Spindle stall, is my PNC V2-50 power limited?

I’m new to machining and have been spending a lot of time trying to understand feeds/speeds. There are lots of great resources online, but I’m a bit confused why a lot of the advice doesn’t seem to apply to my PNC V2-50. I tried using the two most popular calculators (G-Wizard and HSMAdvisor), but the numbers they give are way off from what I’m seeing work on my machine.

I came across this blog post: Pocket NC power limit | A Modicum of Fun that references an old forum post that describes how older PNC-50s were power limited until things were proven out. I bought mine in May 2021 so I wouldn’t think it would be limited as described in that post. It’s not easy to find the power rating of the spindle, but I’ve seen several references that it’s a 200W spindle including the manual (https://www.nsk-nakanishi.co.jp/industrial-eng/download/manual/sale/OM-K0454_003_EM25N-5000_EN_160119.pdf). I bought a power meter to see how much power the PNC uses to see if it seems limited.

It seems like the base load is about 40W when nothing is spinning. I see it go up to about 70W often while it’s happily chewing away, and it goes up to about 80 when it struggles a bit. Here is a video showing my PNC and the meter ending in a spindle stall: PocketNC spindle stall with watt meter - YouTube. It seems like it isn’t using anywhere close to the 200W available from the spindle. If the baseline is 40W, and the most I see is like 80W, then it can’t be using more than about 40W for the spindle, and that’s not counting the steppers.

Is my machine operating as intended? I love my PNC. I’m having a blast w/ it and learning a ton, but I’m struggling to avoid spindle stalls.


P.S. I also found this post. I wonder if this person was dealing w/ a power-limited PNC: https://www.practicalmachinist.com/vb/cnc-machining/newbie-issues-roughing-aluminum-pocketnc-v2-50-a-371780/?highlight=pocketnc

Sounds like the guy on the Practical Machinist was working with a V2-50. That was two years ago so it wouldn’t have had the NSK spindle upgrade that recently became available. Is that what you meant by power-limited spindle?

FWIW, I find that HSM gives me much better data for my Tormach mill than G-Wizard does. On HSM, edit the machine definition to provide the correct travel speeds and spindle speeds, HP, and torque. If PNC can’t provide the spindle HP/torque data you may be able to get info that from NSK themselves.

1 Like

Thanks for the reply. No, afaik the HSM spindle is the same electronically, just has a different mechanism for holding, As long as nothing is slipping I don’t think the distinction is relevant for what I’m discussing, unless I’m missing something?

What tools, feeds, and speeds are you using that are resulting in stalling?

I’m used to industrial machines and the usual settings don’t work on the PNC. The spindle is hardly rigid and the A table only slightly more so. All my numbers start very very conservative and get dialed up while listening to the machine.

1 Like


I’m reluctant to dig into my feeds/speeds, because I’m not sure that’s really the question here. I’m mainly wondering why my power meter doesn’t ever go much above 80W despite a 40W base load and a 200W spindle. If I were seeing more power usage, but then stalling I’d be questioning my feeds/speeds more. I’ve been able to find speeds/feeds that are working w/ a very light cut, but I’m wondering if the machine is using its full power available.

That said, yesterday I was working on a part successfully (at least as far as the cutting goes, other mistakes were made) w/ this configuration:
Brand new Datron 0068630E
40k RPM
47 in/min
0.011811 in stepover (10%)
.04 in step down

I’ve been keeping the RPM at 30-40k as I believe that’s the sweet spot of the power curve, and keeping the feed rate high to avoid rubbing, and then adjusting the cut so the spindle doesn’t stall. It sounds great and makes decent chips as long as I keep the cuts very light to avoid stalling the spindle. I feel like if the spindle were using more wattage I could taker deeper cuts.

I would definitely be interested in what PNC has to say. 47in/min on a machine which is only capable of 60in/min even in rapid with a chip load of .001IPT seems very aggressive for this machine in my experience. When cutting wax .0025IPT is max feed on mine.

Again, curious what PNC says about not drawing full power.

Hi Jake,

You are correct, your machine is new enough to not have the the limited power to the spindle.

The 200W rating for the V2-50 is a maximum power rating. This means that it will not run continuously at that wattage, only peak very briefly there (sometimes not detectable). The 80W reading you are seeing is about right for continuous use of the machine.

Due to the V2-50’s high spindle speed, high speed machining techniques paired with dry machining techniques produce the best results. In general this means that you should be taking a very light WOC, fairly deep DOC and a fast feed rate while using a single-flute tool. Here is an example of a reliable S&F recipe I use with the V2-50 machines:

Material: 6061 Aluminum
Tool: 3mm Datron Single Flute (0068630E)
RPM: 40K
IPM: 31.2
WOC: .006"
DOC: .15"

Hopefully this helps!

Q Rothing
Applications Engineer, Pocket NC

Thanks for the quick reply, good to know it’s working as expected.

I’ve read that you should prefer more depth and less width to take advantage of the whole flute length. I erred a bit more on width for two reasons:

  1. I am concerned that if you get too shallow you start rubbing again like it did when I was using lower feed rates.
  2. When doing an adaptive tool path it’s annoying when it’s clearing a shallow area to be taking shallow width cuts even though it’s already doing a shallow depth, and there doesn’t seem to be a way to tell Fusion to look at the cross section so it can take wider cuts when the depth is already shallow.

I’m probably just being overly conservative about 1 since your numbers are working well, and will definitely try them, but less obvious how to work around #2, I suppose I can divide things into multiple adaptive entries or something, any ideas?

While we’re at it, what do you like to use for helix ramps w/ the 0068630E in 6061? I feel like my settings may be wearing out tools, and not as easy to find advice on that. I’m doing a 2 degree ramp, 40krpm, and like 15in/min feed. Thinking w/ the lower feed maybe I should lower RPM, and maybe lower the ramp angle?

Hi Jake,

Yea the small WOC, large DOC method can be a bit annoying when only needing to make shallow cuts. I usually just try to adjust the recipe so that I end up with a similar material removal rate (MRR) which usually results in a combination of a larger WOC and altered feed rate.

I think I usually set my helix ramp entry to about 4 deg. and keep the same speeds and feeds. In general, I have found that the best sounding ramp entries are the ones that don’t have much changed from the cutting speeds and feeds.

1 Like