Help Needed for CNC Router

How do we get a better finish out of our CNC router?
My team has recently began using a CNC router to mill aluminum. We are based out of a school and have only used it for wood up until recently. It is a Forrest Scientific CNC Router(picture of it bellow).


Our set up right now has two vices bolted in the t-slots on the bed, with an aluminum milling block attached. To attach the milling block we milled holes into an aluminum box tube. We have the milling block screwed to the box tubing.
Recently we have have been practicing with cutting aluminum plate, specifically 1/4 inch plate. We milled a rectangle with our team number on it.
We faced the aluminum with a 1/2 inch 2 flute end mill(we do not have a facing mill). We shaved .003 off with a 80% stepover. RPM of 2500 and a feed rate of 5 IPM, and plunge rate of .75IPM.
We then changed bits to a 1/4 inch 3 flute end mill. We engraved our teams number(3880), a total of .0628 with two paces at .0314 each. RPM of 6000 and a feed of rate of 2.5 IPM and a plunge rate of 1 IMP.
To cut the piece out we used a 3/8 2 flute end mill. Doing six passes each at .0418 each. RPM of 3000 and a feed rate of 4 IPM and a plunge rate of .5 IMP. Bellow are different picture of the final product.

3 Likes

Given the details…

First, that’s a wood router, as near as I can tell the whole line is wood-focused. It may not have the rigidity to do aluminum. (OTOH, it might… and that’s somewhat workable.)

On to the actual suggestions.

Let’s start with the easy one. Roughing pass, finishing pass. Run that program again but this time tell it to do a finishing pass at .005"-.010" material removal on the engraving, rather than .030"+. So that would be something like .028", .028", .005". (Also applies to any expansion to the side, BTW.)

Now that you’ve seen the improvement, spin it faster. The fastest speed you noted was 6K RPM. Try 10K. If I recall correctly, my team’s Velox doesn’t do anything slower. Right about here, I suggest hiding behind a shield, though…

… because endmills are likely to have snapping problems. That’s where you get single-flute router bits instead of multi-flute endmills. Cue about 20 CDers arguing about best brand and size.

And once you’ve done that, you should be able to speed up the feedrate a bit.

Do you have any more specs on the machine? Googling doesn’t seem to help, I’m curious what the max RPM is, but like EricH said, chances are you want a higher RPM, we run ours between 10K and 24K.

  • What aluminum are you using? 6061, 6063 other?
  • Any more details on what tools are you using? I’d recommend something 3 flutes or less (seems like you are), I would get something with center cutting, and make sure the coating doesn’t contain Al (I recommend 3 flute variable helix from lake shore carbide: stub variable flute end mill for aluminum)
  • I would grab yourself a copy of G-Wizard to pick out your feeds and speeds, it’s pure magic
  • Also that working holding probably isn’t sufficient and is vibrating a lot

Looks like a very capable machine, but your feeds and speeds are definitely way off for it. Looks like you have a standard square spindle. What’s the peak RPM of this? 24k RPM or something else?

I have cutting templates for Fusion 360 you can find here. Fusion 360 works great for CAM. If you are using another software, I can parse the feeds and speeds for you. If you are not running coolant or air blast, reduce the feedrate by 40%. If you are running air blast only (highly recommend) maybe reduce by 10-20%. Mist coolant is nice but leaves a bit of a mess. Your vacuum/dust collector shoe will be a good substitute for an air blast if you can hook it up.

You will want a good endmill. I recommend reaching out to Grewin and getting a pack of 20 4mm endmills and 10 6mm endmill for cutting aluminum, with “sharper tip for plunging”. These are high quality and quite cheap, about $130 shipped for that many. I can send you some of these right now if you will replace them for me later. If you don’t want to get a quote from Grewin, The Thrifty Bot and West Coast Products both sell good endmills. You can also get 4mm x 12mm Huhao endmills if you want a few “practice” bits. My templates will work with any of the above bits, but you can probably crank the feedrates up down the line for the non-Huhao ones.

Definitely looks like a machine that will chew through aluminum if you set it up correctly. Get some good endmills, better feeds and speeds and CAM, and an air blast or vacuum, and you’ll be ready to make some nice parts.

