[travis_farmer]

as my father has renewed his interest in making wood projects with his new wood lathe, i thought it would be neat to make him a torch heated branding iron.
my limited research showed that it seems brass is a good material to use. but before i tried it on my machine, i wanted to know what i needed to know to make it work.
i have not designed the pattern for the branding iron yet, but here is my intentions. i planned on using a fairly fine bit (1/32", or so), and a scrap piece of brass from eBay. but i am unsure if brass requires coolant/lube. i have heard that it can be milled without any. my machine does not have provisions for coolant/lube, as i planned on milling just wood.

as i have not updated any pictures in my re-build thread, i will describe how my machine is configured at the moment.

Techno/Isel Gantry III (i think) base machine (about 48" X 48" X 5" working area), with a Makita RF1101 router. i do have a vacuum head installed for dust/swarf removal.

my best guess are to run the feed-rate pretty slow, and router at full RPM. the cuts will be pretty shallow (about 1/16" final depth).

as i do not have any CNC metal milling experience, i am seeking any tips and/or corrections to my plans.

I am pretty sure my limited research on google turned up some good tips, but i wanted to be sure.

~Travis

[ger21]

I would never run that Makita at full speed for anything you do on your machine.

I'd try about .005-.008 depth, feedrate around 10ipm, and maybe 15,000 rpm.
I've never cut brass, but have cut aluminum with a similar size bit.
Use a little WD40. Some brass will cut better than others, depending on the type. With a little WD40, it shouldn't be a problem.

[travis_farmer]

I would never run that Makita at full speed for anything you do on your machine.

call me dumb, but why?

I'd try about .005-.008 depth, feedrate around 10ipm, and maybe 15,000 rpm.

ok, thanks. i will try it.

Use a little WD40. Some brass will cut better than others, depending on the type. With a little WD40, it shouldn't be a problem.

ok, i will probably take the vacuum brush head off, just so it doesn't contaminate any future projects. i can just lay the end f the hose near the work-piece.

~Travis

[ger21]

You are not cutting fast enough to need 24,000 rpm. All that extra RPM is doing is creating heat, and reducing tool life.

I do most of my cutting between 10,000 and 15,000 RPM.

When cutting metal, just use a shopvac, and periodically clear the chips. With WD40, and a 1/32 bit, you won't have chips flying everywhere. It'll be more of a slurry of fine powdered brass and WD40

[Jim Dawson]

I have cut C260, half hard brass on both my router and mill, using 0.020 tip, 5° taper, HSS cutters. On the router I used 13,000 RPM, 10 IPM, 0.022 DOC. On the mill, same cutters, but used my high speed air spindle at about 35,000 RPM, 15 IPM, 0.022 DOC. For a lubricant, I used soy (cooking) oil, just brushed it on. The reason for the 0.022 DOC was I was cutting all the way through the brass sheet in one pass. Held the brass sheet down with double sided carpet tape to a MDF spoil board.

[travis_farmer]

You are not cutting fast enough to need 24,000 rpm. All that extra RPM is doing is creating heat, and reducing tool life.

ok, thank you. that makes perfect sense.

I do most of my cutting between 10,000 and 15,000 RPM.

When cutting metal, just use a shopvac, and periodically clear the chips. With WD40, and a 1/32 bit, you won't have chips flying everywhere. It'll be more of a slurry of fine powdered brass and WD40

ok, and thanks again for the tips.

and thank you Jim Dawson, as well.

~Travis

[wizard]

While everybody has already pointed this out, when machining metal it is more important to match spindle speeds with the feed rate. If not you get tool wear, heat build up and other issues. If the material works hardens that can lead to broken tools. Stainless in some forms is notorious for work hardening if the tool is allowed to rub.

With brass you machining difficulties will vary with the alloy used. Some brasses and brinze alloys can be extremely difficult to machine. So when buying your brass make sure it is a realtively free machining brass.

In any event back to machining. The goal is to have the right combination of feedrate and spindle RPM to give you the right chip load per tooth on the cutter. The problem here is what is the proper load per tooth. Frankly i dont know as i suspect you will need awfully small cutter for what amounts to being an engraving task. However the cutter manufacture should have some data online but im going to guess a half thousands per tooth.

The next issue is depth of cut. For larger cutters it is pretty common to vary depth of cit to match the horse power available. However in your case that will not work as you will have more power than you could ever use. Rought suggestions like half the cutter diameter might not work either. The reason being is that very small diameter cutters are weak. Again id refer to manufactures documentation here.

Oh by the way runout is extremely critical as cutter sizes decrease! Run out can effectively turn a four flute cutter into a one flute cutter. This means your feed rate calculations are worthless. At small sizes ecessive runout can lead to broken cutter.

Oh about feed rate, for engraving type applications you might not make the feed rate settings often. You will often be accelerating the tool. You still need proper values though for bulk removal areas.

In any event have fun and be conservative.