Shapeoko vs. Aluminum round 2, why don't HSM best practices work?

Much thanks guys. Like @Vince.Fab said, increasing cutter engagement helped with stability greatly. The chatter completely disappeared when I went back to a shallow wide cut, I guess I should just stick with what works and no try to optimize too much :slight_smile:

I ended up running the tool path with my “Best Performing” settings above (0.9mm DOC, 4mm WOC), but with the adaptive tool path keeping a constant load in the corners (vs. the 2d Pocket I used previously) I was able to run at 150% feed rate!

I also tried out a radial finishing pass which ended up looking pretty good. Now I just wish I’d run it on the axial surfaces as well.

Completed part fits up great (threads were drilled/tapped off machine):

Here it is installed in the car. This particular bracket is to adapt a cheap off the shelf EGR linear position sensor from a Ford 302 to measure turbo wastegate actuator position on my track car. Please forgive the dirty engine bay.


Now that’s a good looking part! EFR with a TurboSmart actuator? Good combo.

Ide love to see the file if you don’t mind sharing. You can also probably get a better wall finish (less faceting) decreasing tolerances (I use 0.0001) and using a constant engagement path like ramping. Awesome you were able to increase the your mrr so much.

Boring also works very well on circular surfaces. Any plans on trying out thread milling in the future?


The only reason I didn’t thread mill these parts is that my mill is too large. These are M5 and my mill is for M6+.

You’re correct on both fronts, it’s an EFR7163 with the new TurboSmart dual port actuator. I wasn’t willing to pay >$100 for WG position sensing capability and I figured it would be a fun project. It’s on a E30 w/ the stock M20B25 running ~15psi or 300 whp-ish. I need to get it on a dyno as soon as my buddy gets his fully installed and running.

Already ahead of you on the thread milling, it’s great. You have any good leads on reasonably priced thread mills? Here’s an oil manifold that uses the stock oil pressure switch port on the block and adds capability for oil temp, oil pressure, and turbo feed (while maintaining the switch) from a couple weeks ago. Less than ideal surface finish, but an okay overall result. It will bolt onto the stock AC compressor bosses on the block for nice packaging.



Thanks for the feedback and actually using the thing! I fixed the feed force problem and a couple others and will post the latest version on the SFPF calculator thread shortly. What forces do you like on your various machines?

I added another sheet to the workbook that replaced the HF Spindle with your VSEC BLDC motor. If you use it for that you’ll get more accurate results. The increase in motor current when cutting should provide a good measure of actual cutting torque (provided it’s accurate). That, in conjunction with router cutting speed, will give cutting power. I suspect that the VSEC tool’s “Power” is actually VSEC input power.

I don’t know about that, but its the lowest chip thickness their calculator comes up with. I posted that on the SFPF calculator thread along with matching pictures of the three different spindle type options the latest workbook offers.


I expect that the electrical power & current measurements on the BLDC motor will be considerably easier to map to mechanical cutting power and torque than a VFD driven spindle. The VESC has lower losses than a VFD and the BLDC motors don’t have a rotor to induce magnetising currents in, as well as appearing to have lower overall losses than the spindles.

I think you switched the DOC and WOC entries on the worksheet. I guess you’d call this HSM (High [spindle] Speed Machining) in conjunction with HFM (High Feed Machining where WOC >> DOC) rather than Vince’s HEM (High Efficiency Machining where WOC << DOC).


Yes, you’re right. I’m used to seeing WOC before DOC in Fusion 360 so my brain defaulted to that. I fixed the screenshot in the previous post so people won’t be confused in the future.


The VESC provides current into the motor. Torque is the product of motor current and the motor’s torque constant. Power is proportional to torque and motor speed. So the calculation is only dependent on the accuracy of the VESC’s current measurement (which should be quite good) and the motor’s torque constant (which should also be quite good).

The SFPF Workbook tries to do the same thing with HF Spindles (i.e. calculate a torque constant). But, as you’ve pointed out, the magnetization currents make that more challenging and consequently less accurate, especially when so little of the spindle’s capability is utilized.


Once I get my power meter I hope to be able to run my spindle through the no-load speed sweep and then start getting real power kW and motor Amps (once I get around the not-actually-modbus signalling from HuanYang) so we can put measured data in place of some of those assumptions in the spindle model sheet.

1 Like

There are software tools that take into account the machine rigidity (roughly) - remember that the HSM strategy is based on how well it works in large machining centers, where time is money, not hobbyist machines that have a lot more compromises. That said, it does work, but you need to tune things in a bit. @Vince.Fab has way more knowledge than me here, but as he says, takes some work to tune in.

GWIzard is a great tool, and well worth the money. Bob really likes the SO3 machines, and has done a fair amount of work to make the tool very friendly to them. If I remember, there’s a free trial.
He also has a great “get started with aluminum on CNC routers” post. (and some FAQ’s down at the bottom. (nope, not a paid shill, just really like the tool, and it’s saved me a lot of broken tools!)


As explained here, as well as countless other reasons, I’d pick HSMAdvisor over GWizard any day. However, Kennametal’s NOVO calculator is free and likely more accurate than anything else when milling metals with their reasonably priced material specific endmills. But, like with GWizard, you have to divide the cutting torque by the cutter radius to get cutting force.

1 Like

Not arguing, just saying I like it, and for the others, including @Kai , who the reply was to, just wanted to mention there were other tools to help with HSM on small machines.

You asked about reasonably-priced thread mills. I find Rogue Systems Inc. on eBay to provide them for good prices. Roughly $22 for any threadmill.


Or, direct,


Thanks guys, these are both cheaper and a lot faster to get than the ones I got previously on AliExpress.


Just to add a little more complexity, how are people calculating their cutting parameters for contouring 3d surfaces w/ ball end mills. It’s no longer as clear cut as DOC and WOC when you have a spherical cutter. Depending on how steep or shallow the surface is, the part of the cutter which is engaged changes (affecting surface speed) as well as how much it’s engaged (not sure if this is accounted for in Fusion 360’s CAM or not).

Here’s an example of a part I machined in 7075. I would like to think I could achieve better surface finish, but again I’m not sure if my expectations are just too high for a kit based router. Luckily the surface is completely non function and was just a chance to try out something new, but in the future I could foresee wanting to create conical or spherical surfaces with nice surface finish without having to buy a lathe (or for parts too large to fit on a lathe, e.g. 3-pc wheel centers).

0.2mm stock was left before this operation and I used a scallop w/ a 0.2mm stepover w/ a 1/4" 2 flute uncoated carbide ball end mill.


Have a look at NYCNC’s video with some info on ball end mill engagement calculations for propper SFM.

"carbide cutting tools CNC ground in the USA just a stone’s throw from the world famous Rogue River." World famous for catching on fire! :wink:

Carbide Depot sells “pro grade” stuff at reasonable prices and has useful technical resources.

1 Like

To get the best 3d surface finish you might want to try a single flute ball endmill. Datron and 2L inc make them as far as I know. A single flute will minimize the effects of runnout and machine force.

I’m my early days with billet intercooler endtanks it became painfully obvious how direction, stock to leave after roughing, and engagement angles work.

Try bumping stock to leave to 0.5mm and run toolpaths where the side will engage before the bottom. You need enough stock to create enough tool pressure to stabilize the cut. Depending on part geometry, bottom to top is usually the best bet.

Your tolerance and smoothing options will greatly effect the finish especially when feed speeds are higher.

Checkout this set of calculators

Pro tip - match chipload with stepover to create the best finish.


This topic was automatically closed 30 days after the last reply. New replies are no longer allowed.