Newbie Issues Roughing Aluminum with PocketNC V2-50

First off, thanks to all the members on here, I've read countless posts and learned so much. I have the relatively new PocketNC V2-50, so it is difficult finding information relating to such a small machine. Here are the machine basics:
*0.268HP
*Spindle speed of 1,000-50,000
*Feed rate limit of 60ipm
*Shank diameter limited to 1/8"

I eventually plan on milling carbon steel, but starting off with 6061 Aluminum. I'm only using Harvey Tools designed for aluminum, best coating available, and I've tried ball mills, square center-cutting mills, and corner radius end mills, all ranging in 0.093" to 0.125" cutting diameter. I've tried to use the shortest length tools possible for rigidity. I'm having issues breaking tools relatively quickly. I've immersed myself in cutting parameters, but I'm still struggling immensely, even while utilizing Bob's GWizard. The only luck I've had is with a relatively shallow cut (40%) with a light step over (20%) at the recommended RPM for the tool diameter (0.093" diameter = 40k RPM). In this particular instance, I was feeding at a full 60ipm, but the resulting chip load was nowhere near Harvey's recommended roughing settings for that tool (likely closer to 1/10th). At that RPM, the tool burned out in less than 2 hours of cutting, and it was only removing a modest 2.5 cubic inches per hour; in hindsight, I can see how the tool was likely rubbing and the heat from that killed the tool.

Using Bob's GWizard, a 1/8" 3F ball mill (with 0.187LOC, total length of 1.5" which I set for a stickout of 0.75"), with my machines specs, called for 26k RPM with a full 60ipm at a specified DOC of 90% and WOC of 10% (in an attempt for HEM). I backed off all ramping & lead in/out rates to 5ipm. After helix ramping, the tool snapped before even getting toolpath cutting going. Reloaded a new tool, backed off the settings to 10k RPM and 53ipm, snapped her right off in the same fashion. And yes, I carefully entered ALL information (even advanced specs) for the tools & my machine into Bob's software, but obviously something is off there (which is incredibly frustrating considering I paid for the software and it resulted in $75 of broken tools right off the bat). I've tried so many recommended settings otherwise, using the "standard" basic equations and Harvey's recommended SFM (1000), and WOC & DOC for roughing for whatever particular tool I was using, to no avail. Again, it's tough to find information for similar issues for machines this size/power/spindle capabilities, because there just aren't many out there. I just don't understand where I'm going wrong. Yes I could probably back off settings until the MRR is to the point where I'm throwing up aluminum dust, but I would like to achieve Bob's balanced "sweet spot" of good tool life and decent MRR. Tearing my hair out (whatever I have left anyways). I feel like I've studied, read, and have a great understanding of machining basics (relatively anyways), and I'm getting nothing but broken tools. Oh, I'm using Fusion 360 for CAM at the moment if that matters, heading to HSMWorks soon though.

Here is the machine (spindle) power curve, if anyone thinks it would be useful.

I don't have any experience at the micro level. 6061-T6 usually cuts well but YMMV.
I avoid aluminum just because it is easy to fuse it to the cutter. When it works it works well, nice finish, easy to cut, etc. A bit of coolant, rubbing alcohol, kerosene, etc might do wonders for your aluminum.

But I've had it pile up rather quickly on the cutting edge of an end mill.
I once saw a 2" drill at Boeing surplus with a mass of Al fused to it. Small at the tip and maybe 7" dia closer to chuck end.

Try some steel; 1018, 4140 ... adjust your feeds and speeds and give it a try.
Carbide on steel you can cut dry but maybe not at those spindle speeds.
With steel you may get small, really nasty chips (splinters).

Some one on this list will have had experience with Harvey sized cutters, maybe in medical stuff.

Good luck.

First off, I would probably stop spending money on Harvey end mills until you sort out the basics. Until you get some funky variables in control and experience under your belt, end mills are going to be disposable items.

Second, it is kind of a funky setup with the Carbide 3D stuff, as you have a crazy high RPM spindle with no guts behind it, and nowhere near the machine or motion control quality of the kind of machines that are found in industry with that kind of RPM - this is not a Hermle, Yasda, Roku Roku, Kern, or Mikron. Trying to use performance guidance for that caliber of machine on a $5000 desktop mill is going to cause you to lose a lot more hair. I would ditch G-Wizard for HSM Advisor, and clamp down the RPM in the machine profile to 15k RPM and .25hp and 45IPM. This will make everything far more conservative, and keeping tools under .125" will keep you below the power limit. Running at 60IPM on a 60IPM max machine means you have every drive, motor, and the motion control system going as fast as possible, which is a recipe for problems.

