Drilling 1/4" Holes On 3HP Spindle

Any suggestions on drilling using a 3HP spindle? The lowest RPM I can get is 8000 and I’m using a Timberline Counterbore bit which has a recommend RPM of 3000. 8000 RPM causes quite a bit of heat and burn even when using the peck method.

Is there a type of bit that is better for drilling at higher speeds?

I would bore them with an 1/8" end mill. Although not as quick as drilling it does work with the speed range of a router spindle

Use a end mill smaller than the holes you want to drill then use a spiral drilling tool path.

First, I’ll say AVID does not recommend this, but you can slow down the spindle and drill. The reason they don’t is because the cooling fan is less effective, and they don’t want people trying to mill at those low rpm because the hp of the spindle at 1000rpm is only about 1/8 hp. However, if you are just drilling small (<1/2") holes, you shouldn’t have to worry about overheating or stalling. I have run mine fine at 500rpm, but as long as you are down to 1000-1500 rpm you should be able to drill without burning.

I upgraded to the 4hp spindle, but am using the VFD from the 3HP, so I can’t veryify if this is true, but I am told the VFD that comes with the 4hp spindle has a min rpm setting in the VFD, so that may keep folks with that drive from changing the min speed, but if you have the old VFD, you just change the min in Mach4.

That said, I really only do this if I need to go deep, or I have a need to drill a size that I don’t have an endmill for. If I’m doing something like a cribbage board or something, I will buy an endmil that is the right diameter because that will cut cleaner holes and not have to run so slow, and don’t have the deflection that twist bits have at lower rpms.

1 Like

Just realized this was your video, thanks for sharing. Changing the minimums in the Config and in the Machine.ini still did not allow me to go below 8000 RPM. I’m fairly sure I’ve got the old VFD.

Are we allowed to discuss how that is done on this forum?

You updated both of these?:




It was the second one, thank you!!

1 Like

I second smaller end mill spiral ramp. Using 1/8 upcut I have cut 100s if not 1000s of 5mm euro cabinet holes and many others.


I second smaller end mill spiral ramp. Using 1/8 upcut I have cut 100s if not 1000s of 5mm euro cabinet holes and many others.

As @Cliff suggests, this is a really great way to clear material extremly fast with a high speed router spindle. Sometimes I get lazy and just throw a drill that I’m willing to burn up into the spindle and abuse it, but taking a few extra minutes to program a deep/centered helical entry on a small carbide end-mill really is the better way to go.

When you say a couple minutes programming this, are you talking about programming it directly in Gcode, or are you talking about setting up the cut in CAM? I am a Vectric user, and the drilling toolpath is pretty limited, but now I am thinking maybe I could use the ramp function in the pocketing or profile toolpath and a full depth cut to fake it out to do the same thing.

@jjneeb yes the ramp spiral function in Vectric, I drill with it all the time, I only use drill pecking if I have to due to hole size and bit selection. PS any new laser updates on your site? I like your way of presenting engineering type approache to the videos.

1 Like


When you say a couple minutes programming this, are you talking about programming it directly in Gcode, or are you talking about setting up the cut in CAM?

Over here I am using a legacy CAD program that is reasonably ancient and does not support these functions without a LOT of setup steps for each hole. Instead, I had written a small program that one can drag-n-drop a G-Code file (describing a set of drill operations) it runs through that G-Code finds he moves from one drill point to another and at each point one it gnerates/inserts a helical interpolation specified by the user. I had written this program for thread milling both internal and external threads on the CNC mill, but found that it suits my needs for the router as well. The way I implemented it generates ‘huge’ output files, but the tools don’t seem to mind. :wink:

Below it is showing one roughing pass compared to one roughing and one finishing pass, where it is stepping out on the diameter a small amount during that skim pass.

This is how it looks when setup to helically interpolate 1&1/2in-4 ACME threads using a thread mill.

The program doesn’t care if it cutting threads or a hellical interpolation, it just dutifully generates the helical profile requested by the user… So I program it in CAD as if I were going to drill it and then, after a few extra steps, I wind up with G-Code for helical interpolation that I can hand off to the AVIDcnc router.

Thanks. Thats pretty cool. Now I just need to find an easier way to do that in Vectric.

So you just use a profile toolpath and set the max cut depth for tool to be deeper than the full depth that you are drilling, and make sure the ramp is longer than needed as well and then it forces the ramp in to be a continuous spiral and it only makes on round at the bottom then?

I have a couple laser videos to work on, but I’m waiting for a new laser I ordered to come in, and hopefully some SW updates in the ESS plugin in the future. I’ve been stuck on some non laser projects lately.

Jim, have you discovered much that you can do with the 4HP spindle that wouldn’t work as well on the 3HP? I’ve been considering that upgrade as well.
Regards, Rob

There was nothing I did that came close to loading down my 3hp spindle except planing off river tables with a 2.75 " bit. I mainly upgraded for that task, and it is definitely better. If you were going to do a lot of that, I would recommend the 8.8 hp spindle though.

So for most uses it’s not worth upgrading, the 3hp spindle was a good model. I’m also a tool junkie so I got it partially for something to play with :grin:

Use the inside profile cut and a spiral ramp. If the bit diameter is at least one half the size of the hole you want to cut you will come out with a perfectly sized hole. Good for holes greater than 1/8" diameter using a 1/8" bit. Smaller than that use a drill bit. On the high side there is no limit. If you use a bit diameter smaller than one half the size of the hole you will just have a plug left at the center of the cut. This is the best way to dial in the exact size of the hole by using the offset allowance in a trial and error process.

Sorry for the delay. Yes profile tool path cut inside vector and spiral ramp. Have to check but I think I set feed and plunge at 50 or 60 on 1/4 EM (always upcut) some where someone said feed and plunge should be matched for spiral drilling. Not sure that’s necessary since bit is always in plunge mode I have done it at 100 and 50 no problems in the past but now just set both to 60. 1/8EM I think I set at 30.