with lessening vibrations because the tool is cutting the material efficiently, rather than rubbing against it. You may actually need to go at a faster feed rate, since your RPMs are so high. I typically use FSWizard to calculate speeds and feeds, but be careful. It assumes you have a very-stiff production mill. I'd always look at the cutter force output and make sure it's below something like 2-3lbs for a SO3 and you have at least 0.001" per tooth chip load. And start out very conservative.

That said, it's pretty hard to get a perfect surface finish when milling metals. A fingernail can feel imperfections down to 0.0001" or a few microns.

If you are wanting to a facing operation in a traditional sense, the best way to do it is with a fly cutter. It usually gives the nicest surface finish in the least amount of time, since you are machining a wide path.
What I do figure out spindle speed is start the cut as slow as I can and then as it's cutting ramp up until I hear a good sound in cutting. I've tried FSWizard, plugged in good values and got horrible results. It had me cutting things way too fast. Not ideal for the S03. I've fallen back on what I "sense" is right. I'm sure I cut and move way to conservatively but I don't want to damage anything. Nevertheless, I'll try increasing my feed rate by 5in/min and see what happens.

I'd much rather use a flycutter than a small endmill but again, I'm not so good at grinding bits. Can't find any for sale that are already ground. Too bad.
Shapeoko 3, #405 / Dewalt 611 w/Super PIDv2, limit switches

Gadgetman!
Posts: 1061
Joined: Sun Aug 25, 2013 12:44 pm
Location: Norway
Contact:

Re: Facing Aluminum on the S03

Post by Gadgetman! » Tue Sep 01, 2015 7:03 pm

Have you verified that your Z-axis is perfectly vertical, and that your spindle is mounted perfectly parallel to it?
It doesn't take much of an error before it becomes visible in the cuts.
I'm currently adjusting my SO after a rebuild, and I'm using 0.1 and 0.01mm(0.004 and 0.0004") metal shims to get it as close to perfect as possible.
(You can find the most wonderful things on eBay... )
I've only just begun on the Z-axis and boy are there opportunities and issues there...

To find the 'right' speed for a tool I use a zig-zag cut test.
0/0 - 50/15 - 0/30 - 50/45 - 0/60 in X/Y coords, and slowly increase speed and depth of cut.
Then I examine the cut for distortions (usually at the corners) and the width.
Note that this cut will result in conventional milling at half the corners and climb milling at the other half as it starts on the return leg, so the corners may have different distortion patterns.
When it distorts visibly or the tool breaks(!), you generally drop down 20 - 25% to find a safe setting.
Weird guy...
Shapeoko 2014F: 1000mm X/Y, 300W Quiet Cut spindle, Arduino Uno/G-shield and GRBL 0.9i
15x30 drag chains, custom spindle mount, 9mm belts, 8mm endplates, 6mm motor plates.

heathenx
Posts: 114
Joined: Thu Apr 02, 2015 10:59 am

Re: Facing Aluminum on the S03

Post by heathenx » Tue Sep 01, 2015 7:27 pm

Thanks for the tips Gadgetman. I've just finished shimming my vise with round shims that I bought from McMaster. Going to see if that alone will improve things before moving on to other things. I have a number of these shims in various sizes. (http://www.mcmaster.com/#standard-washer-shims/=yr3a9l)

I too suspect that my Z axis isn't precise and no, I haven't checked it. Maybe that explains some of the burrs that I was getting with the flat end mill.
Shapeoko 3, #405 / Dewalt 611 w/Super PIDv2, limit switches

Gadgetman!
Posts: 1061
Joined: Sun Aug 25, 2013 12:44 pm
Location: Norway
Contact:

Re: Facing Aluminum on the S03

Post by Gadgetman! » Tue Sep 01, 2015 7:38 pm

The vise isn't an issue here. If that was out of true, but the spindle was perfectly aligned to the rest of the machine, you would still get a flat result, just not at the level you'd expect across the workpiece.

Clamp down a piece of plywood or something, and cut a shallow trench along the Y-axis, and one along the X-axis.
These cuts will be parallell to the X and Y-axis on your machine, and can be considered 'flat'.
Place a machinists square on the Y-cut and move the carriage up to it. The front of the carriage should be perfectly level with it. If it isn't... loosen the ends of the X-axis and twist until it is correct. (You may need to cuts, one on either side of the machine)
Then compare the spindle with the square.
Also check the side of the spindle and the Z-axis while you're at it.

EDIT:
BTW: What's the thickness of your shims?
Weird guy...
Shapeoko 2014F: 1000mm X/Y, 300W Quiet Cut spindle, Arduino Uno/G-shield and GRBL 0.9i
15x30 drag chains, custom spindle mount, 9mm belts, 8mm endplates, 6mm motor plates.

heathenx
Posts: 114
Joined: Thu Apr 02, 2015 10:59 am

Re: Facing Aluminum on the S03

Post by heathenx » Tue Sep 01, 2015 10:23 pm

Sounds like a plan. I'm a bit short of wood material at the moment. I have a slab of MDF at work that I could use. I could use my flycutter on that.

I shimmed my vice about .024" on one end. I didnt realize it was that far out. I have .004", .008", .012" and .020" shims. They are all millimeter shims actually. I use these at work for a bunch of things.

After i shimmed my vice, I faced again. I was satisfied with the result but think I can still make improvements. Im within .002"-.003" flatness from one end to the other now. Not bad. I also laid it down on my belt sander to remove the swirls. Looked good afterward.
Shapeoko 3, #405 / Dewalt 611 w/Super PIDv2, limit switches

TomDChi
Posts: 184
Joined: Wed Mar 18, 2015 2:36 pm

Re: Facing Aluminum on the S03

Post by TomDChi » Fri Sep 11, 2015 9:33 pm

I ran some test cuts and got those ridges. I shot some video of it running, which I'll post when I have some time to put the footage together.

It was 6061, mounted in a "precision milling vise" (Shars nominal 3" - big enough that it should have countered flexing the MDF base, but "precision-ish" - though that shouldn't have had an effect - I wasn't flipping the piece or anything.) I used a 0.25" square end, ZrN coated, 2 flute end mill.

I used a "back and forth" pattern, so the different climb/non-climb may have played a role in creating the ridges. If I can figure out how to make the "face passes in one direction" option mirror image the pattern, I'll test both ways to see if one is better/worse than the other. It would also be interesting to see if I can get this to run in the mostly Y axis direction, as opposed to right/left (mostly X) and see if that does anything different.

Post Reply