Torque curve for the Spindle on the HDM

Is there a torque curve somewhere for the 2.2kW 220V spindle on the HDM? It can help with getting the right speeds and feeds, I am planning on doing some HEM style of machining.

You’ll need to reach out to Carbide 3D support, I haven’t seen one published on the forum.

Spindles like these are basically always constant-torque though. If the spindle is 2.2kW at 24000 RPM, the torque will be 0.88Nm (a simple calculator will tell you this). That 0.88Nm will apply to the entire speed range of the spindle, though Carbide 3D specifies 8k RPM minimum, so I wouldn’t expect stable performance below that.

If you want to know for sure and Carbide 3D won’t Tell you help, have a look at the VFD settings. The VFD needs to be aware of the speed/torque curve because the current the VFD pushes into the spindle is what actually determines the torque.


Also since you mention finding feeds and speeds for HEM, you’re going to need to experiment anyway, so I’d just jump straight into it.

I’d recommend doing some test cuts:

  • Use the recommended chip load for the endmill, or if your manufacturer doesn’t provide one, find a similar endmill from a manufacturer that does and use that.
  • Start with as close to recommended surface speed as possible (probably max RPM) or use similar from another manufacturer once more.
  • Keep the above two parameters static throughout the entire test.
  • Use the manufacturer’s recommended radial depth of cut.
  • Start with a conservative axial depth of cut (e.g. 0.3mm).
  • Make test cuts, increasing the axial depth of cut until the endmill breaks, the spindle stalls or you encounter chatter.

I don’t think you will have a tq issue with that type of milling in the HDM. Ive pushed ours (1.5kw) to the VFD trip point many many…many times (for science). What I can tell you is that the machine likes 1/4" tooling and once you start to push hard with 3/8s and 1/2, the machine will let you know when it isn’t happy.

Power and machine rigidity is very balanced and I usually hit the limits of both around the same time. Usually around 1000 watts in the cut and around 3 cubic inches MRR in 6061 with good CAM is a good stopping point. Chipbreakers can sometimes add up to 30% btw

On my last HDM aluminum project that had massive MRR requirements (10lbs 6061), I found that more traditional style toolpaths actually meshed with the machine better and provided much better performance. Not as cool as swinging around a big DOC I know…but the reality of these style machines.


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