Would not use acetone … Everything nearby will melt, lol.
IPA is what I use.
I notice you reduced rpm and feed rate. Whilst this has maintained a correct chip load your surface speed is now quite low for a carbide tool on aluminum.
I think you are very close to a clean cut. I think with a tweak on lube and surface speed it will be great.
HSMAdvisor was giving me the very low rpm, decided to give it a try since this Spindle is rated to give 100% torque down to ~7k rpm I think it was.
Bumped it up based off this video. I know thats for the Shapeoko, but it seemed pretty conservative.
HSMAdvisor thinks this RPM is ridiculous lol. (I also upped the stepover a smidgen)
Going to get a short clip of this when I start it.
It’s certainly doing a lot better with iso and the new params. There’s still quite a massive amount of resonance that is probably making my neighbors hate me, but it doesn’t seem to be making the cut significantly worse. I’m probably going to need to reinforce this thing a lot to be able to handle the spindle.
Have you tried running a different endmill at all? If you have an 1/8th inch 2 flute I can give you feeds and speeds to try out that are proven to put almost a mirror down. That way we can rule out of its machine or endmill/feed speed based. Something is going on here because you should not be getting galling like that on a brand new endmill.
That does seem a lot better. I notice the resonance is slightly there when it is repositioning and the tool isn’t cutting on load so it could be something isn’t tight on the machine. I would definitely give Rob’s 2 flute params a go.
Looks like you have quite a DOC now, you could reduce that slightly.
Is the galling on the left of the cut from this cut or a previous attempt? The floor finish looks pretty smooth (please confirm)
Usual preface, I’m with PreciseBits so while I try to only post general information take everything I say with the understanding that I have a bias.
In general I think you’re deflecting. You’ve basically removed the previous limit of spindle power and are now running up against the machine strength limit (and motion limits where you’re losing steps). Those numbers from HSM don’t make sense to me for the forces. If I can, I’ll check some other sources when I’m back at work tomorrow.
If you want to test it, I ran through a simple deflection test here:
A few more things.
Although adaptive toolpaths can make use of it, be careful with WOC/stepovers of less than half the bit diameter. It will cause chip thinning where you are cutting less than you calculated chipload. As an example your last listed HSM screen is 18KRPM at 36IPM with a 33.3% WOC/stepover. It’s calculating that as a 0.002" chipload. That is correct without chip thinning (36/18000/1 - IPM/RPM/Flutes). However, with chip thinning at a 33% stepover you are actually only cutting 0.00188" chipload. That’s not too far off. Let’s say though that we are using the 6% from your first HSM screen. Then your actual chip is only 0.00095", less than half.
That can greatly confuse matters if you are trying to come up with limits based on chipload. It may also explain some of the issues you are having as the smaller the chipload the hotter your cut will get. You could also be rubbing/grinding instead of cutting if you are not hitting the minimum for the material/tool. That will both increase the heat and the cutting forces.
Be careful with this. The max torque for an ER11 collet is 18 ft-lb (24Nm) for a standard nut and 12 ft-lb (16Nm) for a mini. If you go over this not only are you potentially causing damage but you may be inducing runout which will make matters worse.
Also since I’ve run into it a few time here recently… Are you snapping your collet into the nut before using it?
In general I’ve never seen a cutter that can’t do at least 600 SFM in 6061. That works out to ~18K for the 1/8" and 9K for the 1/4". Most decent cutters can do at least 1000 SFM which is ~30K for the 1/8" and 15K for the 1/4". Specialty cutters can go much higher than that depending on what they are shooting for.
Hope that helps. Let us know how it goes.
I do! I have a few of Amana’s 51830 55º Helix End Mill 1/8" that I can use.
That is from a previous attempt. I’ll lower the DOC a bit.
I love your pcb bits 
Ron spent a few hours with me a while ago helping me design a jig for double-sided pcbs.
That makes sense, going to try out this here:
I have separate nuts for all my collets so they are already snapped in, I make sure they are still snapped in though before I screw it on
Edit: That was prob one of the worst attempts, missed some Z steps and missed some X steps, which I didnt noticed until it plowed into the top of the model. Tweaked and tried again, still missing large amounts of X steps now. I think the 50% WOC brought that on
Seems like its going backwards after upping the WOC. This was with 40% stepover and .04" stepdown. Could watch it skip X axis steps as it went.
The plunge that happened after I didn’t notice the missed steps is on the bottom there, that was with 50% stepover and same stepdown.
That is what, 1mm DOC. Maybe back that off to see what happens.
Just looking back, your posting of fusion settings (adaptive 7) stepdown was in mm but HSMA calcs in inches.
I don’t see how 1mm could cut worse than 1.25mm in adaptive 7. There must be another issue. Or units finger trouble 
Yeah, 1mm. I used both inches and mm 
. Everyone typically talks about chip loads and feeds in inches so I’ve gotten used to those but I like to use mm for dimensions. I make sure I paste the right one into fusion. How much lower step down do you recommend? .6mm?
This is with 0.6mm DOC and 50% WOC, could watch the cutter bounce back every time it went it for a cut
Sorry it’s taken me this long to write back. I got one previous post replied to then I haven’t had even 5 minute gaps between having to deal with something. That also might make this more disjointed than usual as it’s written 2 or 3 minutes at a time over 3-4 hours.
