Brass Brand - Need Help

Pretty new to the CNC world so bear with me. I attempted this past weekend a few times to carve/mill a branding iron but the results were horrible. I have seen here on the forum some of the brass carving that has been done so I know that it’s possible. This is what I used:

  • Unmodified X-Carve with Dewalt 611 (speed #4)
  • 1” x 1” x 5” C360 Brass bar
  • 1/8” 2-flute fishtail upcut (roughing)
  • 1/8” 10 degree Tungsten V-bit (detail) the tips on these just snap off Link to Amazon

I believe that I may have a few competing issues here but would like to get some thought/recommendations from the community.

  1. Carve was way too deep
  2. Image detail is too fine for a 1” brand
  3. Incorrect bit(s)
  4. Feeds/speeds


I plan on ordering a different piece of brass (2” wide) to try again. A couple of questions that I have are…

  1. What thickness of brass should I get?
  2. What depth should it be carved?
  3. Bit recommendations?
  4. Anything else?

Any help would be GREATLY appreciated.

Hey Brian -

Try using a single flute bit instead of 2 flute, and try speeding up the feed rate a bit if your machine can handle it.

One big mistake that a LOT of people make when cutting metal is thinking that running slower is better. In fact, running too slow will lead to a lot of heat and premature bit failure. The 2 flute bit combined with the slow feed rate leads to the bit “rubbing” the material away instead of cutting it away. The flutes just aren’t getting enough bite of the material to work properly. When you run faster feed rate and fewer flutes, the flutes are able to get a good bite and use the sharp edge to shear off chips.

Here is a great image illustrating the point:

In the top image, the bit is getting a good bite, and using it’s geometry to cut and throw the chips away from the material.

The bit on bottom isn’t getting a good bite, so it rubs and generates excess heat, which leads to broken bits.

For what it’s worth, I have never had any success with the style of V bit that you posted for this type of work. I use traditional 60 degree V bits with good success in Brass. Counter-intuitively, the 60 degree bit will also be a better choice for the super fine details in your design because it will produce “less steep”, more durable walls for those thin lines.

  • Luke


Here are the results using these tips:


I think you’ve got a couple different issues going on here.

  1. run a facing pass on the brass to make sure its square to your machine with a 1/4 mill
  2. way too fast on the detail pass. For the detail, the fastest i could go was 5IPM feed and 3IPM plunge, .003DOC, or like you said, the tips would break.

I did a brand for a christmas present with a writeup here .

First iteration was aluminum, than brass.

I ended up using these bits

1 Like

@baaja - thank you for the information. What 1/4" end mill are you using to face your brass material?

@LukeWilson - Holy cow!! That is some beautiful work! When you say “Try a single flute bit…” are you recommending any single flute bit OR one specific for metal? The same question for the 60 degree V-bit (metal or will general wood one work). It is difficult to tell from the picture but how thick is the material and how deep did you go?

One last question, where did you get that little brass piece to screw/attach the brand?

For facing I used this

18IPM feed 9Plunge .008 DOC It probably could have been sped up.

Brian -

Everything there is shop made. I machined the brand, the brass adapter, and the small brass bolster at the end of the wooden handle on the X-Carve. The handle was made on my wood lathe. The threaded section is from an 8mm piece of stainless all thread.

I recommend using cheap single flute bits from Amazon. Here are the ones I generally use. I recommend using cheap bits because as you learn you will break them, regardless of if they are cheap or expensive. It’s a lot more fun to break a cheap bit than it is to break an expensive one. Once you get brass dialed in, you can jump up to an expensive bit.

The brand in the picture is from 1/4" brass. Total depth is 0.08". For the main clearing I used an 1/8" single flute bit @ 70IPM 0.008" DOC. This is probably too aggressive for a stock machine, but lowering the DOC should get you back in range. Try to keep the feed rate high.

For the finishing pass I used a 60 degree Amana RC-1148 because it’s what I had laying around. Any “spade style” 60 degree V bit would have worked. I ran it with essentially the same settings you have listed for detail pass.

  • Luke

Where do you all get the brass blanks … good source?

I just purchased one tonight off of Amazon. Did a search for 1/4” x 2” brass flat bar.

Thanks. I was using wrong search terms.

This store on Amazon generally has the best prices I’ve been able to find on small pieces of brass and aluminum.

Hey Brian,

I was in a pretty similar boat last year trying to make a brass brand. Check out this thread that documents my failures: Brass vs. 1/32" bits

@FredrickHousel - thank you for sharing your experience. I too was a bit (pun intended) ambitious with this project but quickly realized that there is many things that need to be taken into account before starting. As a wise man said once; If you’re not failing, you’re not learning.

@LukeWilson - that is the store that I ordered my original 1" x 1" piece from as well as the 1/4" x 2" piece I ordered yesterday. I’m going to attempt to design/cut a piece similar to your “brass adapter” in order to connect the brand itself but have a couple of questions for you.

Based on what I see in your pictures, I assume that the hole for the all thread does not go all the way through the adapter and into the brand, correct?

The holes for the two black screws go all the way through the adapter and into the brand; how deep into the brand did you drill/tap?

I do not have a drill press so do you think that I could drill those holes with the X-Carve? If so, any tips/tricks/recommendations?

The center hole on the adapter is tapped M8 to match the all thread. In the back of the brand, I machined 2 holes using the X-Carve to the pilot diameter for a 1/4-20 thread. Similar settings to above, maybe a hair more conservative to keep the heat down. Then I used a 1/4-20 bottoming tap to thread the machined holes. I believe they are around 0.4" deep (EDIT: 0.2" deep) - just be sure not to poke through the other side. The nut above the adapter plate is tightened against the plate, locking the thread in place.

Luke - thanks again for all the information. For the two holes in the back of the brand, can I assume that you meant 0.04" (not 0.4)?

That looks like the Ruger logo.

1 Like

Sorry, not sure what I was thinking. It should be 0.2" - basically most of the material thickness, but not enough to poke through

The resemblance is uncanny :wink:

What is the consensus on the router setting at 4? I would think turning it down to 1 would also help with the rubbing.

There are two main factors that govern RPM:

  • Chipload/chip thickness (slice per rev.)
  • Cutter speed (SFM), the speed of the cutter as it rotates

With small diameter tools (<1/16") the SFM value drop due to less diameter and RPM need to be bumped up. Same applies for true point V-bits where the center of the bit (tip) have a SFM approaching zero.

So on small diameter tools low RPM may cause more rubbing, so higher RPM may yield better result.

Thank you for the explanation.