Attempting to cut aluminum - breaking bits

Good Morning,

Can anyone give me some advice on cutting aluminum? I redesigned the bottle opener project out there but I am using the same 1/8" thick, 6061 aluminum and the exact bit that was recommend. Even with liberal amounts of cutting fluid, the bit broke within two seconds. I believe its trying to plunge in too deep before starting the cut process, as the Y axis started to struggle and skip after maybe an inch or two. The noise was also pretty much unbearable without hearing protection. ( I expected some noise, but not like this)

Are there some manual settings that someone could recommend that would make this easier? Any Milling bit recommendations would also help a great deal, as I am new to all of this.

I’ve got the larger stepper motors and the 300watt / 24 V DC spindle.

Thanks,

I personally havent cut much aluminum and my few attempts were utter failures, but I do know that in order for anyone to really help you out, it would be good for your to share your feed rates and bit size/type.

I have done a good deal of aluminum milling on both the Shapeoko with a 400w 48V spindle and on the X Carve with a .8kw VFD water cooled spindle. I mill complex parts for 3d printers and other things in 1/8 to 1/4" 6061 and aluminum tool plate.


What is the DOC you tried and the feedrate you used? With the stock spindle and a stock X carve, you have to mill a bit slower then the feed and speed charts say to. Getting good results off the X carve is not hard to do in aluminum but does take attention to how it is done and some mods needed on the X carve help greatly.

If you can give me more info i can try to help you out a bit. What are you using for CAM? Are you on the stock X Carve with the stock controller card? Have you tried using Chilipeppr yet?

OK looking forward to your answers.

1 Like

@Travelphotog
I’ve seen a few pictures of some of the work that you are doing… I think that for me, maybe a bit of a primer of some of the steps you have taken to ready your Machine for the detailed work you are doing would be helpful.
Q: have you done any stiffing mods to the gantry, if so; what method?
A:

Q: what method do you use for cam ( fusion360, cambam, other) and for output to the machine… ie your workflow?
A:

Q: what bits and sources for them are you using (bitman1, toolstoday)? what are your feeds and speeds for those bits?
A:

Q: are you using a feeds and speeds/DOC calculator ( which one) and what adjustments (usual ) do you have to do when using (it). ie… as it is known you usually have to pair the speeds and DOC down a bit because most of the calculators expect that you are using a mill or HAAS…
A:

Wow, I’d say you have some experience. I was using the Easel software, and I was under the impression that it calculated all the feed rates for you. Obviously it’s not playing nice.

I was following this project and using the bit that was recommended.


$12.42 30423-03 1 1/8 in 1/32 in - Fish Tail, 2 Flute, Spiral bit 1/32"

I don’t have my x-carve around, but the feed rate and depth is whatever X-carve plugs in as defaults for Aluminum. I’m open to any suggestions for a good strong bit, and manual RPM and feed rates.

@JohnSheak I will try to answer your questions as best I can and forgive me if I am a bit long winded in some answers…

So first my setup: These images are from my Shapeoko and it was working with the following at the time: 500x500 Shapeoko 2 with 48v 400W DC Spindle. Acme Z Axis, NEMA 17, Full metal slotted bed, TinyG going through Chilipeppr. No real mods other than limit switches and large 3D printed spindle mount VS the stock mount. Currently the Shapoko has two changes, I now run a PLanet CNC MK3/4 controller with Leadshine DSP drivers and I switched the X Carve spindle mount over to the Shapeoko and it has been a good improvement.

My X Carve is a 500 x 500 with the same full metal slotted bed, Acme Z Axis, upgraded NEMA 23 180oz motors, Planet CNC MK 3 controller with Leadshine DM442 DSP drivers, .8KW 1hp VFD water cooled spindle and lastly a chip clearance system to blow the chips out of the toolpath.

Q: have you done any stiffing mods to the gantry, if so; what method?
A: I have not yet but plan to test a system shortly which will replace the main gantry for a stiffer one.

