drilling with endmills

So my team has been given access to a cnc shark hd4, and these WCP endmills
were recommended. Even though they are flat, can we still drill holes straight down with them even if we need to go a bit slower than a bit with a pointed tip?

Yes you can. When you “drill” with an endmill that is also known as plunging. You need to reduce feedrate quite a bit for it to work properly. Devin Castellucci from 1678 (RoboChair) would know more than me, but I find that 99% of the time I can use a helical ramp movement instead of a plunge. Plunging is not good for an endmill, typically.

ok sounds good. but to clarify you are using an endmill still and not changing the tool. So if I wanted to make some 3/16th holes, I would have to change the tool

No, you would be using a helical boring operation. Most CAM programs will allow you to do this, including Fusion 360 and HSMWorks. What diameter endmill did you get? The 4mm appears to be the most useful because it can bore any hole for a 10-32 tap and up.

We havent bought anything yet but we were planning on getting the 4mm. regarding the helical boring operation, that could be done with the 4mm endmill, right?

It can be done with any endmill. 4mm is just particularly good for FRC purposes.

Forgive me if I’m wrong as I don’t know a ton about machining but don’t you need a center cutting bit to plunge? From the pictures I can’t tell if the bit is center cutting or not.

Plunging with single flute endmils can get interesting at times, but it can most definitely be done. You just need to feed it slower than you would a 2 flute or a center cutting 4+ flute.

Yes you can plunge with those endmills, nowhere near as fast as with a split point drill bit however.

Helical boring is a fantastic way to be lazy if you hate doing toolchanges.

You can always drill your holes up to a larger size by hand afterwards(1678 does not drill larger than 0.191" on our router) without messing up your hole accuracy. Unless someone is TERRIBLE at using a hand drill…

Buy a cheap jacobs drill chuck from Shars.com and a shank of the right size and you can use any drill bit(only buy split point, trust me) in your router ~13k is good for #11 drill bits at ~15 IPM plunge to start.

Chuck $5.20
Shank $3.95 or there is a 3/8 shank they have for the same price.

1678 uses 4mm and 6mm primarily.

You can plunge with any endmill, but the helical boring operation is best.


N5001T5(3/8 2F HSS ENDMILL)

Now mind you, I used G41 which is my cutter compensation which allows me to make any size… D35 is for tool five in this example.

J is my radius desired.

This was in aluminium.

After I made countless holes within this piece, the next operation was to ridged tap, which is tapping the hole in a solid tool holder.

N601T6(3/4-16 RH TAP)

Note the G84… I am on a big Mazak so you will need to know if G84 ridged taps on your machine, and look a the feed rate: F.0625, that’s 1/16 or 16 in 1. You calculate feed like that ridged tapping.

Peace, and don’t be afraid to eat metal!

You can plunge with any endmill as long as it is center cutting. Not all endmills are!

The tool on the left will plunge, the tool on the right won’t (not very deep, anyway).

Yea, I didn’t mention this.

You can plunge as far as you want with that as long as you have enough spindle power and don’t care about using the endmill again.

This is not universally true. Fanuc standard is in inches per minute, unless you modify with a G95

And if you don’t care about the part not being bent (assuming its the 0.25" or less typical to FRC applications).

I’m going to add another caveat:

You can plunge with a non-center cutting endmill, provided that you first drill out the non-cutting area (or most of it) with a drill bit or center-cutting endmill.

In case you’re wondering… Yes, I have done that, on a benchtop mill. Needed a big hole and the big drill bit was giving problems. Enter big endmill and big-enough drill bit, and enough of a jig to get repeatability.