Nomad aluminum milling question

So I am really excited that I finally milled my second aluminum part, this time a plastic mold and it works and the part looks great.

Questions:

  1. the surface finish isn’t as smooth as I would suspect. Anyone have a good tips on how to make the finished milled pocket look perfectly smooth?

  2. I mill rough cut with the .125 and finish with the .625 endmill. The .625 left rough streaks when doing y clean up. Any suggestions?

They’ll need a lot more than that to truly nail what will help.

Feeds and speeds, photos, any background info.

Otherwise it’s just the same song and dance to try to cut aluminum.

Yea fair point. I was thinking more general but here is the detail.

The roughing pass was 10000rpm, 276mm/min feedrate, 31mm/min plunge, .8mm depth per cut. 2.5mm step over (#102-z cutter)

Finishing path 5000rpm, 276mm/min speed, 32mm/min plunge, .2mm depth per cut. .6mm step over. (#112-z)

1 Like

I really want the bottom and sides to have a mirror finish.

I’m suspecting a cam issue. Those toolpath marks dont look like the correct finish passes.

Also what chiploads were you cutting at?

Its very hard to get a mirror finish right off the machine but relatively easy to hand polish to a great looking part if its cut correctly

2 Likes

Based on some online calculator the chip load for the finishing pass is: 0.0011 inches per flute. Using meshcam v7.

Is that with thinning included? You should be able to go much lower without rubbing on a finish pass. For a 1/16 maybe 0.0005-0.0008 and you could go a little lower on doc. Sorry, i’m not great with metric

In something like fusion you would do a adaptive toolpath to rough, leave 0.005 radial/axial, horizontal toolpath to finish the floor and a 2d contour to clean the inside wall and cut the outer shape out of the plate.

What did the machine sound like when cutting?

1 Like

I see several things here.

First, you are not using a finishing strategy for the walls of the pockets, hence the scalloping. Depending on the CAM tool there are different ways do this, but, as Vince said, you want to leave a little for the finish pass. It doesn’t appear you used a finishing type toolpath at all. On a Nomad with aluminum, I might leave 0.02 to 0.05mm (0.0008 to 0.002") for a fine finish pass.

I can’t tell from the picture what tool you were using, but I am guessing it is a flat (square) end tool for both the 3.2mm (0/125") and the 1.6mm (0.063") diameters.

The scalloping on the walls looks like no appropriate finish pass strategy was used. On MeshCam, IIRC, a waterline pass will do this. On Fusion360 or Inventor, the 2D-contour tool will do it. This is intended to take off a minimal quantity of material so as to control tool deflection and chip loading to get the best finish you can. TOO shallow may allow the tool to rub rather than cut, and this depends on the material and the rigidity of the tool/machine. On something like POM (Acetal) or PMMA (acrylic), ect., a little more radial engagement might be needed, as the material will deflect under the cutter. The side of the cutter can leave quite a fine finish.

For the bottom, you can likely improve it by taking a light finishing pass, but you will probably need further finishing work to get rid of visible texturing from the corners of the tool and, possibly, swirl marks. THis is just the nature of the beast, and is a concern no matter what the machine. The better the finish overall, the more these marks stand out. This is one reason why many parts have an intentionally grainy or textured surface: to hide imperfections.

In general, the LARGER the tool, the better the finish, within the constraints of machine power and part geometry. Unless you need to to get into a small corner, I would avoid the 1.6mm tool and stick to the 3.2mm. This reduces deflection and tendency to form deep scalloping, as well as allowing the higher surface speed needed for a good finish.

The surface speed at 10000RPM for the 3.2mm tool is 100m/min (300 ft/min) which is in the range for aluminum with carbide, and reasonable for a finish pass. The 1.6mm tool will be about 50m/min, which is the low end for Al, and, in my opinion, a low for a fine finish.

1 Like

First, you are not using a finishing strategy for the walls of the pockets, hence the scalloping. Depending on the CAM tool there are different ways do this, but, as Vince said, you want to leave a little for the finish pass. It doesn’t appear you used a finishing type toolpath at all. On a Nomad with aluminum, I might leave 0.02 to 0.05mm (0.0008 to 0.002") for a fine finish pass.

In meshcam I didn’t see an option to do this, or is it an obvious miss? This makes sense to me.

