October 6, 2020

Benchtop 5-Axis Mill

This was inevitable, but the pandemic has accelerated my home-shop setup.  What with leaving the lab almost a year ago (I miss you Lab Haas) and no MITERS for the foreseeable future, I haven't had access to any machine tools other than the tiny lathe for a while.  Time to fix that.

I've been following Pocket NC since 2012, after seeing them at the NY Maker Faire - they make a tiny but surprisingly capable 5-axis CNC mill.  It has basically the same layout as the big GROB machines, with a horizontal milling spindle moving in Z and X, and a cantilevered trunnion on the Y axis.   I was tempted to get one of their machines, but I think they're just too small and underpowered (and pretty expensive) for the sort of parts I make.  In my search for a small-enough-to-carry-upstairs-into-my-living-room-but-not-too-small CNC mill, I ran across a scaled-up Pocket NC clone made by a Chinese company, Xinshan Tech.  I couldn't find any examples of real people outside of China owning the machine, but after some emails back and forth with the company, including a bunch of videos, I was convinced that the machine was real and not a scam.  This machine was appealing, since it's a fair bit bigger than the Pocket NC, with ~50% more travel in each axis, all steel, servo (rather than stepper) driven, and much heavier (~70 kg).  I've gotten along just fine with 3-axis machines up until now, but I couldn't actually find any 3-axis mills that fit what I was looking for any better, and 5-axis opens up some interesting opportunities.

I decided to go for it, and a month later DHL showed up with a heavy crate:

Out of the crate and on the bench.  The machine is deceptively heavy given how small it looks, and is very awkward to hold onto.  Rigol scope in the background for scale.  

Back side of the spindle visible:  It's a generic 800W ER-11 water cooled spindles.  Maybe something to upgrade in the future:

The three linear axes are driven by brushless servos with integrated controllers:

A peek under the bellows way covers at the (allegedly Hiwin) X-axis ballscrew and one of the linear guides:

The linear axis ballscrews are coupled to the servos with disc couplings, which is nice to see

The backside of the machine, where you can see the X,Y, and A axis servos.  The rotary axes are driven with harmonic drive reductions and supported by crossed roller bearings, which I'm surprised was possible given the cost.

When I unpacked the electronics box, a few screws had worked loose in shipping and were rattling around.  The inside of the electronics box was not confidence-inspiring.  There's a generic 36V DC supply to run the servos, a 1.5 kW VFD, and some pretty sketchy wiring.   The machine seems good mechanically, so I'm letting this slide for now....

I've been using the shipping crate it came in as an enclosure.  If I fold the door up it keeps the chips in and the noise down a little, at the cost of seeing what's going on.  Eventually I'll build a proper enclosure.  I set the crate on top of a Harbor Freight rolling tool cart, which stores the power supply box, water cooling, and related tools:

Screenshot of the the control software below.  The software isn't anything fancy, but does the job.  There are amusingly mis-translated buttons like "Knife", which actually runs the tool probing macro, "overrate", which is the feed override, and "Cold Fog", which presumably would turn on mist coolant if the machine had it.

Not particularly exciting, but here was my first working attempt at a multi-axis toolpath (video at 16x):

Here's one of the first "real" parts I've made - the front side of a motor housing.  Most of the material removal was done with a Datron 3mm single-flute end mill.  Thanks to the rotary table I could do this part in one setup, rather than machining one side, machining a fixture, and machining the other side like I would on a 3-axis machine.  Video at 8x speed.

Here's pretending the mill is a lathe and machining a shaft for said motor, including a lock ring thread cut with a 60 degree chamfer mill.  HSMWorks, which I've been using for CAM since the beginning, is pretty terrible for this style of toolpath, so the surface finish is a little weird.  It buffed out easily though.  In this picture the part is done and being parted off:

And here's that half-a-motor-housing and shaft with a rotor for a frameless motor installed (held on by a threaded lockring also made on the mill), and bearings and commutation encoder magnet pressed in.  

I haven't pushed the machine too hard yet, in the interest of keeping noise down.  It's in my 2nd floor living room, and not very well enclosed, so I've been making the toolpaths conservative to avoid complaints from my neighbors.

Amusing setup from today - a part in the tiny lathe 3-jaw chuck, held in an ER-40 collet chuck, bolted to the table.  Milling a circular dovetail in the part (which is a fixture for yet another part), to match the dovetails milled into the lathe chuck soft jaws:  No dovetail cutter required.