Finally, I would do a complete machine diagnostics with a .0001" dial indicator. Start with spindle runout (dial indicator inside the collet face). Install a tool and check runout on the shank and the flutes. Then check machine alignment and motion - is it square? Does it have a bunch of backlash?

gkoenig said:

First off, I would probably stop spending money on Harvey end mills until you sort out the basics. Until you get some funky variables in control and experience under your belt, end mills are going to be disposable items.

Second, it is kind of a funky setup with the Carbide 3D stuff, as you have a crazy high RPM spindle with no guts behind it, and nowhere near the machine or motion control quality of the kind of machines that are found in industry with that kind of RPM - this is not a Hermle, Yasda, Roku Roku, Kern, or Mikron. Trying to use performance guidance for that caliber of machine on a $5000 desktop mill is going to cause you to lose a lot more hair. I would ditch G-Wizard for HSM Advisor, and clamp down the RPM in the machine profile to 15k RPM and .25hp and 45IPM. This will make everything far more conservative, and keeping tools under .125" will keep you below the power limit. Running at 60IPM on a 60IPM max machine means you have every drive, motor, and the motion control system going as fast as possible, which is a recipe for problems.

Finally, I would do a complete machine diagnostics with a .0001" dial indicator. Start with spindle runout (dial indicator inside the collet face). Install a tool and check runout on the shank and the flutes. Then check machine alignment and motion - is it square? Does it have a bunch of backlash?

Click to expand...

Great feedback, thank you. The thought had entered my mind that the spindle runout might be out of spec (0.0001in), but since the machine is new, I didn’t give it much credence; I’ll look into it. Regarding clamping down on machine limits and switching to HSM Advisor, I’m all for it, I can get going on that tomorrow (12/23/19) when some new tools arrive; I’ll report back. Questions:
*Considering the power curve I posted, do you think it would be acceptable to clamp RPM limit to 22,500 for roughing operations, since max torque occurs around that RPM range?
*Regarding MRR per HP: for Aluminum, typically 3in^3 per HP per minute, for 11L17 (machinable low carbon steel), probably closer to 1-1.5. So for my machine, I’m looking at 0.75in^3 for Al, say 0.25in^3 for 11L17; are these numbers still going to hold up given how small/weak this machine is and the 0.125” shank limitation (and no coolant)?

Not having coolant is going to kill bits even when you have everything else sorted. Can you set up a mister? I would expect that to be a huge improvement over cutting dry.

some machines dont track stable at high feed rates. machine/part/fixture vibration, servo oscillation not going around corners with small radius too good.
.
cutting parameters are very much dependent on tool holder, machine being used, part being machined, how part held or vise fixture etc
.
and of course metal can have hard spots or slag in it. you can be going along ok than bam break tool cause it hit something it didnt like especially if running near tool limits.
.
and if coolant not reaching deep holes or if recutting a lot of chips that can cause big problems

LOTT said:

Not having coolant is going to kill bits even when you have everything else sorted. Can you set up a mister? I would expect that to be a huge improvement over cutting dry.

Click to expand...

I know some users have set up some minor misting, I will look into this. Is coolant going to be a huge boost in my end goal in milling 303 SS & 11L17 (low carbon alloy)?

You have a crazy situation here trying to do real work on a hobby machine of this type. Still anyone can certainly appreciate your gung-ho-ig-ness about it. You seem to be taking to heart many of the suggestions given which is great.

While here I want to 2nd the coolant suggestions. Coolant is really going to make a big difference on gummy metals like aluminum, some stainless and low carb steel. Especially at the speeds and the near microscopic flute/chip spaces that you're dealing with in such small cutters.

I've used G-Wizard successfully for decades, but never on a machine like this. Let me suggest that you go to your machine setup page and fill in all the appropriate spaces there. Look at the spindle HP area and hit the adjust button. In there you can use the "curve compensate" function and plot your HP curve straight off the one you've already shared. Also there is a button at the top you can check to tune the software to "hobby machine" and/or "cnc router rigidity" status. Perhaps some experimentation there will give you better results. At least it should help you de-tune the software to fit the severe limitations you're dealing with.

Dave

Three words.... coolant coolant coolant.

Try spraying some WD-40 on your work.

13engines said:

You have a crazy situation here trying to do real work on a hobby machine of this type. Still anyone can certainly appreciate your gung-ho-ig-ness about it. You seem to be taking to heart many of the suggestions given which is great.

While here I want to 2nd the coolant suggestions. Coolant is really going to make a big difference on gummy metals like aluminum, some stainless and low carb steel. Especially at the speeds and the near microscopic flute/chip spaces that you're dealing with in such small cutters.

