What's the right way to increase speed?

CNC Machines Shapeoko
1

I’ve been milling a lot of aluminum lately using the preset speeds in carbide create, and I’m fairly confident that my machine can handle a greater DOC or IPM or something.

Machine has: HDZ, saunders baseplate + rails, vfd spindle, mister, etc

My ape brain thinks I can just double the depth of cut and hope for the best, but I figured I should check in here to see if y’all had any thoughts on the matter. <3

2

I don’t know about doubling, but you can certainly incrementally increase DOC and see if the machine is still happy, leaving everything else unchanged. Watch out for chip evacuation, deeper cuts increase the risks of chip recutting.

Now IPM, if you want to increase it, increase the RPM by the same ratio to maintain the same chipload.

On a Shapeoko and with traditional (non adaptive) toolpaths, probably best to move faster than going deeper, as the machine is rigidity limited.

3 Likes
3

Awesome! I was hoping it would be that simple. I’ll do some experimenting and get back with the results. -Thank you.

4

I have a similar setup to you. Vince’s video really helped me a lot.

Like @Julien said, our machines are rigidity limited so making use of strategies that require less rigidity is key. That means adaptive tool paths (Fusion 360 can do these) for roughing. As a general rule, high stepover with a low DOC toolpath style will work best. Vince’s video goes over this. Another general rule is to keep your chipload above 0.001" or you can start smearing rather than cutting. This doesn’t apply in all situations but is true the vast majority of the time. I don’t know what speeds and feeds you currently run but if you are using the defaults from Carbide Create, there is lots of room to go faster. I would highly recommend learning Fusion 360 if you haven’t already. Carbide Create is great but will be a significant limitation if you are trying to maximize your speed in aluminum.

3 Likes
5

The approach I take on my (mutant) Nomad is:

  • Start with as close to the endmill manufacturer’s recommended feeds and speeds as possible. If the endmill manufacturer doesn’t provide recommendations, buy endmills from one that does or find recommendations for a similar endmill. In particular, pay attention to chipload.
  • Keep to 60-75% radial engagement.
  • Start with a shallow axial engagement like 0.2mm.
  • Do a few test cuts, increasing axial engagement one step at a time and see where the machine starts to struggle.
    • On our rigidity-limited machines, this means you encounter chatter.
    • So “struggle” means “sounds like something is being violently murdered” not just “sounds louder than usual”. The surface of the cut will also have visible marks.

If that isn’t enough:

  • Try a larger endmill. Larger means higher surface speed means reduced cutting force.
  • Try a higher flute-count. I usually use 3-4 flute 6mm endmills where I need high MRR.

And for some specific numbers, my usual roughing feeds and speeds are:

  • 3-flute endmill
  • 27k RPM
  • 2400mm/min feed
  • 0.9mm axial engagement
  • 2.4mm radial engagement

For finishing, I’ll use the same recipe but with 0.5mm axial, 0.5mm radial.

5 Likes
6

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