I only have one shot at it so I need advice 0.200 aluminum

Ok, I have a very cool idea of a detail picture made of aluminum. The aluminum is 0.200 thick. I plan to use a 1/16 cutting diameter bit on a DeWalt 611 router on the X-Carve. Please be very specific and tell me what I should do as far as router speed, etc. The DeWalt 611 has a speed dial. Do I have it all the way up?..slow it down? The dial goes from 1 to 6. 6 being full speed. .003 depth per pass and 5 inches per minute. Is this going to work? Please be very specific if you recommend any changes to the settings I mentioned.
Thanks in advance :wink:

P.S.- I’ll be doing all of this in Easel.

I work in MM for all my milling so I converted everything over. Looks like you are working in 5mm think stock and want to do passes of .0762mm? What is your total depth you need to mill out? Have large is the piece? What are you using to do you CAM with? Are you going to mill a special waste board for this project to insure it is 100% flat? What size X Carve? I mill aluminum 95% of the time on my Shapeoko and X Carve. If you can answer some of these questions I can try to give you some advice along with others here to help you out.

Right off the bat your DOC is VERY shallow for a 5mm deep stock. But it depends on what your TOTAL DOC will be on the piece I guess. You need to make sure the stock is in a milled pocket on your waste board to insure it is flat and level in respect to the spindle. You feed rate is in the good zone overall for up to a .5mm DOC on that endmill though i would keep your DOC around 2.5 at most to play it safe OR slow down your feed rate a bit. Making sure your Z offset is 100% spot on will also be very important. A 1/16" (1.56mm) endmill does not like to slammed into a milling surface.

Also what alloy are you milling? 6061 T6 will tend to heat up and smear if milled wrong. Keeping the chips clear is a must with a high RMP spindle and 6061. The chips will melt onto your endmill and ruin your job in a matter of seconds if you allow them to build up too much. Also a 1/16" endmill not mill well if the chips are not cleared if you are doing a contour cut or slot that is only 1/16" wide. The chips will pile up inside the cut and break your endmill, so keep the stock as chip free as you can once your DOC is deeper than say 2mm.

Most of my current milling is in 5000 series toolplate aluminum which mills far better and easier than 6065 with a high speed spindle. On the 6065 you will want to keep the chips cleared and the stock COOL with either some sort of oil or water coolant. A small spray bottom will do the trip if you are careful. But above all chip clearance is going to be very important.

1 Like

Ok, I’ll admit, most of what you posted confused the heck out of me lol. I’ll do my best to respond.
1-The material is .50 mm thick. I want to go all the way through it into my waste material underneath.
2- Depth of cut 2 1/2 …noted.
3- What do you mean “making sure your Z offset is 100% spot on”? Where do I set that? Using Easel so babysit me there.
4- I don’t know the alloy. I got it from Lowe’s. http://www.lowes.com/pd_42279-37672-11488___?productId=3057473&pl=1&Ntt=3-ft+x+24-in+aluminum+sheet+metal
5- piece is 31 x 24.
7- keep chips clear…noted.
8- Using Easel, please be specific and tell me what to put in each box. My apologies, I get confused and overwhelmed easily so I need things spelled out to me as simply as possible :confused:
9- For coolant, will WD-40 work?

Well I ran some numbers through Gwizard. It looks like you are carving the Mona Lisa in Alu. I hope you are using a 1/16" ball end mill for the relief carving.
Material 6061 T6
With a DOC of .003" WOC .015 27000 RPM Your feed rate is 29 IPM and plunge rate is 9.4 IPM
Your deflection is .00003 and in the safe zone. These little end mills don’t like deflection.

At 5 IPM you will be rubbing and not cutting.Your chip load is way to low. The recommended surface speed (SFM) is 600 at 27K RPM you will only get 189 SFM

You want to keep your tool stick out at .75" or less. Use WD40 applied with an acid brush in front of the cut to keep the tool well lubed so it does not weld Alu to the tool and break it.

Good luck getting Easel to run this.


Man, you guys sure know your stuff lol. All these abbreviations and numbers scare the crap outta me! Hmmm, I have another idea…if I use a sheet of aluminum and spray paint it black…what depth do I need to cut to ONLY scrape
off the spray paint to expose the aluminum? The only 1/6 bit I have is the 2 flute fish tail. If this isn’t doable for the first idea…how about the spray paint idea? Again, please use very simple wording :confused:

So much for surprises lol. Here’s the design…far more detailed than the Mona Lisa. Call me stupid…or ambitious.