Summary of thoughts/impressions so far:
  • The core mechanical pieces of the machine seem pretty good.  Brushless servos, linear guides, ballscrews, and harmonic drives, on a steel structure is impressive at this price point.
  • The less-critical hardware is a little janky - the bellows way covers, the sheet metal spindle cover, the electronics box, the water cooling loop.  But those are all relatively straightforward to re-do or repair if needed.
  • With good tools (I've been having great luck with Datron single flute cutters for roughing), it performs pretty well cutting aluminum.  I've been roughing with a 3mm endmill at 20k RPM, 2.5mm stepover, .5mm stepdown, and 2000mm/min feed with no problem.  It could definitely be pushed harder but it gets loud.  I haven't tried harder materials yet.
  • I haven't done a ton of experimenting yet, but "conventional" style toolpaths with large stepover and small stepdown seem to perform better than "adaptive" or "trochoidal" style toolpaths with a large stepdown and small stepover.  Needs more testing though.
  • I wish I had a way to pre-set tool lengths with the ER-11 spindle.  The machine has a built-in tool probe, but swapping collets and probing takes a while.  I'm thinking about making a bunch of shrink-fit holders that all have the same shank diameter and bottom out in the spindle, so the collet and collet nut never have to come all the way off. 
  • There are a few vendors of the machine (It's even on Amazon, but also RobotDigg and a few other sites), but it's cheaper to get directly from Xinshan.  
  • Support has been really excellent so far.  I've had tons of questions about how things work, and I always get a response the next day.  When I've had g-code that behaves confusingly, they'll run the code on their machine and send me a video.
  • CAM-wise, I've been using HSMWorks.  I think the kids these days are using Fusion 360 (Autodesk bought HSMWorks and I think has ported it into Fusion), but I've never tried it.  Solidworks integration is super nice since your CAM updates when your model updates, and I don't really want to switch to Fusion for CAD.  HSMWorks/Fusion 4/5-axis toolpaths are kind of a joke, but 3+2 (position the rotary axes then do a 3-axis toolpath) work great.  The "real" answer for good 5-axis toolpaths is probably a more legit stand-alone CAM software, but I'm going to stick to HSMWorks for everything I can.  
  • Cool feature, the machine can do TCP, Tool Point Center control - this means that the CAM origin does not need to be at the machine origin (the intersection of the two rotary axes).  You can put the CAM origin wherever, set the work coordinate system offsets by touching off to the part, and the machine will figure out the kinematics.  This makes CAM much simpler, since you don't have to know where the part/stock are on the machine when you're doing the CAM.  That's what you'd expect for 3-axis stuff, but with the two rotary axes, it's not just an offset in X, Y and Z anymore.  I haven't been to adventurous with this, but offsetting the Z at least seem to work just fine. 


  1. Hey ben if you dont mind me asking, how much $ did you get this machine for?

  2. Interesting! Great machine and great showing!

  3. Duuuuude. This looks pretty amazing for the size. My woman would hate me even more than when I got a cheap CNC engraver in our apartment but this looks pretty justifiable considering what it does.

  4. Looks like a decent setup! Did you look into the Abdi Automation machine? Probably too heavy considering where you have to install it. I think an Abdi machine would be pretty neat, if you swapped the steppers for servos.

    1. I did - it's a bit heavy, and doesn't look very polished. I would sooner build my own machine (which I also considered) than buy the Abdi machine, I think

    2. I completely agree - I think the idea is good (epoxy granite frame, off the shelf spindle, linear rails + ballscrews), but everything downstream of the mechanical design is pretty rough (and no way covers???). It should really be sold as a kit.

  5. You are crazy (in a good way) :D

  6. Looks like a really interesting alternative to a PocketNC with bigger travels and a beefier spindle. Re: pre-setting ER11 collets, GenSwiss makes quick change ER collet adapters which can adapt an ER11 taper down to ER8. It basically fits like a baby CAT or BT toolholder, allowing you to set up tool tables, at the expense of extra runout/stickout/ER8 size collet

  7. Hi. Do you have files for post-processing in Fusion 360?

    I also have this machine, but I only have files for PowerMill, and I prefer Fusion 360.

    If you have these files, I would be very grateful for sharing them.

    I wish you all the best.

    1. Added a link to my HSMWorks post file at the end, which should also work in Fusion.

  8. Hi Ben, I have an identical machine that I bought from Robotdigg in August last year. I agree with all your points and that it is an excellent machine for the money you pay. I have a couple major complaints that you didn't touch on however. This is that the control software is Windows XP based and that they didn't have any drivers for later windows versions. I therefore had to go and find an old second hand laptop that can run windows XP. My other major problem is that the controller often loose connection with the machine which then stops in the middle of a job which then require new alignment since the Rotary and Z axis inevitably move a bit when turned off as the servos have not brakes. I am therefore currently installing a completely new stand alone 5 axis controller from Syntec to overcome this. I think the controller from Masso would also be compatible.

    1. 32 bit windows, not XP necessary (for my version at least). I'm running the control software on windows 8.1 32 bit.

      Haven't had connector issues yet, but time will tell.

      If you put up any documentation, I'd love to see how the conversion turns out!

    2. You could have run 32 bit windows on any new Windows machine. Just use Vmware.

  9. will do. I did not have as good experience with Robotdigg as you have had with Xinshan Tech in terms of support. My machine came with post processors for Fusion 360 and Powermill. The 360 post processor was not set properly up and made the mill crash so I had to go in and modify it to make things work. I see you are using a different CAM software. Where did you get the post processor for this?

