Counterbore feeds and speeds

[PhoenixMetal]

I am using a counterbore tool for the first time and need to determine what feeds and speeds to use.

Specifically, should I do the calculations treating it as a drill, or should I treat it as an endmill? The two options give significantly different numbers:

Here's how the numbers work out given the workpiece and tool material:

Calculated as a drill bit:
0.4375" tool diameter
25 SFM
0.01" IPR
= Speed: 218 RPM, Feed: 2.18 IPM

Calculated as an endmill:
0.4375" tool diameter
3 Flutes
60 SFM
Chip load per tooth: 0.0025"
= Speed 524 RPM, Feed: 3.93 IPM (however since its plunging, I'd /2 = 1.965 IPM)

I really don't want to break a tool trying to experiment. Does anybody have experience with this?

Thanks in advance!

[kazikw]

Simple use 2000 rpm and feed 20. That should give you nice surface and tool will be not broken.

[PhoenixMetal]

Originally Posted by kazikw Simple use 2000 rpm and feed 20. That should give you nice surface and tool will be not broken.

Thanks Kazikw, but while that may not break the tool, those numbers have got to be way wrong. RPM is way way way too high and the feed is too low. Cutting at too fast SFM is wrong as each material has a specific speed that it can naturally be cut at. So if you run at too high RPMs, it will just wear out the tool prematurely. Also, cutting at too slow a feed will cause the tool to rub instead of cut, which also will wear out the tool prematurely.

Anybody else know whether counterbore speed/feed calculations should be handled as a drill or a plunging endmill?

[Glacern]

PhoenixMetal,

You should treat it like an endmill. Drills can plunge faster because of the tip angle, especially 118 degree drills, due to chip thinning.

You can also consider using circular interpolation in the future. You can use endmills that you likely already have and save a decent amount of time if you have a lot of holes to counterbore.

-Sol
Glacern Machine Tools

[PhoenixMetal]

Hey Sol - thanks for your reply!

I have always used circular interpolation in the past for this purpose, but found it to be very time consuming. I was also getting a lot of squealing of the endmills as they made their way through such tight helixes while plunging (I'm generally making small counterbores - for the heads of 1/4-20 socket head screws) which wasn't helping tool life. I imagine some further tweaking of the feeds/speeds could correct that problem though. So, with that in mind, I wanted to try a dedicated counterbore tool.

After lots of searching (and prior to your response), I finally found two pieces of information from very old books on google book search - which was giving drill-style numbers (SFM numbers similar to what would be used with a drill, and feeds in terms of IPR, not IPT) but with lower feedrates than what would typically be used with a drill.

I gave it a try and found it to be a pretty messy ride - feed too high relative to the speed, or perhaps something else. The spindle load meter was all over the place as the tool fought its way through.

I'll try your suggestion next with endmill-style numbers. The truth is the bottom cutting edges on the counterbore look a whole lot like an endmill anyhow.

I think I'll also try getting the correct size endmill and using it to plunge straight down. I wouldn't be surprised if that works better than a dedicated counterbore tool anyhow as the counterbores I've seen aren't the best designed products in my opinion. I think they're unnecessarily long (which allows more deflection), and the pilot in the center makes tool measurement a pain (you've got to account for the additional length in your CAM software).

BTW Sol, I happened to have checked out your website a few days ago (saw a banner ad on here). Your vises look really well designed, and man those videos are outstanding! The turning center videos - that's what I call factory porn!

[Mcgyver]

why a different SFM for a drill or end mill? the SFM is a theoretical optimization for a given cutting tool material and work material; doesn't matter if its lathe, mill, drill etc. rpm's for anything = 4xcutting speed/dia. Obviously setup and machine characters factor into whether you should actually use this theoretical number, but its the same theoretical number whether drill or mill.

Also, cutting at too slow a feed will cause the tool to rub instead of cut, which also will wear out the tool prematurely.

I dont think thats true, there is no penalty other than through put to cutting slower. cutting slower will improve tools wear. If you look at a graph of wear vs speed, its fairly linear up until the recomended cutting speed (thats what the cutitng speed, the theorectical max sfm before tool wear shoots up). There are many times when at a machines capacity it makes sense to lower rpm but maintain chip load as the best way to get the max removal rate and tool life.