Headscratcher for me?

[TIAEngineering]

Hey Folks,
First post here and needed to get onboard as a means to try and hunt down an issue that is puzzling me.

I started this Next Wave journey by picking up a used SD110.
Had absolutely zero knowledge on CNC machines in general but have learned a lot over the past year.
And just like that, I now own 3 x Next Wave machines. Two of them are SD110's and the 3rd is a SD120XL
On top of that, 2 of the machines (1 SD110 and the XL) have now been upgraded to 24000RPM spindles and this is where I am having a problem.
I will do this in bullets, so it shows the timeline:

- The main caveat to this thread is that I cut aluminum almost exclusively which I understand the machines weren't necessarily designed to do but with practice and patience they do a pretty decent job.
- I started by picking up a spindle for the single SD110 as I had not purchased the other 2 machines yet.
- Machine was running very old firmware - 2017 - but I was new and didn't think anything of it. The machine worked fine.
- was on that steep learning curve but eventually got that machine cutting nicely.
- When I picked up the other 2, I needed to move the SD110 to a new bench as the original spindle was hardwired in and the bench area was the right size for the XL.
- So now the XL runs the original spindle I purchased and the SD110 has a brand new one. Exactly the same brand and model and exactly the same VFD settings (confirmed this)
- I had learned some practices for aligning the spindle to the bed but I also make waste boards out of MDF to do any cutting I do. This levels out the machine further.
- I had been working the XL for quite a while and it worked / works perfectly. Go it cutting just as good as the SD110 did. Finally moved on to getting the original SD100 setup and cutting.
- Was surprised and shocked when the SD110, with the brand-new spindle started galling the aluminum and this started to really impact the machine. Started to hog in and such. Anyway, it was truly horrible.
- Files were all using the same feeds and speeds as I had used before and as stated above, I went through every single parameter against the other machine.
- I did the deeper dive on aligning the head and even went so far as to tap in a couple of M4 screws to allow for a more accurate alignment fore/aft. Side to side was pretty aligned anyway but I also enlarged the
holes to the next size up so that I could more accurately align the spindle to the bed. None of that has helped and I have even reduced and increased speeds and feeds to try and find new settings that work but alas,
this just resulted in breaking a couple of 3.175mm end mills bits.

On one more note, all three machines have now been updated to the most current firmware and the pendants have all been upgraded as well. The XL continues to cut perfectly and the SD110 is sitting - waiting for an answer.
The only question I have that may help is whether or not the pendant / controller relationship may have something to do with it? All three pendants are physically, exactly the same and all 3 have the most current firmware.
The only oddball difference is that one of the pendants continuously asks me if anything is plugged into the front port of the controller (4th Axis and such). The other 2 pendants do not.
Hoping that someone out there has a similar situation and may be able to shed some light on this.

Great to have this forum.
Bernie

[Rando]

Hey Folks,
First post here and needed to get onboard as a means to try and hunt down an issue that is puzzling me.
<snip>.....
- Was surprised and shocked when the SD110, with the brand-new spindle started galling the aluminum and this started to really impact the machine. Started to hog in and such. Anyway, it was truly horrible.

Bernie:

I also do quite a bit of aluminum cutting on my shark, so hopefully I can help you out. I liken machining aluminum--compared to working with wood--on a Shark to walking on the edge of a razor blade. It takes a bit of effort to figure out how to balance on that sharp edge, but once you do, you'll eventually see that you can actually move around on the very small flat part of the razor blade. It's then, once you've figured out how to get to the right F&S spot and move around within it, THAT is when you'll find success. Here are some of the mirrors I've made on my now-ancient Shark HD2+

"Galling" isn't exactly the case here, I'm guessing. There's another related phenomenon called "built up edge" (BUE), where the aluminum will essentially weld itself into the micrograin structure of the carbide bit. This (yes, like the culprit in galling) is caused by the bit's cutting edge rubbing or sliding across the surface of the metal, instead of cutting through it. As tiny bits of aluminum collect on the surface of the bit, it makes more and more friction and heat, and essentially melting the metal. At which point the molten metal gets into the flutes, and it's game over. It's important to learn how to visually recognize built-up-edge as it begins to form on the bit. A dull bit will be much more prone to it than a shiny new bit, but more on that a bit later....

Here's a great article that explains the sweet-spot concept of cutting on a machine tool:

https://www.cnccookbook.com/feeds-speed ... -fs-email/

Disclaimer: I'm a long-time user of their G-Wizard products (calculator and editor), but I don't receive even a thanks from Bob

Below are some rather random thoughts on what is likely happening, as well as some of the things that I've found really help.