    1. I'm using HSMWorks, which is basically identical to Fusion CAM. I had some tool-offset related issues with the Fusion post they provided, so I made a few modifications. There's a link to the post processor I've been using at the very end of the blog post.

  10. Thanks, I prefer to do my CAD in Solidworks but also have Fusion 360. I think it's time for me to drop the Fusion 360 and then get HSMWorks. Fusion 360 is very very poor in terms of Simultaneous 5 axis as most of the few functions that are available are charged at additional cost. I am also going to try and have a go with Powermill for the more complex parts to save some milling time. I will revert to you once I have finished the controller upgrade. For me it's an incremental progress improving one thing at the time. I have already improved the base plate with my own work holding attachment system with a standard system for all my work holders as shown in the link below. Following that I may have a go at improving some of the other mechanical bits such as incorporating a large bearing for the rotary to stabilize it further. https://www.youtube.com/watch?v=LAUFuG1OoyE

  11. is there a reason you didn't buy their enclosure and opted to build your own?

    1. I would have if I'd known about it when I'd ordered the machine. But shipping was going to be very expensive to get it separately when I looked into it later.

    2. Enclosure have one big problem. If you want to work on a flat part, you cannot see the job and cannot make some positioning by eyes. Without the enclosureyou can be behind the spindle and move the tool . Sometimesyou just have some drills and you just need to place the first hole , the others will be relative and mororised.

  12. did you purchase any work-holding from them?

  13. Hi Ben, Thanks for your experience sharing, I am hesitating between the pocket and this one, are you still satisfied ? Looking the specs of both machines, I have the impression the pocket is a bit more precise, at least on theory, I am wrong ? Robotdigg has now a v4 while xinshan stay with a v3.5 : any opinion on this ?

  14. How much did it cost to get thru customs?

  15. Hello Ben,
    My name is Dan, was great to find this blog. I ordered the V4 with enclosure about a month ago from Robotdigg, is still in the process of being shipped (I hope). I will let you know my impression once I get it. Happy Chipmaking...

    1. Hi,

      I would be interested in knowing your thoughts on the machine when you receive it. looking to make a purchase myself.

  16. Hey Ben just bought this machine just wondering how you actually run g code on this software

    i have code loaded, the machine connected, part zeroed and cycle start seams to have no effect

    1. The machine needs to be in "Auto" mode.

    2. Thanks Ben figured this out just 1 hour after comment.. i am also running the software in a 32 bit VM which seams to be working well

    3. What depth of cut are you able to take comfortably without compromising the material or cutters? Say with a 3mm end mill.

  17. Hi Ben, do you know of a CamWoks post process (or SolidworksCAM) for this machine (ctl file). Thanks

  18. Hi, I just got my machine, I ordered from Xinsham. The thing is built really well, the box with the enclosure was 100kg. They don't mention it but the enclosure comes with the coolant pump all plumbed in, the sump holds just over 2L, has a chip tray and another filter and led light array inside. The enclosure also holds the spindle coolant pump, radiator and fans as well. Have not figured out how to zero the A and C axis properly yet.

  19. Hi , thks for this blog . I go to buy it a few days. I use Solidworks and solidcam but I wil migrate to hsm. I really enjoy to be in a community or a forum . I will certainly have obscur situation and I will need help sometimes.
    Is it possible to share emails ? May be not usefull of robotdig have a serious hotlinr/support
    Thks for your job. Now i can buy .

  20. Hi,

    I also got this machine with a factory supplied enclosure model (v4), and when I received the machine first time .. as soon as fired up the provided software for controller interface I was very disappointed as the software looked so basic and lacked a lot of features and had full of bugs.

    Since I am a software developer by trade, I had to do something about this and after some months of work .. I have re-designed and developed a completely new controller interface for this machine.

    I am currently getting this software evaluated by few users, anyone interested in joining the evaluation of the beta release with a 30 day evaluation license are welcomed to send me an email at;


    Here is a link for a screenshot of the new interface : https://ibb.co/pzMFmsp

    Thank you!

  21. Dear All,

    New cnc interface is now in production, and already in use by many users.

    Currently interface provided with a specifically tuned PowerMill post processor, however Fusion 360 post processor is in development. Software also comes with Powermill machine simulation files to fully simulate 5-Axis cnc milling operations as if you were actually performing these on the actual machine.

    New interface supports many of the features that is not available with the vendor supplied software which is outdated and unfortunately very unstable.

    - Mid program manual tool changes
    - IJK / R Circular Interpolation
    - Helical Milling
    - 24k, 42k and 60k spindle support

    Please see below links for screenshot of the new interface and PowerMill simulation.


    Thank you for your support!


  22. Looks like screenshot links may not be working for some, please also try the following links for screenshots if the previous links are not working for you.


    Thank you!

  23. Thank Ben‘s comments and other users' support on our machine, now there are four versions for 5 axis DNC milling machine, V3.5/V3.5 with enclousre/V3.5 pro seperate/V3.5 pro complete, hope you can check and like it