Q: what method do you use for cam ( fusion360, cambam, other) and for output to the machine… ie your workflow?
A:I use HSMxpress currently. Might switch to FUSION360 shortly. The images above were from the TinyG and Chilipeppr. My current system has a proprietary gcode sender/interface for the Planet CNC controllers. It is basically a cross between Chilipeppr and MACH3 overall. I find it far better than either one for my needs.
So I design my parts in CAD, use HSMxpress for CAM then send the Gcode to the controller with the CNC USB controller software interface from Planet CNC

Q: what bits and sources for them are you using (bitman1, toolstoday)? what are your feeds and speeds for those bits?
A: I mainly use Destiny 3 flute bits from Drillman1 ( http://www.ebay.com/itm/381351391953?_trksid=p2057872.m2749.l2649&ssPageName=STRK%3AMEBIDX%3AIT) I also use a 4 flute 1/8" 45 degree chamfer on all the edges. I use a 1/16" 2 flute flat end mill from Drillbits unlimited ( http://drillbitsunlimited.com/ ) I also use a 2.5mm 1/8" shank drill bit for the M3 tap holes. 95% of my bits come from Drillman1 or Drillbitsunlimited.

Q: are you using a feeds and speeds/DOC calculator ( which one) and what adjustments (usual ) do you have to do when using (it). ie… as it is known you usually have to pair the speeds and DOC down a bit because most of the calculators expect that you are using a mill or HAAS…
A: 2 part answer. Part one for the OKO with the DC spindle: There is not near enough power to remotely use a calculator with a DC spindle on the OKO or the X Carve. Milling aluminum on the stock DC or an upgraded DC spindle on the X Carve or the OKO is NOT a fast process and is closer to “scratching” than true milling of aluminum. BUT it does work if you allow it enough time. The OKO and DC spindle with the 3mm Destiny 3 flute end mill did a DOC of .12mm and feedrate of about 135mm/M for the shots you see above. The 1/16th 2 flute endmill ran about .1mm DOC and around 75mm/M. Chamfer was ran around 75mm/M. These shallow DOC and slow feeds are due to the lack of power in the DC spindles and the overall weaknesses of the older Shapeoko design in relation to flex on gantry and the spindle mount. It was subject to a great deal of flex if pushed too hard and would break end mills.

Part 2 the X Carve and the .8KW VFD spindle: Yes and no for the calculator. I am using the Gwizard calculator and it is a great tool by all means, but still manages to break end mills. This is due mainly to far more aggressive DOCs though and failure to clear chips fast enough. Dry milling aluminum is NOT a good idea and it WILL bite you every chance it can. But it can be done as all my aluminum milling on the Shapeoko and X Carve are done dry. I have installed a custom chip clearance system on my X Carve to fix this issue and so far it has allowed me to come within about 85% of the Gwizard DOC and feed rates. For those wondering, I have told Gwizard that I have a .6KW spindle with a 24000 upper and 1500 rpm lower limit. I am still working to dial in the settings in relation to an X Carve as like you said, it is more suited to a HAAS style mill than a X Carve.

Above all there are three important steps for milling aluminum. One is a fully calibrated SPU mill in all axis. This means using a dial indicator to check your SPU (steps per unit) on each axis down to .001". The stock settings for the X and Y Axis rarely are truly correct due to belt tension. For milling aluminum with fine end mills this is a hugely important step. If you are able to allow for backlash also like in the Planet CNC controller, all the better. Both my X Carve and Shapeoko have about .0550mm on the X and Y axis of backlash. Which on a fine trace PCB can ruin a board.

The second one is ALWAYS to mill a sacrificial waste board for each project to make sure you stock is 100% flat and level in respect to the mill. Otherwise a .12mm DOC could jump to a .25mm DOC due to an uneven waste board or mill and this will snap your small end mills. A small piece of plain pine board works great and is cheap. They can be refaced for more than one job to reduce costs.

Third and equally important is to ALWAYS use a touch plate or probe your Z height/Zero. Being off even .1mm will change your DOC to something the DC spindle or the small end mill can not handle at a given feed rate and snap your end mill.

