Cutting Chamfers with Flat End Mills

[mayu]

Hello eM,

When tool stations and holders are limited, we have to get crafty with our resources.

This is a common challenge with live tooling on CNC lathes.

The milling heads are expensive, and when there are alot of them in a machine it causes clearance issues.

The case in point is a tapped hole on the OD of a part with a c-axis lathe.

The conventional approach would be to spot face, spot drill, drill, and tap - but that would occupy 4 tooling stations, and possibly get in the way of other tools.

However in theory we can spot face, drill, interpolate, and create the chamfer on a hole with just a flat end mill.

Can anyone offer some advice for creating chamfers on holes with flat end mills?

So far, as shown below, the 'Wireframe > Curve Flowline' feature seems to do the trick. It creates wireframes on 3D solids, which can then be chained, but it is slightly cumbersome when it comes to actually chaining the toolpath.

Any advice would be highly appreciated.

Thank you

 

 

[AHarrison1]

Why not look at drilling and chamfer in one?

For example,

https://www.walter-tools.com/en-us/tools/standard_products/holemaking/overview/drilling/xtratec-d4580/Pages/default.aspx

[mayu]

2 hours ago, AHarrison1 said:

Why not look at drilling and chamfer in one?

We looked at these drills in the past and they are absolutely useful for many applications.

The main concern is the spot face - we are working on the OD of a part and feel that the spot face is important.

Perhaps the Xtratec-4580 combo drills are compatible with flat end mills?

I'll have our tool guy look into it and post an update once I get some feedback.

Meanwhile, using an end mill to do everything is still a potentially high value trick - not just on the lathe but on mills too because you can reduce the number of tools in a setup.

[AHarrison1]

46 minutes ago, mayu said:

We looked at these drills in the past and they are absolutely useful for many applications.

The main concern is the spot face - we are working on the OD of a part and feel that the spot face is important.

Perhaps the Xtratec-4580 combo drills are compatible with flat end mills?

I'll have our tool guy look into it and post an update once I get some feedback.

Meanwhile, using an end mill to do everything is still a potentially high value trick - not just on the lathe but on mills too because you can reduce the number of tools in a setup.

It really does depend on the application. The only time I've come across a spot-face (chamfer) being important was for sealing off against an o-ring

for high pressure  hydraulics, and even then it was more the surface finish that was critical.

If this is just to chamfer a tapped hole, the quicker the better especially for production purposes.

[mayu]

On the OD of a part it seems like the drill would deflect as it engages, and cause the drill to walk. This is concerning because there are some tight true position call-outs on the bolt circle in relation to the centerline. Creating a spot face just gives the drill a flat surface to start with.

Although a nice stubby drill with light pecks might not walk.

 

[AHarrison1]

26 minutes ago, mayu said:

On the OD of a part it seems like the drill would deflect as it engages, and cause the drill to walk. This is concerning because there are some tight true position call-outs on the bolt circle in relation to the centerline. Creating a spot face just gives the drill a flat surface to start with.

Although a nice stubby drill with light pecks might not walk.

 

A carbide drill with a drill length of 3xD and a peck of at least 1xD will work just fine. I have never had drill wonder on me while drilling OD.

[nickbe10]

11 hours ago, mayu said:

Any advice would be highly appreciated.

Mikron (and Sphinx) are some of the best drills for difficult situations. Up to 9 diameters you don't need a flat or a spot drill even on a tube as long as you are not too far off center, for off center they have the crazy drill cross pilot.

We do wirelock holes across the corners on hexes, Mikron crazy drill cross pilot will pilot on almost any slope or radius (the video on the website is outrageous) followed by a 12D drill using a deep hole drill cycle and done. We do this on wire lock holes from 0.047 - .090 in 15-5. They do chamfer/drills too.

If we are drilling right through the tube in aluminum we use Guhring 5518 series, no need for a flat or spot drill here either. Limited diameter range though.

[mayu]

27 minutes ago, nickbe10 said:

Mikron (and Sphinx) are some of the best drills for difficult situations.

Thanks for sharing your knowledge.

 I’ll definitely check those out. 

[crazy^millman]

Excellent advise given above nothing to add about the suggestions it was covered very well by both of them.

One thing is get rid of the flat endmill and use a bull endmill. You get a much better surface finish on that chamfer using a bull verses a flat endmill. The edge will break down over time, so by using a bull you get better tool life and also get a better finish win win. 

[mayu]

1 hour ago, crazy^millman said:

One thing is get rid of the flat endmill and use a bull endmill. You get a much better surface finish on that chamfer using a bull verses a flat endmill. The edge will break down over time, so by using a bull you get better tool life and also get a better finish win win. 

Excellent points.

Yeah I'll go with a flat end mill that has a minimum .01R.

For the sake of time I'll stick with 'Curve Flowline' for now.

I was able to create one toolpath and copy it to the other holes.