How do I mill 260 brass?

[ecotectoo]

Hi - I'm pretty much a newbie at this having gotten my CNC router about a half year ago. I've learned to manage okay in wood and 353 brass... and now need to cut out some parts in 260 brass.

Specifically: .025" HH 260 brass sheet. I used the same settings I used with the HH353 .032" brass sheet: .0394" 2-flute carbide endmill at 24imp S20K. I also rub around some water-soluble oil on the material.

Where the 353 cut is mirror-smooth with no burs at all, the 260 broke my cutter in 1/4" of travel. I kept reducing the F&S down to 12imp and 12K amongst broken bits to finally get a part cut out - but it's incredibly ragged.

What's going on? What F&S are recommended for this? I can't seem to find anything on the web about it.

-- Richard --

[HuFlungDung]

Is the part securely held down?

The machining characteristic of brass that one needs to keep in mind, is the tendency to work harden, release, work harden, release, over and over again.

Initially, the workhardened skin is created by the tool itself. So the material resists cutting, and then the next edge comes around and since the feed has advanced the position of the material, the cutting pressure is now much higher than it was, and the material skin gives way and the edge penetrates the work, but the chipload is much higher than planned for. The positive cutting rake of the endmill provides a wedge effect that lifts the work onto the rake face of the tool (inside the flute). This is called 'hogging in'.

This creates poor cutting results, especially on thin sections.

The surefire method to eliminate the hogging in problem is to use a straight flute tool, with absolutely no honed edge (ie, sharp, not brushed or overcoated). Typically, you can grind a little bit of the endmill, just inside the flutes, creating a flat facet that changes the geometry of the flute right at the super acute cutting tips. All you need is a tiny flat zone, that is radially oriented and parallel with the tool axis.

This same trick works wonders for drills when drilling brass.

You will also want to use a stub length flute on the tool, when working with a tiny diameter like that, to keep the tool stiff enough to consistently take a chip with every revolution.

[ecotectoo]

Is the part securely held down?

I think so. The sheet is 9"x12" and has a continuous clamp bar down both long sides. As the part is cut out I use a couple of sticks to keep the sheet from bowing up.

The machining characteristic of brass that one needs to keep in mind, is the tendency to work harden, release, work harden, release, over and over again.

That's interesting as that might explain the type of roughness of cut I'm seeing though I assume that this hardening thing *doesn't* apply to 353 brass which cuts very easily and "cleanly"?

The surefire method to eliminate the hogging in problem is to use a straight flute tool

I can't seem to find any which are small enough. I'd like to get close to what I've been using: .040"

with absolutely no honed edge (ie, sharp, not brushed or overcoated).

I have absolutely no idea of what you mean. I'm not a machinist and I wouldn't know how to do any of that stuff to a cutter even if I knew what you're talking about.

You will also want to use a stub length flute on the tool

Yes, the cutter I'm using is a stub length. I'll try to attach a photo of what my part looks like.

-- Richard --

[Karl_T]

I think so. The sheet is 9"x12" and has a continuous clamp bar down both long sides. As the part is cut out I use a couple of sticks to keep the sheet from bowing up.

That's not clamped enough then. i suggest you "make a sandwich" That is have sacrifical material above and below your part. This holds a thin sheet well.

i also stone the edge of the endmill for a very short section of 0 rake angle when doing brass. This would be very easy to show, but I don't know how to describe it better.

[ecotectoo]

That's not clamped enough then. i suggest you "make a sandwich" That is have sacrifical material above and below your part. This holds a thin sheet well.

What could I use that would be thin enough so that my tiny cutters will still reach the brass?

i also stone the edge of the endmill for a very short section of 0 rake angle when doing brass.

I don't know what you mean by "stone" or "rake" (remember that I'm a total newbie to machining and CNC stuff).

-- Richard --

[thinkntink]

Hi Richard,

There might be an easier way (than honing a carbide end-mill) to get around the problem you are having.

First of all, even for thin sheets of material, you can often end of with a much better cut using multiple passes. Looking at the picture that you provided, it is clear that:

a. the part was chattering quite bit (giving you the rough edges shown)
b. you were conventionally cutting the part (the cutting edge going in the opposite direction as the cut). Climb milling is usually better for materials whose swarf tends to "weld back" behind the bit.

In this case, I would proceed as follows:

1. stabilize the part by super gluing it to a thick phenolic substrate (Masonite glued to a 3/4" piece of pine works great). You will need to use a catalyst to trigger the super glue. I like the Loctite® 7113™ Accelerator that seems to work with most cyanoacrylates or the accelerator sold at any Hobbytown USA. Apply adhesive to the back of the brass sheet (AFTER you have wiped it down with lacquer thinner). Press the brass down against the smooth side of the Masonite until some adhesive oozes out around the edges. Drip the accelerator around the edge. Hold for about 30 seconds for the accelerator to do its work.

2. mount the board to your CNC table.

3. tip off you tool (set the Z axis zero)

4. flood the brass with your water soluble cutting oil

5. set the cutting depth to 0.013", the speed to 21 KRPM (max on your router), and the feed rate to 24 IPM (faster is probably better but this is a good start)

6. set up your code to "climb mill" the part (going anti-clockwise around the part as seen from the top)

7. make some brass chips

8. put a bundle of money in a brown paper bag and send to Ron at Anytown, USA.

Please let us know how this works with the 260 brass.

best regards,
Ron Reed