I've used G-Wizard successfully for decades, but never on a machine like this. Let me suggest that you go to your machine setup page and fill in all the appropriate spaces there. Look at the spindle HP area and hit the adjust button. In there you can use the "curve compensate" function and plot your HP curve straight off the one you've already shared. Also there is a button at the top you can check to tune the software to "hobby machine" and/or "cnc router rigidity" status. Perhaps some experimentation there will give you better results. At least it should help you de-tune the software to fit the severe limitations you're dealing with.

Dave

Click to expand...

Appreciate the kind words. I'm not ready to spend $50k on a 5-axis machine (which I need for my end application), so I'm learning on this $8500 wonder. I'll try playing with GWizards power curve settings for the machine, see what it comes up with. Sounds like I better get on the coolant train ASAP.

13engines said:

You have a crazy situation here trying to do real work on a hobby machine of this type. Still anyone can certainly appreciate your gung-ho-ig-ness about it. You seem to be taking to heart many of the suggestions given which is great.

While here I want to 2nd the coolant suggestions. Coolant is really going to make a big difference on gummy metals like aluminum, some stainless and low carb steel. Especially at the speeds and the near microscopic flute/chip spaces that you're dealing with in such small cutters.

I've used G-Wizard successfully for decades, but never on a machine like this. Let me suggest that you go to your machine setup page and fill in all the appropriate spaces there. Look at the spindle HP area and hit the adjust button. In there you can use the "curve compensate" function and plot your HP curve straight off the one you've already shared. Also there is a button at the top you can check to tune the software to "hobby machine" and/or "cnc router rigidity" status. Perhaps some experimentation there will give you better results. At least it should help you de-tune the software to fit the severe limitations you're dealing with.

Dave

Click to expand...

Tried plugging the power curve into GWizard (all the other settings were already correctly set), no difference. I'll email Bob, hopefully he can help in these regards.

I don't think not enough power is the problem. I use HSM advisor. It will often tell me to do crazy stuff. It's assuming ideal conditions, like tons of coolant, and no chatter warnings. You might also try 7075 AL as it is less gummy. I'd cut the RPM in half again until you know what works.

sdinzy said:

Appreciate the kind words. I'm not ready to spend $50k on a 5-axis machine (which I need for my end application), so I'm learning on this $8500 wonder. I'll try playing with GWizards power curve settings for the machine, see what it comes up with. Sounds like I better get on the coolant train ASAP.

Click to expand...

When researching the machine in question here, I was surprised at the cost of this small machine you're now dealing with. Unless you are space limited, I think you could have done yourself a great favor by buying an older used CNC mill w/tooling for the same price. Older mills from the 90's (and certainly earlier) are going for dirt at auction. Your planned jump from this small machine to a real 5 axis is much-much bigger then moving from an old 10,000 odd pound CNC mill. Except for programming, job organization and some tool design knowledge and skills you might be learning now, there will be little of what this small machine teaches you that will move directly over to a real one. From what I can see you can tuck this machine of yours into a suitcase. I don't know... hopefully I'm wrong about all of this. You're giving so much energy to it, I hope a bunch of it doesn't become useless. Or worse yet, lead you to believe in things that aren't true in a full size machine. Oddly enough, the stuff you talk about in your original post would likely not be as problematic if you were on a full size machine. Anyway... Good luck with this journey. It's a good one.

Dave

sdinzy said:

*Considering the power curve I posted, do you think it would be acceptable to clamp RPM limit to 22,500 for roughing operations, since max torque occurs around that RPM range?

Click to expand...

The problem is that the 60IPM limit throws you so far off the feed per tooth ideal for high RPM spindles that you’re going to always be burning up tools. I run 1/8” finishing mills at 16k, .05 WOC, .25 depth and 90IPM. You would be running at significantly less engagement, at way higher RPMs and making nearly dust.

Let’s get you to a place where the spindle is bogging down on HP slightly, then back the feed parameters off till we find the happy place.

*Regarding MRR per HP: for Aluminum, typically 3in^3 per HP per minute, for 11L17 (machinable low carbon steel), probably closer to 1-1.5. So for my machine, I’m looking at 0.75in^3 for Al, say 0.25in^3 for 11L17; are these numbers still going to hold up given how small/weak this machine is and the 0.125” shank limitation (and no coolant)?

Click to expand...

I would ignore MRR at this point. The initial goal (after a complete machine alignment and basic motion assessment) is to just find some stable cutting conditions and get some successful parts made, even if they take a lifetime.

Also yes to coolant- misting would be good, but even just air blast over the part would be a great benefit. You’re making tiny chips that can stick inside the gullets of the tool and make it into a plow.