I have a DW660 (the crappy dewalt, I really need to get rid of this thing) and I get good results at .015" DOC and 30-35IPM on a 1/8" 2FL (or even 3FL) flat TiAlN coated. If I’m doing a rough pass and a finish pass, I’ll do the rough at 30IPM and the finish at 60IPM (assuming .015"DOC and <40% WOC). Typically with a 1/16" bit I will use the same settings except DOC is set to .0015" (10% of the 1/8" bit). These are fairly conservative numbers, you could get away with going 50% faster, but you will not like the edges it leaves.

Depending on how precise you want to be, the Z zero is super important. I’ve found that with the smaller more fragile bits, you bring your bit down close to the top of the stock, release the collet so the bit slides down on top of the material, then VERY SLOWLY lower the spindle until the bit is in as far as you like. Then tighten everything down and zero out the Z. There was a video floating around somewhere on the forum where someone did this for PCB milling. I’ve only tried it once but it worked great for my 1/16" ball.

Cool design by the way.

Edit: Just saw your confusion over the terminology, haha.

WOC = Width of Cut
DOC = Depth of Cut
2FL = 2 Flutes

As for the spray paint idea, I’m not sure how thick the layer of paint is. You could test this by getting a piece of material, measuring, then applying the paint as you would and re-measuring. The difference is out thick the paint is. I’d imagine its probably as thick as a piece of paper, something like .1mm?

OK I will help out as best I can.
If you are cutting all the way through your stock then you need to make sure once you cut it that it will not come flying off the mill at your or a pet, kids… all the fun soft stuff that bleeds. Most of my item have screw holes for which i use to hold down the stock. short of that you have two choices and I would use both. You can use a thin double sided tape like this style http://www.amazon.com/Scotch®-Double-Sided-665-Inches/dp/B00006IF5M/ref=pd_bia_nav_t_2?ie=UTF8&refRID=1R1M7EKM093N1MA5YCTV (not foam style). you can place strips of it along your work every few inches and then I would also use tabs in your design to keep it attached to your stock until you are ready to remove it. With .50 mm stock I would go with tabs about .125mm or so. not much thickness but beats nothing.

On the DOC: if my math was off and you are at .50mm or 1/2MM then i would do a DOC of about .125-250 depening on how your work is going to be held once it is cut free of your stock. doing a full depth cut (more then .50mm) will put a good deal of stress on what ever you use to hold your cutout with. Going with a shallower cut on the final pass will reduce the stress on the stock from shearing lose and ruining your project.

I admit I have never milled a single project with Easel. I started cnc milling aluminum on a Shapeoko before Easel an option so i have never used it. Most of the items I mill are of complex shape and depths so I have to use other programs for my stuff. I will have to differ to others for Easel settings I am afraid. But there is a huge wealth of guys here who have used it nonstop and they should chime in here shortly I am guessing.

Alloy wise I would assume 6061 and treat it as such which just means keeping it cool and clear of chips. So on the subject of chips. You will want to get a cheap paint brush so you can brush the chips aside as you mill. Once you apply wd40 (which works OK for this) the chips get damp and tend to want to clump together in and around the mill path. Just use the brush to brush them aside and either leave them or vacuum them up (might need the brush to “help” them). but often once wet the chips will not vacuum up well. such a shallow DOC will produce very small chips that often do not fly far enough away from the cutter when wet.

I would also suggest milling it in wood first to make sure you are happy with everything settings wise and such. Wood is FAR cheaper to test with than your aluminum stock.

The Z offset is making sure your endmill is JUST on the surface of the stock, not above it or below it. Getting a set of feeler gauges from an autoparts store will allow you to use the thinnest one. You place it under the endmill and slowly MANUALLY turn the Z Axis down while sliding the gauge back and forth under the tip of the endmill until it JUST grabs the gauge. then you would zero out your Z axis. That will work on the wood or aluminum. For the aluminum you can also rig up the pin 5 probing of the Arduino shield and then attach a lead to your stock and another lead to your endmill and the spindle will auto set your Z offset. You can search the forum for info setting this up as I have seen a number of posts about it.