EDIT: forgot to mention. To fixture your aluminum plates, I recommend using wood screws and washers around the edge of the large aluminum stock, maybe a 4x4’ in your case. Drill all the holes in your parts (you will want to do multiple at once), and then screw them down into the MDF wasteboard with #6 stainless steel flathead woodscrews. Then run your pocketing and cutout operations. This will make really clean parts and allow you to maximize throughput by machining many parts at once. You will want to stack a couple pieces of MDF on top of your existing one so as to avoid ruining the existing bed.

7 Likes

The name of the machine is Makerfab 4800 4x8 5-Axis CNC Router. The max RPM is 18k. We have been cutting on 6061 aluminum. All our bits are uncoated HSS and center cutting. We have 2 and 4 flute of most common bit sizes. We have found that the work piece does not vibrate but rather the whole gantry has very small vibrations. Still, what holding set up would you recommend?

Definitely switch to carbide single-flute endmills first. 2FL HSS will need a much lower RPM and feedrate, and overheat more easily.

4 Likes

RPM = SFM * 3.82 / Diameter
Aluminum SFM = 400 ---- 1000
RPM = 400 * 3.28 / .25
RPM = 6100 (approx)

Feed = RPM * NumofTeeth * Feedpertooth
Feedpertooth for a 1/4" = .002 (Alum)
Feed = 6100 * 3 (flutes) * .002
Feed = 36.6IPM

So if the machine is not rigid, lower your depth of cut. DOC of .0314" seems about right. Adding a finishing pass of 0.01" would probably clean it up a lot. Does look like a lot of flex on that plate with the engraved numbers. Those multiple circles on the the flats look like the bit is bouncing or the aluminum is flexing. If you are not using air or mist, those bits can gum up. Recommend ZrN coating, helps reduce the gumming. Do not use any of the Ti coatings, these are designed to get hot and do not reduce friction until they are hot. Hot aluminum = bad. Also I do NOT recommend trying to mill any of the 5000 Al alloys. 6061 should mill nicely.

If one is using single flute carbide endmills, 5000 alloys mill fine in my experience. 3 flute endmills will quickly gum up on any alloy when slotting on a router once the aluminum warms up - I’ve always had to go to 1-2 flutes when cutting out for this reason. I imagine that larger CNCs with higher pressure flood coolant keep chips evacuated better and don’t suffer from this issue.

Are you really running at 2.5 inches per minute feed rate? This would give you a chip load of:

Feed (IPM) / (Speed (RPM) * Teeth/rev
2.5 / (6000 * 3) = 0.00014 inches/tooth

At this chip load, the bit teeth don’t really have any material to cut into. A a couple thousandths, like @pryland mentions, the bit can dig in and cut out a nice chip. At 1.4 ten-thousandths, the bit does more rubbing on the material than it does cutting. The rubbing generates heat. From the close-up photos of your completed cut, there appears to be evidence of melted aluminum welding to the top surface of the part.

With router RPMs you should be cutting aluminum with a single-flute bit. Your feed rate has to go way up to stop the rubbing.

Most spindles do not run well at less than 1/3 of their max speed. The torque tends to drop off rapidly at slow speeds. If your spindle max is 18K RPM, you should probably not be running it at less than 6K RPM. If it’s an air-cooled spindle with the fan driven by the spindle (not an independently powered fan), the spindle cooling will not be sufficient at less than 1/3 of max speed.

Recommendation:

  • Switch to single-flute carbide endmills. If you are looking for the clearing rate of a 1/4" tool, 6mm tools are close in size and are likely available at lower cost.
  • Run your spindle in its power sweet spot. For a 6mm bit at 12K RPM you’d be at 864 surface feet per minute, which should be fine for aluminum.
  • Run at least 0.002 inches per tooth chip load. For single-flute bits at 12K RPM, this means 24 inches per minute feed rate.
  • Start with light depth of cut and increase as your machine can handle. You could start with just a couple hundredths if you want to be very conservative. Work your way to deeper cuts if the lighter ones are working.
  • You could also work toward higher chip loads. Most 6mm bits can handle 0.004 chip load. Moving to 40-45 inches per minute feed rate may be possible.
  • A mister is a wise investment for cutting aluminum. Without a mister, spraying something like KoolMist from a spray bottle is better than cutting dry. WD-40 is actually pretty helpful for cutting aluminum, but it’s less safe (MSDS signal word DANGER vs. WARNING for KoolMist). If cutting dry, a compressed air blast helps to evacuate chips from the cutting zone. Re-cutting chips is another way to make melted aluminum.
1 Like

This topic was automatically closed 365 days after the last reply. New replies are no longer allowed.