These fly cutters would fit in a ER20 collet; haven’t tried them. Question is whether your spindle can run slow enough - what’s your minimum RPM ?
I tired something similar but I think their max RPM at 5k, the minimum spindle RPM is 8k.
2 Likes
I’ve been able to run mine reliably at 800-1,200RPM for the edge finder, the VFD has a silly value for min RPM. Running at 2,000-2,500RPM for spot drilling it has lots of torque and seems quite happy.
My concern is the lack of balancing on a fly cutter, the Shapeoko just isn’t rigid or heavy enough to take those out of balance cutters or the heavy loads in an out of balance large radius cut. The single flute cutters are OK but they’re < 8mm diameter and balanced to run at 20,000RPM taking tiny cuts.
Ahh - So you should be able to see some significant motor currents when drilling at those low RPMs? Maybe another argument for those monster water cooled spindles?
Not much current, only running a teeny feed rate to avoid the rumble and more importantly the down-force from the HDZ can bend everything else really easily. I’ve got the 3, 4 and 5mm spot drills working really well at
2500RPM
30mm/min plunge
0.012mm / revolution
which with some isopropanol lubricant and a retract every 1mm gives a nice curly continuous chip and a clean hole.
800 RPM sounds more reasonable.
Let’s say the small fly cutter has its centre of mass 4 mm out of centerline, then at 1200 rpm that would mean 6g centrifugal acceleration. How much does that thing weigh? 150g maybe? Would be 9 N centrifugal force, rough estimate. That half-inch cutter discussed above will certainly generate way larger radial cutting force contributions than that…
Have wanted to try Sensorless Vector mode, but still haven’t got my spindle installed, I did try to enable it on the bench once but didn’t work out of the gate (I have a different VFD (than in the video) that offers the mode but with limited parameters).
I missed that - what was it?
I have a used Invertek ODE-3-220105-1F42, might try contacting their tech support. Might also try a different VFD if it comes to it.
It’s a “white label” VFD that is under some other brand names as well.
OK,
But won’t I have to run a feedrate based on a Shapeoko sized feed per tooth and thus grow a beard waiting for the bit to finish surfacing?
Looks like a nice VFD! It apparently has an input EMI filter and even an optional output filter. Are you sure your HF spindle can support the extra current/torque that vector mode could provide? Do you think you need or could use it?
I’ve been looking for some more ‘grown up’ cutters but have no experience using them and I’ve not had much luck figuring out which of them are balanced to run at VFD spindle sorts of RPMs.
There’s a few in the Korloy Alpha Mill range with 10, 11 and 12mm shafts;
https://www.cutwel.co.uk/milling-tools/indexable-milling/90-degree-indexable-milling-systems/alpha-mill-90-degree-indexable-milling-system/alpha-mill-90-degree-milling-bodies?od_upper_diameter_im=19226%2C19227%2C19228
Of which this looks like a candidate;
As it has more than one tooth (I suspect hillbilly cutters won’t be well balanced)
Any experience with these sorts of cutters?
You need to use a water-cooled spindle to go at a lower RPM. Air-cooled spindle have a min rpm so it can still be cooled sufficiently with air. I ran my watercooled spindle at 2.5K and it was still able to drill though def not a crazy about of torque.
Let me re-phrase ‘manufacturer recommended’ you can run a spindle at 10 rpm if you wanted. The torque drops right down at lower rpms making most of the larger surface mills not suitable for use on a shapeoko or any other desktop based cnc with high rpm spindle.
1 Like
Oh I see yeah. I was only able to drill with a low doc at RPM lower than 6000. I see some people drilling at 6000 prob for that reason too.
Oh and it also draws a crazy lot more current at lower RPM and even 14-16 AWG motor wires will start heating up a bit.
That looks way better than any VFD that comes included with the spindle. Sensorless Vector mode seems very interesting. EMI reduction would help the shapeoko a lot.
Certainly.
The question is then, what kind of facing is intended. If most of the material is gone but the face looks horrible after an aggressive roughing pass with, say, an 8mm 1-flute, then perhaps a fly cutter slowly peeling off 0.1 mm maybe just the thing because the finish can be nice. Provided that the machine is trammed to the micrometer (mine definitely is not).
If facing is about removing a fat slab as quickly as possible, then I absolutely agree that large-diameter tools need not be better if all we have is spindle speed and relatively fast feed capability, but neither much torque nor feed force.
FWIW I run a 10mm “face mill” at 10kRPM on the Nomad.
Whether that’s a good idea or not I’m not sure but it does work. I use it at suuuuper low DOC though.
This is where it gets interesting and the type of tool comes into play.
Here are three face mills I have lying around.
From right to left
- 60mm indexable face mill - turned down to fit in a spindle
- 19mm indexable face mill
- 30mm solid carbide face mill
The 60mm face mill will run in a shapeoko - but really really badly. It isn’t balance even at 100mm a min and 2000rpm a 2.2kw spindle doesn’t have the torque to make it useful. At 5000 rpm it’s max rated speed the vibrations are crazy. It is designed for a different type of machine. Yes it fits and will cut but it’s not a tool I would ever suggest anyone uses on a desktop mill
19mm indexable face mill - this is designed for HSM - it’s max rpm is 10,000 and it’s balanced, vibrations are noticeable at 12k rpm. It will chew through ali at 1mm doc 2k a min - however the atc spindle it runs on is 10kg and not suitable for a shapeoko (it also costs more than an XXL fully kitted out
30mm solid carbide face mill - this is a great bit of kit, it’s rated to 20,000 rpm, has 4 flutes and can leave a really shiny surface.
https://www.instagram.com/p/BvhUZcegxap/?utm_source=ig_web_button_share_sheet
The tool balance and max rpm make a huge difference. Personally my strategy with face mills is to hog material then a 0.2doc-0.1 finishing pass, however most of the time I will do this with a 8mm bit. Buying these large bits is ‘great’ but usually they don’t save much time unless you are running a project hundreds of times. The tool change time alone can take longer than the time saved by using one. Not to mention all tools above cost over $100. In order to get the most out of them the spindle also needs to be trammed. Note those terrible lines in the above insta pic - that’s bad tramming and on me.
3 Likes