On small cutters like we're relegated to use, a huge source of broken bits and failed cuts is that the cutting face will literally shatter off the bit. Even a tiny nick out of a cutting face will ruin that mirror-finish you're after. The most often cause of this is varying chiploads. So, you might have your cutting parameters at 0.001" per tooth, but all of a sudden it jumps to 0.005", and then back down to 0.0001". The high number might shatter the bit, and the lower number might result in rubbing, not cutting. We are doomed in this regard with our machines because of a variety of things:

1) Machine Rigidity (well, a lack thereof) which allows the spindle to move and flex, moving the cutting face out of perfect position.
2) Low resolution motors, because they only have about 0.001" resolution, the stepper increments can result in a start-stop-start action relative to perfect position.
3) Spindle and collet runout error is a major issue. If you have a dial test indicator (the kind with the pivoting finger), take a reading on your spindle with a bit in place. I found when I was using either cheap eBay ER20 collets or even musclechucks, that my runout was often >0.010". Imagine how that random movement will affect chipload when I'm trying to get it to 0.002"! Once I moved to high-end Lyndex collets and collet-nut (yes, $50 EACH), my runout is now down to under 0.001" and my surface finish is much better, with almost no bit breakage.
4) Bit deflection is always an issue with thin cutters, so always use the shortest length-of-cut (and biggest diameter) bit that you can get away with. Those 1/8" diameter, 0.75"LOC bits should be reserved for getting the last bit of material (REST machining) out a deep pocket. The G-Wizard calculator does a good job of estimating deflection.

If I had to guess, there are two things going on for you: 1, your bit is dull. 2, the new spindle's collet (insert) and collet-nut have excessive runout.

Spindle bearings need to be run-in just like a car's engine, and they work best when the spindle is in the 90-110F temperature range, not cold, not even cool.

One way to prevent BUE on carbide bits is to get some of those gray scotch-brite abrasive pads. Not the red ones, not the green ones, but the gray ones. Holding the bit in your hand, fold a new pad around your bit with moderate force, and then spiral out the bit in the REVERSE direction. If you go in the forward (cutting) direction, you'll dull the cutting edge. But, going in the reverse direction will actually polish the cutting edges, and remove the beginnings of BUE. If it's happening, catch it early and clean the bit.

Whenever I am doing aluminum cutting, I keep on-hand a brand new "next" bit, and even another brand new "next next" bit. Trust me, there's nothing worse than having to wait the weekend, or even overnight, when something stupid happens.

There are a lot of tips-and-tricks involved with cutting aluminum to get a perfect finish. Some of them, in no particular order, are:

1) Make test cuts
2) Keep a cut catalog of what works and what doesn't
3) Use a spray mister and Kool-Mist with an intermittent pulse timer set to something like 0.2 seconds every 4-5 seconds aimed at the bit
4) Use a chip BLOWER to get the chips away from the cut; re-cutting chips leads to shattered cutting faces, chips welded on the newly machined surfaces, and making a general mess.
5) Radius the corners of pockets and profiles about 0.020" larger than the bit so you don't have axial-engagement spikes, which break bits!
6) Use radiused endmills so the sharp tips don't dig/dive in or break
7) Use high-speed machining toolpaths, available in higher-end CAD/CAM packages, and often NOT available in Vectric.
8) Use helical ramping on pockets,
9) Use lead-in and lead-outs with overlap > the bit diameter on finishing passes and profiles
10) Sometimes you'll want to use a finishing pass, sometimes not.
11) Almost always use climb milling for parts you want dimensionally accurate
12) Watch out for the top of the bit hitting a tall vertical wall when it's cutting the bottom layers; use LBS (Length before Shank) bits that have about 0.010"-0.020" diameter-reduced section between the (shortened) cutting flutes and the shank where you clamp the bit into the collet.
13) Invest in a dial-test-indicator (0.001" per tick) and make a habit of checking bit runout
14) Invest in a small set of high-accuracy collets and collet-nuts. I recommend Lyndex-Nikken, NOT eBay. If it's $50 for the set, you're getting shafted. If it's $50 per ITEM, you can be pretty sure it will have truly excellent precision and low runout.
15) Don't use a bit until it fails. You should be able to detect when it's starting to get dull; replace it then BEFORE disaster strikes
16) Invest in a good 30x magnifying loupe and look closely at the chips you're making; they can tell you a lot about what's going on, even when it's going right.

And I'm sure there are many more

Anyway, hope that helps get you farther along the path to dancing on that razor-blade's edge that is aluminum machining on a shark.

Regards,

Rando

[Kayvon]

That's a great photo, Rando. Very impressive what you've managed with the Shark. Next Wave ought to include your results in their promotional materials!

[Rando]

That's a great photo, Rando. Very impressive what you've managed with the Shark. Next Wave ought to include your results in their promotional materials!

Thanks, Kayvon! You're too kind

In some sense, they have. While the HD2+/3 generation was their lead model, they featured a bunch of my aluminum work in a display case at an annual tradeshow. Of course, my machine now is only barely a shark, since replacing the old-style steppers with hybrid stepper-servo motors twice as strong as the original, adding rigidity to the gantry backplate and under-bed cross-member, and putting in a Mach4 + Ethernet Smooth Stepper motion controller. It works like a dream, with actual measured resolution of 0.0001". Yes, one ten-thousandth That photo, however, was done on the old, nearly original system.

What I never understand is why NWA didn't buy out my gantry-carriage design; would have solved a BUNCH of issues with rigidity. And, of course, why they don't solve the static problem: it's just one resistor, after all!

Regards,

Rando