My nomad 3 is working well except for drilling 6061-T6511 aluminum…it was a nightmare. Shallow spot drill squawked like crazy. Drilling #10 hole with 135 sp cobalt stub drill was worse. Light feed .002 and full peck didn’t work. I think the spindle is running way to fast for drilling, but haven’t got an answer from Carbide on minimum spindle RPM and Fusion 360 library has it at 10000. I back it off to 5000 but don’t know what its really running at.
I don’t see an open query from you on support.
Which drills are you sourcing which can be safely spun at the speeds the Nomad spindle turns at?
The Nomad spindle is rated at speeds of:
- Spindle RPM: 9000 - 24000 RPM
so you need to source tooling which works at those speeds — one example is:
https://www.harveytool.com/products/specialty-profiles/drillend-mills
Usually folks just use a smaller endmill and cut as a pocket — a coated, and if possible single flute tool should work well for that, see the #MaterialMonday videos at:
To “drill” on my Shapeoko Pro using Fusion 360, I use “Bore” operations. You mentioned Fusion, so I’ll assume that’s what you’re using.
I think a #10 hole is around 3.5mm. For holes between 3 and 3.7mm, I Bore with a 2mm end mill (these are just cheapo uxcell end mills from amazon) with a pitch of 0.25mm, a cutting feedrate of 60mm/min and a plunge feedrate of 40mm/min. I follow up with a second Bore operation with the same end mill to clean up the hole. The second bore operation is identical except I use a pitch of 2mm so it takes little time to clean up the hole. This is all done with an air blast but I doubt that makes much difference. I don’t use any other coolant with this recipe.
I feel comfortable to about 1/4" in depth. After that, I worry about deflection causing the end mill to bind and break.
These are not fast holes, but I would rather take my time than ruin a job by embedding an end mill in a failed hole. I think it takes around 2 min for 1/4" deep hole.
1 Like
Thanks for answering the spindle question. I called support on this but never got answer. So when I set rpms in fusion 360 under 9000 the machine runs at 9000 correct?
Thanks, most helpful. I have #29, #10 and .272 holes 3/8 deep. Harvy has some drill/mill tools I might try but in meantime I think I will predrill on my Sherline. The machining operations on the Nomad have been great so far, just drilling is problem.
A friend of mine has a Sherline that he bought new and never used. I have tried to get him to sell it to me but he wants to keep it. I would really use the mill but that is the way the cookie crumbles. The one he has would need to run on Mach3 with a parallel port from a PC. How does yours interface?
Necessity is the mother of invention.
Mine’s conventional with DRO. Amazing machine for its size.
No, the machine should turn at the requested speed, but it doesn’t have sufficient torque below 9,000 to actually make a cut.
I had backed off to 5000 RPM. Could definitely been the reason for the chatter and motor stalling. I think I will try the Harvey tools you suggested and try again. I’m definitely not familiar with these high RPM’s.
I don’t have any experience with Nomad, so take everything I have to say about drilling aluminum on a desktop cnc with a grain of salt.
I tried drilling on the shapeoko w/24k rpm spindle and had some success using micro pcb drills. The biggest drill I was able to use is 4mm at around 10k rpm, everything above 4mm was snapping immediately. Also, regular long drills didn’t work for me at all. Tool runout always seemed excessive and couldn’t fix that. The deepest holes I could drill were around 1/2in (the length of a pcb drill flutes), deeper than that and chatter was killing the drills.
These are the drills that worked great.
Spindle seemed to loose power very quickly below 8k rpm so I’m not sure how well will that work on Nomad.
The issue with drilling on Nomad and Shapeoko is the routers run too fast for a typical drill. If you have a spindle and not a router you can run at a lower rpm and drill.
Drill bits are not designed to be run at high speed.
Here is an example of a google search about drilling aluminum with a 1/4" drill bit.
What speed should I drill aluminum?
200-300
Recommended Speeds for Standard Materials with H.S.S. Drills
| Material | Recommended Speed (SFM) |
|---|---|
| Aluminum and its Alloys | 200-300 |
| Brass and Bronze (Ordinary) | 150-300 |
| Bronze (High Tensile) | 70-150 |
| Die Casting (Zinc Base) | 300-400 |
A router cannot run that slow 70-400 rpm and if you try to drill at 16,000 RPM you will likely overheat your drill bit and it will lose temper. They do make some drills that are specifically for cnc machine that turn at a higher rpm than a drill press. Look for those to see if any are rated for your minimal router/spindle speed.
Some like Toolstoday, Drillman and ebay.com as well as Amazon.
1 Like
This topic was automatically closed after 30 days. New replies are no longer allowed.