So I ran some numbers in millalyzer (it’s the easiest to setup for this). While it’s far from perfect it does give some good numbers for what’s going on in the cut. I used as much data for the tool as you have in the HSM numbers. Don’t know rake so I went with 20°. That will change the forces but it’s shouldn’t be enough to render the data worthless. I’m going to call the previous one with 0.060" DOC, 0.0833 WOC, and 0.00188" chipload dataset 1. Dataset 2 will be 0.040" DOC, 0.125" WOC, and 0.002" chipload. Common to both 18KRPM, 1" stickout, 0.75" flute length, 0 radius, 0.25" diameter. Here’s the results:
Dataset 1:
Dataset 2:
Dataset 1 has higher peak forces but less overall time in cut per flute per rev. It’s a combination of chipload and stepover. I think regardless you are at the edge even with the previous cut or something else is changing.
In theory dataset 2 while requiring more torque should be a better cut. It has less peak forces and smoother engagements. But that means that the steppers and spindle are working harder and/or longer at peak load potentially causing the issues.
Changing millalyzer to the “desktop cnc”, which my understand is, based on the nomad (another reason I’m using it for this). Then changing the spindle power and max RPM for the new spindle I now get these numbers.
Dataset 1 Desktop:
Dataset 2 Desktop:
The things to note here are the tolerance is about triple and the “peak forces” warning for both. I don’t know how good this model is for the nomad but it’s saying both cuts are at the edge or over the peak/mean force limits for the machine and causing at least some deflection.
So there’s other things not taken into account here. The first is again the deflection. Since you are climb cutting the deflection is pushing the cutter away from the material. This means that whatever your deflection is gets added back to WOC in the next cut.
I don’t mean to be depressing, especially after you have just made a big upgrade. But the short version here is that you are running up against the limits of your motion system and I would bet deflection (machine rigidity). Forces are functionally cubic material removed per flute per rev. Although tool geometry can change the force amount and direction of those forces. So I would look at reducing either the pass depth, tool diameter, or chipload. My personal choice would be tool diameter.
Then I’d use this method. Start off at an absurdly low DOC. Something like 0.005-0.010". This will help to minimize any deflection and force limits. Then run passes at different chiploads to find where you get a decent/good cut. I don’t know that tool geometry well enough to give great numbers on that but don’t start at less than 0.001" chipload. Probably the best cut for the mill is going to be over 0.002" chipload. After you find that number use it and start running test passes incrementing the DOC. You should reach a point where you realize that you are exceeding a maximum (e.g. skipped steps, large change in volume, poor cut quality, etc). Stop there and then back off 5-10% to give give yourself some margin for things like tool dulling. Alternatively, you can use this data as a base line for forces to use in a chip thinned adaptive if that’s your preference.
I have more that I’d like to expand on with this so if I can I’ll come back later and fill out some things. But going to post this for now. Let me know if there’s something specific you want me to address or that I can help with.
Thank you! This is super helpful! I figured I was going to prob hit the limits on the rest of the machine with such a more powerful spindle, i’ll have to upgrade that next 
There is so much resonance going on that the machine is actually bouncing around occasionally which I imagine will make deflection worse than it already was by a lot.
I have a set of Trinamic drivers that I’ve read are significantly better than the stock TI ones, I’ll spend some time trying to increase the rigidity of the machine as well, might be able to bolt it down to something much sturdier. The ball screw upgrade might be worth it, seemed more complicated though.
Millalyzer looks super useful! Is that free software I can download?
Millalyzer is very nice software though its not free. Has a few small bugs but its a one man dev team. I use it for my hdm. You can import your machine settings rigidity power limits ectect and it will spit out technical data on the simulated cut vs the optimal cut force graph. It will also tell you how close to your machine limits you are based on settings you input. You can set a peak force limit and high force limit for each axis and tool tip and it will tell you when you nearing your limits but also tell you when you have potentional other problems like rubbing and tool stress. Its nice for learning about feeds and speed visually but its not needed.
Oh my god lmao the VFD actually did have the direction set backwards. Mechatron told me it was fully preconfigured so I didn’t bother to check through everything 
No wonder its been doing fairly poorly 
Nice catch Rob.
Well, that will defiantly increase the cutting forces. Nothing like milling with the back of the tool. On the plus side I bet the edge is barely worn at all.
Kidding aside, that’s actually really disappointing from Mechatron. They usually do a good job with those and a decent number of our customers have had good luck with them.
Think the other questions were answered. You can grab millalyzer here if you want it (Link). It’s €69.00 for a forever license. Honestly it gives a lot of good data. But it’s idealized data that you still have to apply a lot to and know what the values actually mean. The help pages are ok but they assume a certain previous level of knowledge.
Let us know how it goes.
I was pretty disappointed with the performance the first time I tried a battery powered circular saw.
Later when turned the blade around I was much happier.
Oh wow, nice spot Rob. Gotta see this spindle cut some decent chips now it is diagnosed. Awaiting new vid with metal flying and mirror finish…
Sick, glad it was something simple. Do yourself a favor as a new machinist and watch this video from nyccnc @Vince.Fab made. https://youtu.be/b8CndwnfoCM . Please do not get caught up in every little technical detail and just enjoy cutting. If your machine is making angry noises and not sounding smooth it probably isnt happy. Most if not ALL pre done feed and speed programs assume your using a vmc not a small desktop mill so the feeds and speeds almost never translate over well. It is very easy as someone who chases numbers to get stuck in a black hole and it can suck the fun out of making things. Also Welcome to the club of custom nomad 3s! Vince has one (older nomad 883 iirc) and I also have one. Now you have one. This here is mine Bromad - The nomad 3 dewalt dwp611 conversion project