1. Where is this "$50K 5-axis" machine of which you speak?

=> Serious point = Does your work really need 5-axis? Maybe not. (Observation from a guy who bought a 5-axis machine as his first VMC early in his career....)

2. If you can't do fluid coolant, try mist. If you can't do mist, try spraying WD-40. If you can't make those work, try blowing a lot of air on the cutting area. (Do you have a compressor???) This is done as preferred technique in some processes in hard steels. And I can tell you straight up that it helps a lot with aluminum.

3. When your endmills snapped, did you examine the cutting edges? They could have snapped because the machine jerked on them. Or because fusion gave you a path that buried them in a corner. Or some other thing that suddenly increased load.
But they might also have failed because they got aluminum welded to them, or heavily built up on them.

4. Don't feel too bad - snapping small endmills is sometimes a problem even on my 14K# DMU 60. So with a rather small machine combined with rather small endmills, the difficulty of your task is about squared.

[But mostly, read gkoenig's post #15 carefullly.]

gkoenig said:

The problem is that the 60IPM limit throws you so far off the feed per tooth ideal for high RPM spindles that you’re going to always be burning up tools.

Click to expand...

Yes this is exactly what's happening, as they'll run fine for a bit (aka less than a couple hours), then dull out. Or if I get to aggressive with the WOC/DOC, snap right off the bat. The other problem is the power output throughout the RPM range; at 20k, I've only got 0.15hp, which makes it tough for the tool to cut through anything of substance. I'm starting to lean towards having a machine shop do the basic roughing of my stock for me at this point, then I can utilize my 5-axis for the finishing work.

gkoenig said:

Let’s get you to a place where the spindle is bogging down on HP slightly, then back the feed parameters off till we find the happy place. The initial goal (after a complete machine alignment and basic motion assessment) is to just find some stable cutting conditions and get some successful parts made, even if they take a lifetime.

Click to expand...

So what would you recommend? To be honest, I only started with Aluminum because I thought it would be easier to learn on than 11L17 (highly machinable low-carbon steel), but that doesn't appear to be the case with all the issues that the non-ferrous material brings. Can we just focus on the steel instead, as that is what I'll be working with in the end anyways? I've seen carbide SFM for 11L17 range from 200 to 400, although it's probably closer to the higher end since Harvey has an SFM of 250 recommended for less-machinable steels that are harder (11L17 is around 140 Brinell, the recommendations from Harvey for these medium-alloy tools start with a Brinell of 200). I've got (6) Harvey 907308-C3's arriving tomorrow, so that would be a great tool to try and get dialed in for this roughing application. It's 4 flute, AlTiN coated 1/8" end mill, corner radiused 0.01, with a stickout of 0.81", so it should be pretty rigid. Roughing IPT recommendation of 0.0008 by Harvey. Plug these numbers into the "standard" formulas (assuming SFM of 350), and we've got 10,700RPM with a feedrate of 34ipm. Would you adjust these parameters? What are your recommendations for WOC/DOC? Thank you immensely for your help!

bryan_machine said:

1. Where is this "$50K 5-axis" machine of which you speak?

=> Serious point = Does your work really need 5-axis? Maybe not. (Observation from a guy who bought a 5-axis machine as his first VMC early in his career....)

Click to expand...

Yes, my finished part is definitely a 5-axis undertaking; it's more of an aesthetic part than a mechanical part. Lot's of fillets, curves, bent cylinders, etc.

bryan_machine said:

1. Where is this "$50K 5-axis" machine of which you speak?

If you can't do fluid coolant, try mist. If you can't do mist, try spraying WD-40. If you can't make those work, try blowing a lot of air on the cutting area. (Do you have a compressor???)

Click to expand...

I have a Gast compressor (with a regulator) blowing 25PSI through the spindle, which ends up blowing on the part. I have zero issue buying another compressor that blows directly on the cutting edge. My machine has a lot of exposed cables and whatnot, I would be hesitant to set up a misting system, but I'm open to WD-40; with this cutting rate though, I'd be sitting in front of the machine all day.

If you are going to cut aluminum with small cutters coolant really helps. A mist buster style coolant dispenser works great without a cloud of mist. I keep a container of Sodium Hydroxide/Potassium Hydroxide around. As soon a tool starts getting packed throw it in and let it sit overnight, completely clean of all aluminum. If you can deal with the potential explosion hazard of Isopropyl alcohol it works really well and reduces load on the cutter.

After looking this thing over it doesn't look like you are going to be cutting much of anything, unless it's foam. I'm gonna go out on a limb here and say you picked the wrong machine.