Have you tried a #274Z using the settings in Carbide Create?
The bit might be covered under the 30 days mistakes are on us thing if you got the machine within 30 days.
That said, as I suggested in other thread, take a look at the video. your feedrate could go faster with the higher rpm. If you want quick/easy math, just double everything. Adaptive in the video was
10k rpm
30 IPM
Opt Load .012"
Stepdown .03"
New settings would be maybe be:
20k rpm
60 IPM
Opt Load .012"
Stepdown .035"
I always forget that I have the coated bits, so I rarely end up using them.
3 Likes
Those are actually the settings I used since I never used a single flute before, and it snapped, so I am hesitant to buy another $35 mill and have it break again! Unfortunately I did not know I had to order them with the machine to get the guarantee!
Please send the file which snapped the tool in to support@carbide3d.com and we’ll do our best to look into this with you.
Oh, I pulled those from the video on the coated cutter. Let me find singleflute settings.
Nomad 883 pro:
RPM: 10000
Feedrate: 12 in/min
Stepover: 10%
Cut depth: .01 in
Plunge rate: 4 in/min
Nomad 3:
RPM: 20000
Feedrate: 24 in/min
Stepover: 10%
Cut depth: .01 in
Plunge rate: 4 in/min
You could probably add a bit to cut depth, but that’d be where I would’ve started. That bit is fragile though, so I would’ve set z height above my material and let it cut some air a bit.
1 Like
I also broke a 274-Z. It was the only one out of the 9 endmills I tested that broke under harsher cutting conditions.
Given the price of the Carbide 3D endmills, I’d recommend looking elsewhere. For the price of their ZrN endmills, you can easily buy a handful of decent DLC endmills somewhere else and I’ve found DLC to be fantastic with Aluminium. Nothing sticks to it!
If you want to go fast, you should also look into 6mm multi-flute endmills and an air blast. More teeth + same feed per tooth = more feed. You only want to use larger multi flute endmills though, otherwise chip evacuation is really hard unless you have flood coolant.
The rule I found worked well on the 883 Pro is:
- High RPM (I’d go 24k RPM on the Nomad 3)
- Conservative feed per tooth (e.g. 30um, or 720mm/min at 24k RPM)
- Around 60-75% radial engagement
- Start with around 0.1 x endmill diameter of axial engagement
Start with these settings then do test cuts. For each cut, increase axial engagement. Don’t touch anything else, especially don’t touch feed per tooth. Eventually you’ll reach a point where the machine sounds like a dying cat or the spindle starts to visibly slow down. When you reach that point stop and back off a bit axially until it sounds nice again.
You’d probably like someone to just tell you “cut like this” but it’s really hard to be able to do that. Different alloys, endmills, geometry etc. can complicate it. The most reliable way is test cuts.
Amana is mainly for wood from what I saw.
1 Like
I have used the Amana and Carbide 3D single flutes a bunch in aluminum. I have a SO3 but the same rules should apply to your machine. I broke a few in the beginning while learning but have not broken one in a very long time. The rules I follow generally are:
- Make sure you are cutting a machinable grade of aluminum. 6061 or equivalent is the best.
- Keep your feed per tooth at least 0.001".
- Make sure the chips are clearing the cut.
- Start with 10% of the tool diameter as a depth of cut and 50% width of cut to start. Increase from there.
24000 RPM and 30 IPM is 0.00125" feed per tooth on a single flute. This should work great. A 1/8" tool should cut comfortably at 0.01" stepdown (as long as you can ramp down, if you are plunging I would reduce this by 25% or more) and a 0.06" stepover.
Amana makes many single flutes for aluminum:
4 Likes
What brand/website do you recommend to get the dlc end mills?
If your bits are clogged with melted on alum you can try cleaning them with lye. Just take safety precautions with caustic solutions.
1 Like
Ah, the ones on the Carbide 3D shop are for aluminium though right?
Endmill suppliers are highly regional and I’m in Europe, so I think my suppliers might not work for you.
1 Like
Your speeds sound okay to me. I run my Nomad 883 at 10,000RPM and a speed of 400-800mm with a DOC of 0.1mm to 0.2mm on aluminium and brass.