3 Likes

The 2 flute bits they use should work well. Though I prefer to use a 3 flute Destiny tool Viper bit myself. But they are of course a bit pricey at about $12 each for the 1/8" size. I noticed that the instructions for that project are no longer posted (which is odd). The stock DOC I think is about 135mm/M with a .1MM DOC as I recall. That should do just fine if you are 100% sure you are just at the surface of the stock and that your stock is level. If you check the post above to John, I mentioned about milling a sacrificial waste board when milling aluminum and about making sure your Z zero is a true ZERO and not down by .1mm or more. When taking such shallow cuts in the aluminum with a stock X Carve spindle, being off even the tiniest amount in your Z zero will result in taking too deep of a DOC and break bits.

If your mill a pocket in a sacrificial waste board and make sure your end mill is at a true Z zero when you start, the stock feeds and DOC of 135mm/M and .1mm DOC should work for you, it just takes a bit to finish up.

3 Likes

@Travelphotog Great info. Have you tried 3 flute ZrN coated endmills? I just ordered a few, to use on my brand new .8kw watercooled spindle.

I’ve been trying to figure out new speeds and feeds for when I finally get my spindle up and running. Chipload is the #1 factor this time around, targeting .003"/tooth. G-wizard likes to use the max RPM for milling aluminum (24k rpm), which means my feed rates need to be something like 120ipm (3000mm/min). Obviously depth of cut needs to be adjusted to whatever the machine can take at those speeds. Have you tried this approach? Before I would “eyeball” everything and use g-wizard mainly to calculate deflection (the metric i used to estimate machine strength, in my case keeping it under .0004 always gave good results). Using the new chipload-based settings and reducing the depth of cut will decrease my cut time significantly, I’m worried the xcarve can’t manage .01" DOC at 100 IPM (24k rpm) even if the spindle can.

1 Like

@EricDobroveanu I have been very impressed at the DOC and feed rates the X Carve can use. The limiting factor has been lack of cooling. The numbers Gwizard puts out work fine, but tend to heat things up to the point that even with a good vacuum shoe or forced air chip clearance system in place, the end mills still end up breaking about 5-6 large cuts into a plate of aluminum. Only by reducing the feed rate have I been able to stop breaking end mills on the .8kw spindle. I am playing now with DOc and feed rates but since the failure results in a borken end mill, I have stop experimenting so much and gone back more towards “safe” feed and speeds which are allowing me to keep production up once again instead of breaking end mills and having to restart tool paths. I have found a RPM of 18480 and DOC of .5mm with a feed rate of around 150-200MM/M is working OK for production. It does “rub” far more than it should, but the finish is usable for my needs and it does not break end mills. I can mill 1/4" stock with that setting for 24 mounts which runs about a 4-6 hour milling session without breaking an end mill and producing 24 mounts for my project. I plan to get some cheaper end mills and play around more with Gwizard once I have production caught up from milling delays due to broken end mills and taking time to make the PCB project write up. Have you done a full calibration on each axis for SPU? Have do you do your Z Zero and are you using chilipeppr?

1 Like

@Travelphotog Interesting. I never broke endmills on my DW660 (the crappy dewalt) unless I did something really dumb with the gcode and even then I’d get more chip welding than broken bits. TiAlN coated endmills are insanely strong. I have an air hose hooked up to blow the chips away (look on littlemachineshop.com) and will usually baby sit the machine and spray some WD40 every 3-5minutes. Because I use only TiAlN coated endmills heat isn’t such a big issue in terms of tool wear but I haven’t noticed a big difference in finish quality cutting 100% dry.

I haven’t done a full SPU calibration, I’m actually trying to get my hands on a dial indicator before I finish setting up the spindle.

To zero, I’ve been lowering the bit very close to the material, undoing the chuck and letting the bit drop to the material. Then slowly lowering the spindle until it is just about inside the collet then tighten it all down. I seem to get a fairly accurate Z0, but I was actually going to make a probe first thing when my machine is put back together.

I use UGS mainly, chilipeppr’s json server doesn’t always cooperate. I’d like to use chilipeppr though, cause I actually hooked up a webcam to my spindle. I haven’t gotten it to pipe through to chilipepper successfully yet, though.

