Horrible issues with Aluminum and Zrn/Tin bits

Not having any luck with any of these bits on my Nomad. Some of them aren’t even lasting 1 cut!

The only luck I have had with no issues are some bits from Kyocera TiCN bits. I even had better luck with uncoated than the Zrn ones, which does not seem to make sense!

My questions: first,any ideas why this is true? I ordered some lye to try and clean them, but the Kyocera bits work perfect without changing any settings

Second, for the Nomad 3, what are ideal RPM settings/speeds? I find it very frustrating the everything I can find from Carbide is for the 883 pro. I am shooting for 30-40 IPM at .008 - .010" depth. What RPM should I set it at?

I have had a lot of sucess, but cannot understand why I cannot achieve any good results with Carbide3d, or amana ZRN coated bits

Thanks!

I did fine w/ a #274Z the one time I used it in 6061 alu. using the stock feeds and speeds in Carbide Create.

Which alloy of aluminum are you cutting?

Using what feeds and speeds?

Using what CAM tool?

The Nomad 883 feeds and speeds should be a good starting point — once you have a chipload which works you can adjust feed rate and spindle speed so as to maintain that chipload while cutting your parts so as to take advantage of the greater possible spindle speed on the 3.

I purchased the Nomad 3 so that I could go faster, as advertised, so using the 883 settings seems to kind of defeat that purpose.

Cutting only 6061; my goto settings right now is 30IPM, .010" depth, 16000-18000 RPM. The Kyocera bits work flawlessly; the carbide3d, haven’t had any success at all. I have an amana ZRN single flute that worked ok, but still filled up with aluminum pretty fast. I am sure it is me, but I have tried a ton of changes with no sucess.

I have used both Carbide create and fusion.

I bought a 274Z, and it broke literally second into the first time I used it, which was very disappointing to lost that much money that fast, with no explanation (used safe settings to test it only 10 ipm, at .010" depth and it literally snapped 5 seconds in). I know it would be very hard, but I wish carbide stood behind their end mills, but I understand why, since a lot of people would probably take advantage of it.

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:

  1. Make sure you are cutting a machinable grade of aluminum. 6061 or equivalent is the best.
  2. Keep your feed per tooth at least 0.001".
  3. Make sure the chips are clearing the cut.
  4. 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.