Inventables Community Forum

Easel Aluminum Speeds & Feeds

Yes, I did search the forum. But my Australian mm to your American weird inches confuses me. Not to mention some of your dont use easel.

I have 18mm 6061 Aluminium. I’m wanting to cut it using a 1/8 bit (3.175mm).

I used the “Recommended” settings in easel which came to 22 hours. Someone please tell me this isn’t true.

I pretty much always have my Dewalt router setting 3-4 who knows what they mean, not me. But it’s in the middle so seems like that’s what I should have it on.

Easel recommends:
FR: 124mm/min
PR: 76.2mm/min
DOC: 0.1mm

Total Machining time 22h 38min. I don’t have that long :stuck_out_tongue: someone tell me I can go to 6-900FR and .5DOC :smiley:

I have a 2 flute endmill (the one inventables sells).

I always deal in hardwood, never metal, so this is new to me. I’d rather not test on a 22 hour cut.

Choose speed setting #1 (16k RPM)
Try 1200mm/min, keep plunge/DOC as-is and see how that works out.
If that works okay try 0.2mm DOC. With Easel you can change FR on the fly to dial in further as you go.

For 0.5mm or deeper DOC you need a rigid/tight machine.

When you go deeper per cut you need to change the feed rate a little since the cutting edges now do more work, vs tip only when doing 0.1/0.2mm DoC.

Then try RPM setting 1, 640mm/min and 0.5mm DoC (320mm/min per tooth)
This allow for a chip thickness = 0.02mm per revolution/tooth.

Test on a smaller piece before going full scale.
Lubrication will also aid a fair bit, WD40 in a pinch, even air only is better than nothing so chips are cleared from the cut path.

The Dewalt manual does. This is for the 611 but it’s probably the same for the 220 version if you have it.

I’ve cut at 48 ipm (about 1200 mm/min) into aluminum with no real issues. Keep the depth relatively low (0.2mm should be fine, I think I did 0.005” which is like 0.15mm.

But overall, yes the Xcarve takes longer to cut aluminum than wood because it’s harder to cut aluminum and honestly, it’s not really what the Xcarve is designed for. Not saying it can’t, it just can’t do it very fast.

BTW - if you are doing pockets and using the 1200mm/min/0.1-0.2mmDoC set step over = 75-80% vs the default 40%
This will further reduce the carve time for pocket/facing operations.

For single line, deep slotting a nicely trammed Z is vital otherwise the shank will rub the slot walls. Chip clearing is also very important for deep slot cutting aswell.

Obstacles of cutting aluminum.

  1. Flexing you will encounter if you try to go too deep with each pass. To see the flex I am talking about simply push down on the top of your router and you will see it move due to the twisting of the gantry and movement in the V Wheels of the Z axis and the Z axis carriage. Shallow cuts help to avoid this flexing.

  2. Feed Rate is critical. Too slow and your bit heats up too much and causes the aluminum to stick to the bit. Too fast and you put too much stress on the gantry and causes flexing or twisting. This will cause the bit to wobble during the cut and can break your bit or at the very least yield a terrible cut finish. I have had success with a feed rate of 75-120 inches per minute with a depth of cut of .007". FR 1905-3048 mm/min DOC 1.778 mm) Keep in mind that I have a beefed up X Carve that has had stiffening mods applied and very good tramming. The higher feed rates keep heat buildup from melting the thin chips that come off the cut.

  3. Tramming. Your Z axis must be trammed as close to perfect as you can get it. If you are out of tram you will get wobble in your straight and ball nose end mills. V bits don’t suffer as much from a slightly out of tramm machine but they don’t like it either. If your way out of tram then a Vbit will drag in one direction and dig in the opposite direction.

  4. Bit selection. No more than 2 flutes on end mills. More flutes will collect the aluminum chips and they will stick to your bit generating too much heat. They will also start sticking to the cut you just made. If you are going to do much aluminum cutting you should get bits designed for cutting aluminum. Drillman1 has an ebay store that sells bits for aluminum. They will last longer and give you a better finish.

  5. Chip Evacuation. One of your worst enemies. The last thing you want to do is let the chips you just cut get in the way of the bit. It’s like chewing sand. Very bad. Keep some air flow going during the cut to blow them away. Air flow also helps keep the bit cool.

  6. Lubrication. Lub is for more than the more fun things in life. It will help to cool your aluminum and bit pluss keep the chips from sticking to your bit and make your bit cut cleaner. WD-40 in a spray can works well because it does more than just lubricate. It can help coll the bit because it comes out cold and also blows the chips away.

Best of luck to you. Cutting Aluminum with the X Carve is possible. I do it daily.

Charley Thomas
Triquetra-CNC

6 Likes

I was reading your comment and I was like this guy sounds like a teacher/professional! Then I seen your sign off and realized you are lkl

lkl ???