@EricDobroveanu I rarely if ever broke end mills on the Shapeoko. The gcode is the very same, just with updated feeds and speeds. Gwizard wants me to run a .5mm DOC at around 18480-24000 rpm with 15mm stickout at around 500-900+ MM/M feerate. At that fee drate even the smallest snag in the end mill will snap them off. Unless I can change a few things and set up either Fog Buster or a full flood system, I am not able to run the settings Gwizard wants. Most of the time I am cutting a production run which is 20+ objects on a large piece of aluminum tool plate. So the marger tool paths can run 5+ hours to process all 20+ object on the plate. While the run time was longer on the Shapeoko and the Dc spindle, I was able to leave the mill to run for 8+ hour at a time with no oversight on the TinyG and Chilipeppr (before it Chilipeppr became to unstable as you mentioned). It just looks like the Gwizard is aksing for very aggressive DOC and feed rates which just are not working well without a cooling or lubing system. With run times of 5+ hours I am not able to stand by and spray it manually.

This is a typical plate with 20+ mounts and a number of smaller objects thrown in to use the plate to the fullest. The main cutout of the mounts is about 4 or so hours alone so it is not a process where I can add cutting lube manually throughout the mill run

I am looking at a automatic drip system I can control from my Planet CNC controller with Gcode to add a drop or two of a lube from a tube next to the end mill. I just have not taken the time to mess with it yet. The Destiny end mills are coated with their “Stealth” coat which is meant for aluminum milling is and the best coating I have found so far for the purpose Vs uncoated or TiAlN coated. The forced air chip clearance system I installed has worked really well and allowed me to get to about 85% of what Gwizard wants to run the mill at.


So with a misting or lube system installed soon I think I will be running at close to 100% of the desired values shortly.

2 Likes

@Travelphotog Ah, ok. What alloy aluminum are you cutting? I should mention that I cut almost exclusively 6061-T6, one of the easier to machine alloys. Have you tried facing aluminum? I’ve found the need to face a part here and there when I want it to be perfectly flat, but a 1/8" bit just doesn’t cut it in terms of quality. I bought a 7/8" (1/4" shank) carbide bit for wood, not sure how well that will work on aluminum though.

For this project I only mill in Alca 5 tool plate ( http://www.alutrade.se/alca-5-2/?lang=en ). It is face milled from the factory to within +/- .005” which is one of the main reasons I use it. 6061 t6 plate has a far looser spec for flatness and is very hit and miss for how flat a given piece of stock will be. The 5083 alloy in Alca 5 is also great for anodizing after milling due to a far smaller pore size in the cast plate over the typical 7000 series cast plate like Mic 6 which is very hit and miss for anodizing and often needs a nitric acid dip to remove the sulfuric acid molecules from the larger pore structure so they do not contaminate the anodize dye and cause it to either fade over time or produce black spots with the anodize layer. 6061 T6 is very easy to anodize and works very well for may projects. But since this is the mount for a 3D printing head, I needed it as flat as I could get it from the start so I went with the 5083 tool plate. It mills great and is very easy to surface prep for anodizing after milling.

I have done face milling on the 6061 I have used before. Doing it on the X Carve style mills is not hard, but the mill must be perfectly square and the tram must also be perfect or there will be a small step in your passes. The X Carve and the Shapeoko are very difficult to get a perfectly level tram on. I spoke to Bart about that when I visited the Inventables offices in hope the X Carve was improved over the Shapeoko in that area but he confirmed it is still the same setup in that regard for calibration. It takes a great deal of work to get it level with the weight of the .8KW spindle but it is doable with effort. I have done it with a 1/4 flat end mill and also with some success with a fly cutter. I also have a large flat bottom cutting 1/2" end mill i sue to face my sacrificial waste boards. Once I order another in I will give the old one a try on Aluminum and see how it does as a face mill.

