Branding Iron

[Red (Unregistered Guest)]

Has anyone tried to mill their own branding iron from solid metal? If you have seen the electric heated branding irons. In particular for branding wood.

[bleeth]

Branding irons are either cast or forged. If you care to heat steel to melting point and pour it in a mold you can certainly use a cnc router for carving a master to create a sand mold from.

[Brady Watson]

Red,
If you can get the resolution that you need, you can mill your own branding iron/logo in brass. It would be very similar to the ones that Rockler sells.

-Brady

[stevem]

I believe the electric branding irons for wood are machined from brass. You should be able to get good results on a bot with the correct cutting bit and lube.

[Red (Unregistered Guest)]

Thanks for the replies. The design I had in mind is rather "simple", so I thought the bot would be able to handle it.

Any ideas on how "thick" the brass would need to be?

[gerald_d]

Red, how big is the pattern/logo? The thickness will vary according to the size of the "iron".

[cnc_works]

I've milled branding irons out of brass with no problems on my router. Fine details in small letters are limited by the size of the bit you use. I really don't remember feeds/speeds at this point, it has been awhile and I didn't take notes as I probably should have.

You can see a sample at www.cncworks.biz (http://www.cncworks.biz), click on engraving and it is the first image. Worked out OK, except I was having some problems with perfect repeatability in Z, so the background has some variance.

My problems came in maintaining appropriate pressure and temperature to make it work consistently. I think the attachment for the drill press would probably be the be the easiest to control.

Donn

[cnc_works]

By, the way, the size is about 1.5" X 2.5" or so.

Donn

[mnrite]

Donn,

I checked out your site, nice work. Is the gold and brass paint on the corian lids One Shot or something else?

Mike

[Red (Unregistered Guest)]

Donn:

How were you heating it?

Gerald:

In the range of 8 to 12 sq inches.

[cnc_works]

Mike, I use a product by Krylon available at hobby shops. Basically paint in a 1/2" diameter tube applied with a large felt tip. I have been very pleased with the color retention as some of my boxes are several years old and all the colors have retained their vibrancy, even the gold.

Red, down & dirty...a propane torch. Though I did acquire some old soldering irons with big heating elements that I was considering to use except I kind of lost focus on the project.

Donn

[wemme]

Donn, What software cad/cam do you use for you signs? Cheers.

[cnc_works]

Wemme, I own the Cimigraphi software. Kind of like ArtCam.

Donn

[kaaboom_99]

Hi guys. I am looking to make my own branding iron. I have a piece of brass 1.8x2.5x0.5"
I have a few questions.
What is a good height for the characters?
I have 1/16", 3/32" and 1/8" endmills chucked into a Makita router. Any suggestions for feeds and speeds?
How about lube, required and what type?
How much taken off per pass?
Thanks guys

[grant]

I have done some brass cutting, so I'll see if I can help. I did some cutting in solid brass a couple months ago, I made belt buckles as gifts for my groomsmen and a couple other folks. I used a 1/4" ballnose designed for wood, an engraving bit and a 1/8" O flute, designed for plastics and aluminum. All of them worked well. In my experience, when you run the shopbot really slow, it is about as smooth as anything out there. My delicate engraving bits required this, and I was rewarded with the results. I did all of my cutting dry, no lubricant of any kind. The chips that came off the cutter were VERY hot, but there was not even a hint of rewelding. It seems that brass is considerably more forgiving than acrylic or aluminum can be. I did use a cold gun, a pneumatic vortex tube chiller made by Exair corporation. I don't know how much difference it made, honestly, but since I had it I didn't see a reason not to use it. They aren't very expensive, $200 or so if you wanted to pick one up.

With the 1/4" ballnose, which is what I used for the 3d shaping of the top of the buckle, I cut a maximum of about .2" deep with a .02" stepover. The machine definitely had some resonance with that depth of cut and I don't know that pushing it too much deeper at a pass would have good results. I was comfortable trying that depth because I started my cut off of the material, as it made the first few passes the bit moved into the material laterally. Even though my cut depth was fairly aggressive, the small stepover kept the cutting load from becoming very high. I used a feedrate of 1.5"/second in X,Y and Z, and if I recollect my spindle speed was 9000 or so, giving me a chipload of approximately .005" with the 2 flute cutter.

With the 1/8" endmill, I used a cut depth of .06" and a feedrate of 1"/second with the spindle speed at about 10,000, giving me a chipload of .006". With this cutter, I didn't have far to go vertically and a lot of work done already, so my priorities were more along the lines of caution than ambition. This cutter was a single flute upspiral "Super O" made by Onsrud cutter. www.onsrud.com (http://www.onsrud.com) It did a fine job. They may have more specific advice for you on other cutters that might do as well or better, I was to some extent working with what I had on hand.

With the engraving tool, which looks like this: *
2378 I wanted to be extra careful. I actually used a stepdown of .08", which is deeper than the 1/8" tool I used, but the feedrate was at a snoozing .25"/second, the stepover at .004". If I recall, the spindle speed was something like 8000 rpm, which gave a very light chipload, just under .002".

I sourced my brass from McMaster Carr, an odds and ends supplier for industry and hobbyists. They may not be the cheapest for a large order, but they have a fabulous website, a range of offerings and they ship incredibly quickly. www.mcmaster.com (http://www.mcmaster.com)

Oh yes, a couple words of caution. Every chip that comes off the tool will be a tiny razor sharp knife. Don't even go near your machine without heavy gloves and glasses on, cleanup is best done with compressed air and a broom. Also, because the material is hard there will be considerably more vibration than while cutting wood. Make sure to fully tighten your collets (don't abuse them though), I either forgot to tighten it or didn't tighten it enough, the ballnose vibrated loose and hacked up the only bit of spare material I had (whew!)

I have attached some pictures of the results after light deburring with a file.

*
2379
*
2380
*
2381

Best regards,

Grant Bailey
ShopBot Tools Inc.

[Red (Unregistered Guest)]

Thanks Grant. The details and pics are great. The buckles look cool too. How thick was the brass?

Did you cut the perimeter with the shopbot? If so, I assume that was the last cut performed. How did you hold down the material for the perimeter cut?

Thanks,
Red

[kaaboom_99]

Hi Grant. The pix look great. I too had success with my venture into the brass engraving (though limited). For my setup I used a 1/8" endmill along with a standard 90 degree, 1/2" Vee bit. I went to a depth of 0.100" for our branding iron making my rough cuts at 0.010" per pass for both, step over (for the 1/8" 2 flute) was 0.050" and 0.010" (for the Freud Vee bit), cutting speeds at 8000 rpm @ 0.5" per sec for both bits. I held the 2x4x0.500" block down with wedge clamps. The end results were satisfactory, not super as I too had my collet come loose once. As well, my block got loose on me once (it actually tipped down on one end. Not sure why.) The font was a fine script style so my little incidents had a 'minor' effect on it. After finishing though I did try it out and it worked well enough. My thought now is to 'flycut' it clean and try another font. Finished prodect will also have to be relieved of some material in the back as it takes a lot of heat presently to get up to temp to make it usable.

[milver]

Brass melts at ~1650F. Anybody attempted
to melt the stuff, with maybe a MAPP torch, into
a prepared mold?