Better choice for drill bits with a desktop CNC machine?

[dbb-the-bruce]

I've been a little reluctant to post questions related to desktop CNC as most people here are oriented to much bigger and more powerful equipment. I've found it pretty hard to get good advice even on other CNC specific sites.

But this is a great group of people with a heck of a lot of combined experience (who won't laugh at my machine ) so here goes.

The machine is a Nomad 3 for those who might know of it. Spindle power is 130W (yes watts) spindle speed is 9K to 24K RPM.
Work area is 8X8X3 it is very solidly built for it's size and it is accurate with feed rates that are more than fast enough - I've never run into feed rate limitations.

It is a great machine for what I mostly want to do - small accurate parts. This is the latest version and the spindle power is almost double of my previous machine, also a Nomad. Stuff that was a struggle is now a breeze and it will easily handle working with steel that was a stretch before.

What I have learned is that with this type of machine, you are always working on the edge chip load (bite) and available power/torque. The machine works great at high spindle speeds and feed rates taking cuts that approach the minimum chip load.

Then comes the drilling.

Maximum bit size is .125
The new machine has a minimum spindle speed of 9000K.

I've been using a "standard" relatively cheep HSS bit 118 point, no chisel. Mostly because they wear out quickly and I can resharpen them easily. Tried carbide but found they snap too easily in this sort of setup.

The issue is that for the spindle speed I have to work with, the plunge rate needs to be pretty high for the bit to be cutting more than rubbing. However the spindle doesn't have the power to maintain a high enough plunge rate. So you have to do excessive and small pecking to have any success on a deep hole (.5 deep in steel).

working cut parameters:
12000 RPM
2.8 IPM plunge
0.00023 feed per rev at initial RPM 0.00011 per cutting edge(!)
0.10 depth in a single peck

Independently measured spindle speed bogs down and drops to ~7 or 8 K RPM at bottom of "peck" so drops by roughly half.

My question here is:
Are the drill geometries that will work better in this kind of situation? Remember that I'm stuck using very high RPMs and low torque, and the bits are small.

Looking specifically for possibly trying different type/style of bit.

-Dave

 

[Reddinr]

End-mill maybe? I noticed that the demo video showed plastic and aluminum as the raw materials. Steel might be a bit outside the capability of this machine due to rigidity issues.

 

[JimDawson]

You might try 135 degree split point cobalt bits. Tougher than HSS but more forgiving than carbide. Also check Amazon for circuit board drills. https://www.amazon.com/s?k=circuit+...circuit+board+drills,aps,134&ref=nb_sb_noss_1

 

[mattthemuppet2]

screw/ stub length black oxide coated 135deg cobalt drills would be my choice, plus some kind of air blast to clear off the chips so you're not recutting them in the hole. You can also get carbide tipped drills, but I'm not sure they're available that small.

 

[DavidR8]

Drilling with a high-speed CNC spindle is a challenge.
Winston Moy has a good video about the challeneges of drilling with CNC router.

 

[Karl_T]

drill mills are spendy but bet they would work very well for you. here's a 1/64" offer"

https://www.mscdirect.com/browse/tnpla/78715307?cid=ppc-google-Smart+Shopping+-MMR+Milling+-+NCA&mkwid=%7cdc&pcrid=572851640628&rd=k&product_id=78715307&gclid=CjwKCAjw6raYBhB7EiwABge5KvsWFmZxqgiXD3Xw5jSXlDvscr3Qg1sPIdwmehICUh18ljYCxCXCiBoCnDkQAvD_BwE&gclsrc=aw.ds#navid=2106253&refinements=Mill+Diameter+%28Inch%29%3A1%2F64

or a 1/8"

https://www.mscdirect.com/product/details/01319698

 

[Jimsehr]

I would try a hss parabolic 135 split point drill . The cobalt ones are thicker thru the middle and sometimes make it harder for chips to evacuate. It might be worth it to try hss and cobalt to see works better.

 

[Reddinr]

I just had a quick look at their website again. [Edit] The spindle is driven by a belt. If you have a lathe, you can make a set of step pulleys, or just reverse the pulleys having the small pulley on the motor and the large pulley on the spindle. You may need to space the spindle block out from the surface a bit to give you room. You could reduce the spindle speed quite a bit that way.
(And, you get more torque too.)

 

[dbb-the-bruce]

I'm going to do some more experimenting. Winston's video basically covers the issue I'm dealing with. Spindle speed is just too fast. The machine is plenty sturdy - at least I haven't noticed issues with it and drilling. It would all be the down force on the Z axis and would show up at higher plunge rates. Higher plunge rates just stall the spindle.

@Karl_T - I don't think a drill mill would make any difference as it's intended to drill in and then make lateral cuts. The drilling down would have the same issues as drill with similar geometry.

@Jimsehr - for the shallow .1 holes, I'm not having a recutting or chip build up issue. Also the spindle has a fan/disc snapped on it that does a remarkably good job at clearing chips. I found a parabolic screw length bit (expensive) but will give it a try.

I wonder if something like this might work better:

Half-Round Drill Bit

Putting together an order of stuff to try.

 

[dbb-the-bruce]

or just reverse the pulleys having the small pulley on the motor and the large pulley on the spindle.

I thought about that - A little nervous about messing with a brand new machine. I'll ask on their forum. I've also got the prior version Nomad 883 Pro. Was thinking that maybe I could put a lower speed higher torque (less accurate) spindle head on it. Like from a hand held battery powered drill.

It could be my drilling machine.