Small cutter feeds

[Dave SParticipant @daves59043]

CNC work forces me to actually look at the feeds and speeds of a cutter, rather than just “going by feel” on my manual machine.

Ive been running some tool paths for the rackform cutter and the recommended feed for a 1mm ball nose endmill is in the 0.001 a 0.003 mm per tooth @24k rpm (used SGS / Kyocera tool calculator)

That seems insanely small  – like rubbing rather than cutting.

Thoughts?

Dave

[JasonBModerator @jasonb]

Once you start to get below 3mm dia the chip load starts to drop as the tool is not rigid enough to take larger cuts. To some extent the actual feed rate is not so bad if you can run the cutter at the recommended spindle speed

Those figures do seem a bit low, looking at my YG-1 catalogue 1mm ball nose are in the region of 0.008 in steel, speed 16,000rpm and feeds of 350mm/min with 0.2 for Ap and Ae assuming this is a finishing stepover like ramp or scallop.

They also give a “high speed” option where chipload is 0.026mm , spindle 25K so feed of 1300mm But Ae (stepover is only 0.05mm so really no difference in the amount of metal removed

[Julie AnnParticipant @julieann]

Here’s a 16DP bronze bevel gear being cut using a 1mm 2-flute ballnose cutter:

For all operations the cutter was running at 24000rpm and 350mm/min giving a chip load of 0.0073mm/tooth. This was the first time I’d used such a small cutter so I was being cautious with feeds. My choice of chip load was partly influenced by the fact that there is no point setting a chip load smaller than the step size on the CNC axes. The finished bevel gears:

Julie

[JasonBModerator @jasonb]

Julie, out of interest what sort of stepovers were you using as that can have quite a bearing on how loaded the cutter is as “chipload” is really the thickness of the chip but stepover also accounts for it’s width.

Smallest I have on video is a 1.5mm 3-flute flat ended. I’m limited to 5000rpm and with the feed of 100mm/min that works out at 0.0067mm chipload. a bit over the suggested 0.005 mm for cast iron but the ramp angle meant I was only seeing a maximum of 0.075mm depth so fed it a bit faster. Total depth 4mm

This is a 2mm 4-flute ball doing a 3D scallop path. Chipload 0.01mm, again 5000rpm in cast iron giving a feed of 200mm/min. Ap (Vertical would have been upto about 0.75mm after the adaptive and Ae (sideways stepover) 0.15mm.. If this had been a 4mm or 6mm cutter which is the size I tend to use more often then feed would be 4-500mm/min so 0.02-0.025mm chip load and a 0.25mm stepover

[JasonBModerator @jasonb]

The other thing to remember when using a ball ended cutter on 3D work is that on the near horizontal surfaces you will be cutting with the tip of the cutter which is not rotating very fast so it could be the calculator is taking that into account. It would be interesting to see what it gives for a 1mm flat ended cutter both side milling and also slotting.

 

This is a section from the YG catalogue, about half way down gives cutting details for the small ball nose cutters

[JasonB]

On JasonB Said:

Julie, out of interest what sort of stepovers were you using…

The bevel gear was milled in three stages, all using a 1mm ballnose cutter running at 24000rpm and 350mm/min; roughing, parallel pre-finishing and parallel finishing.

The roughing stage goes round the blank multiple times stepping down at each rotation. Toolpaths are parallel to the axis of rotation. Stepover and stepdown were both 0.3mm leaving stock of 0.15mm with a tolerance of ±0.05mm.

The parallel pre-finishing pass follows the profile of the bevel gear so there is no stepdown control. Pre-finishing removes the steps, especially in the root, left by roughing. Same stock and tolerance as roughing and a stepover of 0.1mm.

Parallel finishing brings the bevel gear to size and improves the surface finish. Essentially the same toolpath as pre-finishing, but 0 stock and tolerance of ±0.01mm with a stepover of 0.04mm.

Julie

[Charles LamontParticipant @charleslamont71117]

Those bevels are very impressive. How long did each one take to machine?

[Charles Lamont]

On Charles Lamont Said:

Those bevels are very impressive…..

Thank you! Quick answer is that each bevel gear took just over 3 hours to machine. With no tool changes one can just walk away and get on with something else.

Longer story is that I had previously made a couple of sets of larger (6DP) bevel gears for differentials. The majority of the time was spent in understanding the design of bevel gears and how to draw them in 3D CAD. The bevels are true bevel gears, so cannot be made on manual machinery. The bevels are drawn as 1DP gears, the last operation in CAD being to scale the part, for the bevels shown scale by 1/16.

The original 6DP bevels were machined using the top speed of my CNC mill main spindle, which is 5100rpm. When I started looking at the CAM for the 16DP bevels it was giving machining times of around 16 hours. I am patient, but not that patient! So I decided to add a high speed spindle to the CNC mill. After looking around I did a deal with Ketan at Arc and bought their high speed spindle demo unit. Arc were discontinuing the spindles due to, I think, low demand.

Julie

[JasonBModerator @jasonb]

Thanks for the detailed reply Julie. Quite a reasonable cut on the roughing path considering the diameter of the cutter, then as you say just knocking off the tops of the crests with subsequent paths.

I don’t tend to use parallel that much as most of what I seem to do has surfaces that go from flat to vertical so the steps become excessive as I get towards vertical, so mostly use scallop which steps along the surface no matter what angle. Though I did use parallel a couple of times on the current MTB engine where some of the curved surfaces were reasonably flat and not compound.

The high speed spindle certainly comes into its own with these fine stepover cuts with small tools. With a 2-flute cutter I would have taken 5 times as long, at least the 4-flute balls I use half that.

[Dave SParticipant @daves59043]

Kyocera / SGS have an online calculator for their tools.

This is the ball nose one:

And this is the equivalent square ended one.

 

Seems they have quite conservative parameters compared to YG?

My spindle is also one of the Arc high speed ones – the ER16 version from 2013.

On the plus side I have managed to cut the tool without breakage this time.

Tool paths are:

Adaptive Clear with 6mm – to remove the bulk of the material

Contour with 6mm – to run along the cutting edge

Parallel (along the ‘troughs’) with a 3mm ball nose – to remove a chunk before getting down to smaller cutters

Parallel with the 1mm ball nose

Parallel with the 20 degree 0.2mm tip V

then Project with the 20 degree tool with follows the side walls to final clean up.

Would need hardening and polishing if this was the real one, but that’s fairly straightforward.

Need to figure out the indexing – a collet block would be ideal, but of course I down have one…

Dave

[Author]

Posts