I can’t tell from the picture what tool you were using, but I am guessing it is a flat (square) end tool for both the 3.2mm (0/125") and the 1.6mm (0.063") diameters.

Yes,exactly, Tool #102-Z and #112-Z.

The scalloping on the walls looks like no appropriate finish pass strategy was used. On MeshCam, IIRC, a waterline pass will do this. On Fusion360 or Inventor, the 2D-contour tool will do it. This is intended to take off a minimal quantity of material so as to control tool deflection and chip loading to get the best finish you can. TOO shallow may allow the tool to rub rather than cut, and this depends on the material and the rigidity of the tool/machine. On something like POM (Acetal) or PMMA (acrylic), ect., a little more radial engagement might be needed, as the material will deflect under the cutter. The side of the cutter can leave quite a fine finish.

I am new to this so while I did add a finishing pass there is a good chance I did it wrong. In V7 release 27 I didn’t see an option for waterline just finish path overall. I did do a 2.5D run which dragged the bit all over the bottom. I think what you are saying here makes sense and probably 2D would have probably been better.

The surface speed at 10000RPM for the 3.2mm tool is 100m/min (300 ft/min) which is in the range for aluminum with carbide, and reasonable for a finish pass. The 1.6mm tool will be about 50m/min, which is the low end for Al, and, in my opinion, a low for a fine finish.

So are you saying for the finish pass I should be having the tool run through the material much faster then roughing? 100m/min seems really fast. I ran at 276mm/min.

By the way, note only the large pocket and most of the air lines. The very bottom of the airlines is ugly because I left some material and had to manually grind it away. The scalloping is totally what I am seeing on the bottom and sides. The roughing pass actually seemed cleaner.

Depending on endmill flute design and geometry the tool might actually be cutting better with a higher tool pressure. Im not a big fan of the cutters they have offered but the aluminum specific ones coming out soon are nice!

Endmill stickout wasnt anything crazy right?

What was the work holding setup like?

Bolting/clamping down is always best to ensure no movement.

Keep in mind even on large production machines with latest tools will still require hand work to get a mirror finish. Just to keep things realistic on these small desktop machines.
You should be able to get a much better surface finish, but mirror is pretty much out of the question

There are two speeds involved. One is the surface speed of the cutting edges (how fast the cutting edge moves through the material), which is controlled (mostly) by the tool diameter and RPM. 3.2mm*\pi*10000RPM=100m/min. The other is the feedrate, which is your 276mm/min. This is the rate at which the tool centerline advances. The two of these together determine the chip load-- how far the tool centerline advances between successive cutting edges meeting the material. How deep the tool is into the material (radial) combined with this determines the actual chip thickness.

The speed the cutting edge moves through the material has a lot to do with the finish, as does the chip load and the depth of cut.

As an example of the difference between surface speed and feed rate, consider a bench grinder. The surface of the wheel may be moving at 5000FPM (1.5Km/min), but the material is advanced across it at a rate of only a few feet per min (a few m/min) when cutting.

Finish passes may be run at higher feedrate than the roughing in many cases, since there is generally a lot less material being removed, but not that much higher…(EDIT: running a finish pass at higher rate presumes a number of things, and in NOT something I would be doing here.)

The toolpaths I am talking about are waterline (which for a vertical surface will follow the surface at progressive depths) and “pencil cleanup” (which traces the bottom edge). See http://www.grzsoftware.com/blog/bimages/2013/osxbig.png … I don’t use MeshCam much, but the version I have is roughly the same layout. I would run waterline passes to get rid of the scalloping, and, if needed, a pencil pass to finish. You want to have enough material left to cut that you get cutting, not rubbing for this, and you need a tool with sufficient depth-of-cut (for a 10mm deep pocket, the tool needs to have at least a 10mm depth-of-cut-- from the tip to the end of the cutting edge must be at least that. The tools Carbide sells, IIRC, are 12.7mm and 19mm depth-of-cut)

I guess I should clarify. When I meant mirror I didn’t mean a perfectly polished mirror finish. Sorry that’s my bad. I just meant a smooth even look not the scalloped look. I think you guys gave me enough things to try next time.

I will suggest that you test with a material such as pine before running on aluminum. You can up the feed to 150mm/min or more to get a quick read on what the result will be.

This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.