I am very sorry I can not offer much help in Easel. I am sure others can and will shortly. I would advise test milling in wood if you can first and ask as many questions as you wish here so we can all help make sure you have the best chance at success the first time out.

@Travelphotog I think we are confusing the crap out of him switching between inch and mm :laughing:

1 Like

sorry guys! I never work in inches these days… I also admit I have not a single clue about working with Easel so that part is something I can be of little help with.

Some terms you will learn with CNC
DOC= depth of cut
WOC= width of cut
IPM= inch per minute
SFM= surface feet per minute

When Travel said “Making sure your Z ofset is 100%” he is saying that Z 0 has to be perfect if not and the machine runs you tool into the material at rapid rate there is a good chance that it will break.

I’m typing this and others are chiming in while I type.

Complete change of what you are doing. You are trying to do an engraving. Go online and get some engraving tools in 60 degree with a .005" tip. Then do zero off set so the tip of the tool follows the lines.
I dought that Easel will handle this.


1 Like

I would listen to Dave above ME! He does amazing work and I am guessing has a background in CNC or machining. I am a professional sports photographer by trade. This is just my side hobby.

All of you guys are awesome. I really appreciate all of the attempts to break through my wall of confusion lol. I may go with the spray painted idea and/or wood…but never say never…like I said I’m either an idiot or overly ambitious lol. Thanks a bunch guys.

So I just looked at your project (one of the perks of working at Inventables), your settings look fine more or less, .003" depth is fine, but 5 inch/min is way too slow. I’d bump that up to 20 at least, but id recommend staying under 30. If you have a 1/16" ball I’d use that for the engraving. If you plan on doing an outline you’d have to switch to a flat end mill. Since you have early access to the roughing/detail feature you can achieve this pretty easily. You’ll have to set the rough bit to .0625 and the detail bit to .0625 as well. With the way roughing/detail works, outlines are done on the detail pass (this is because we assume outlines need to be done last).

Definitely get some double sided tape, I recommend carpeting tape because it is very thin and incredibly grippy. I’ve had problems where a long, thin sheet of metal would bow upwards in the middle and wreck all kinds of havoc.

Your design is extremely complex with very fine detail and it will probably take a few hours to cut. Since your material is so thin, you could in theory do 6 passes at .003 before you would cut through the other side. Assuming everything is perfectly flat 1 pass would be enough, but thats rarely the case. I’d set your engraving depth to be 2 passes deep (the way you have it setup now, thats .006"). Honestly, with such a thin depth chip clearing wont be as big of an issue as it would otherwise be, but you will definitely want to get some WD40 and keep everything nice and slippery.

Also I hit generate tool paths like 5 minutes ago and its still going. So this will probably be a 4 or 5 hour job.

Good luck!

Both. Thanks Travel we need some of your sport action shots on your build thread.

Stick with it. There is a step learning curve to this whole CNC/machining stuff. One of the programs I will not do CAM work without it open in my left screen is Gwizard. I plug every cut I make in CAM into it for feeds and speeds.
Bob Warfield the developer of the program will let you try the program for 30 days before you buy. He updates the program at regular intervals and adds more to the program.


Thanks Eric. Coming from an Inventables employee your compliments are that much more flattering. I really appreciate the advice.

I think Gwizard is next on my list of items to buy for my milling. Moving up from the 400W dc spindle to the .8kw VFD on the X Carve is meaning I need to start playing by the rules now that my spindle can take it better. There is always something to learn in this great hobby. As for pics… At the request of the Inventables guys, I will be doing a fair number of projects here shortly that will be picture heavy (Stone engraving is being done today). Now nice thing about being a photographer and selling your milled work is the promo side of stuff is a breeze. It is the milling side I am working on now!

1 Like

David, You bring up something I was curious about. Is it possible to use a Vbit on Aluminum? I assume that it would require a coated vbit compared to the bits I am using in wood. I would also be concerned about how Vcarve just plunges the vbit into the material without respecting the depth per pass setting.

I have used V bit style end mills in aluminum with great success. I often sell them as signs. I mill the aluminum panel to desired size and shape, then anodize it the color of choice. Then it is etched out with a 30 degree .2m end mill much like most folks use for PCB trace milling. I use HSMxpress or Aspire for CAM on the signs and they do fine. But both do allow me to set the pass depth. But as far as the bits go they work great.

They also work pretty good in soft stones, though it is a one time deal when you finish.