I am running the 1000mm x-carve defult board but put on the DW611. still waiting a collet nut and collet upgrade from www.precisebits.com. still deciding on how I am going to setup my work bed… have started a full size vacuum plate ( buddy is doing that on his HAAS at work.
I don’t plan on doing aluminum myself ( well maybe :slight_smile: ) but I have seen a lot of these threads here and at a few other sites and folks seem to hold onto those settings like they are car setups in Iracing. Figured I would get the question and answer session going… But that was a great bit of info. thanks.

@Travelphotog So I got the 800w WC spindle up and running. Holy crap what an improvement over the DW660. As a fellow anodizer I took the liberty of customizing the dewalt spindle mount that I used (this was just after a test cut so there is a lot of sticky, greasy aluminum chips stuck to it).

But yeah, overall the quality of the parts compared to the previous spindle are an order of magnitude better. Before I would have to spend probably 3-5minutes filing everything down to make it smooth (for the sake of mechanical operation of the part), but those 2 test triggers I made just needed a bit of de-burring and they were golden. Really happy so far, need to do more testing tomorrow. And I need to custom anodize more parts of the machine :smiley:

1 Like

@EricDobroveanu Man I total forgot you anodize also! Too many folks to keep up with on here and that slipped my mind. Are you milling from 1/4" plate? You should REALLY give the 5083 tool plate a try if you are. It anodizes and mills like a dream. You might neverr touch 6061 again!

The VFD spindles are really nice and I wish more guys would give them a try over the Dewalts. Just on noise alone they are worth it. Glad to see you got yours up and running. Did you go with a closed loop cooling system or just a large bucket?

@Travelphotog Us anodizers are a rare breed, we gotta stick together, haha! The largest plate I cut is .19", but typically I cut .16" or .125". I have cut .5" before though in an attempt to make a spindle mount, but that didn’t turn out so good. Looking around online for prices, I can’t seem to find 5083 alloy. Whats the price difference like? I don’t really need something super strong for my parts, though (not sure how much tougher 5083 is to 6061). I’ve found that anodizing 6061 is a dream when its fresh/new though, but I do nitric dip everything anyways, though. Usually make about .65mil of anodize, I find going higher than .75 or so will make 6061 “bronze”, not a problem if its going to be black, but if you want white, its a huge problem.

For the cooling, I ended up using a 5gallon bucket with a few holes drilled in the lid. I have a bunch of PC watercooling parts lying around (radiator, old pump, reservoir, barbs, etc) but since the spindle doesn’t use G1/4 threads its tough to connect everything. I could use some adapters but I’m not sure how my (5 years old, at this point) pump would fare. I looked into some modular AIO units but the ones I would get are $150+, too much. The bucket setup cost me ~$40 for everything (except the silver quarters i threw in there to prevent algae) which was acceptable. The only problem is that the pond pump I bought is really really weak. I had the pump under the table the x-carve is on but it couldn’t push the water all the way through the spindle and make the return trip. I ended up having to raise the bucket almost to the same height as the xcarve to get it to fully cycle properly. I guess thats what I get for buying from home depot, haha.

@EricDobroveanu & @Travelphotog
I noticed you both have aluminum extrusion custom base boards. Would either of you care to share where you found them? I looked on 8020.net and the only thing they had close would have taken 13 strips to get to the 1000 mm sized board.

I ask because I just got my X-Carve assembled and was very disappointed that the waste board is not true to the gantry. I have a high point at X0 Y0 but as I move away from there there is at least a .05" difference over 10" in both directions. That’s a considerable amount by any CNC standard. I have read in several places in the forums where others have the same exact high point, and the only solution is to pocket out sacrificial boards. That would be rather expensive over the long haul, in time and material, since I bought this to produce items for sale in the minimal time I have after my regular job. So I am looking for something that will not warp and that I can trust to be true every time I go to use the machine.

Any other affordable upgrade suggestions would be welcome also, i.e. where to find a better spindle, controller, etc. I am very familiar with CNC machines from college and work, but I am rather new to home based DIY CNC machining. I thought I had read enough to understand most of it, but I now see that I didn’t know the right questions to look up. This is a great learning experience.

Anyway, I look forward to your answers!

This is where I found out about them:

Hmm cheaper than the 8020 option for sure. Thanks for the info!