I don’t use the fancy bits since they are way too expensive. I either use this type of uncoated, or this type of DLC coated (similar to the ones @Moded1952 mentions).
They last a surprisingly long time. I use the same bits on my S03XL but lift the DOC to 2-3mm and ramp up the travel speed and spindle speed to hit around 0.025mm per tooth.
However, on the Nomad I don’t “go large” like Lucas, since my stock machine would probably choke up. I do find that short flute lengths help reduce chatter enormously, and that the tiny 2mm endmill can easily cut slots in aluminium and brass without any choking or clogging (I do have air blasting for chip evacuation though)
1 Like
On the stock machine they still worked quite well, you just can’t scale the whole MRR up dramatically like you can with larger machines.
The increased surface speed and feed rate is really worth it though, even stock.
1 Like
That’s good to know. I have some comfortable parameters for the Nomad that don’t stress it too much and keep it moderately quiet, so I’m happy for it to do jewellery-level work.
For big clearing, the SO3 XL with a 2.2Kw spindle on it can hog out material quickly enough for me. Benefit of two different machines, I guess.
I would still be curious of the actual toolpaths you are running. Those milling parameters sound fairly good, maybe a little high on the chipload (~0.003 in/rev/tooth). Your toolpaths are equally important in how they are set up. You can be as ideal as you want and then plunge directly into the stock to end up with a broken endmill.
If you can share more about your setup, we can help troubleshoot it more without you spending money on more endmills that you probably don’t need. The C3D Zrn single flutes work great and if you can’t get them to work at all for you, I doubt you will really find anything else that will.
2 Likes
From what I can see, all the Amana kits that Carbide 3D sells are for wood and plastic. It wouldn’t make much business sense to sell Amana’s aluminum tooling when they are selling their own. I don’t know who is the OEM for Carbide 3D’s tooling but I can tell you from buying both and comparing them that the 278Z and 274Z appear to have identical geometry to Amana’s equivalent.
As I stated before, the single flute broke ass soon as I tired to use it, so I never got a chance to really try. Its hard to spend another $35 after that happened, for no reason I can figure out at least. It was a simple
I have had great success with the TiCN bits from Kyocera, which is why I was wondering why I was having so much bad luck with the Zrn bits. The Kyocera bits are also considerably cheaper, which also had me scratching my head.
Most of my tool paths are contours, but I program them so they are only engaging about 50% (I am working on discs with holes in center which allows me to do this type of path)
I am mainly trying to figure out what I am doing wrong, since everyone seems to rave about the carbide end mills!
1 Like
The one I was using was purchased on Amazon, and is for aluminum cutting, with a Zrn coating. It still built up aluminum on it after about 2 hours or less.
I have used some of my Amana tools for 50+ hours. I would guess that you might have been recutting chips. This can quickly cause a buildup of aluminum on the tool edge. This can also happen if your chipload isn’t high enough.
1 Like
It can be somewhat tricky to figure out what’s happening, I brutally murdered a few bits on Aluminium to start with by not understanding things like, toolpaths running round a small circle like a bore or helical ramp, have a way higher effective speed.
I have had great results with single flute uncoated and DLC coated cutters bought locally here, they’re not expensive.
I have found that if the workpiece starts to heat up then the Aluminium goes very gummy and welds to almost any cutter, a few drops of Isopropanol as lubricant can help with that, or just reducing engagement (or surface speed on larger cutters)
And, as Nick says, recutting chips heats them up and melts them, I use dust extraction all the time on Aluminium.
Right, but this goes back to what I asked about. What was the toolpath you were trying to run when you broke the endmill? Did you plunge, ramp, helical into the stock? You say 50% engagement, is that axial or radial? Contours can be difficult since it doesn’t allow for as good of chip evacuation so are you running roughing passes first or contouring directly in with sidewalls on both sides? How are you holding down your parts? If it isn’t solid, it can shift and break endmills that way (done that one myself).
If you are able to share your CAD/CAM, we can break this down better and help remedy the situation so you can use whatever endmills you want. Many people around here use the Carbide3D Zrn endmills in aluminum so there must be something off with the way you tried to run them and we can help figure that out but only if you share everything you did.
6 Likes