.png){kind=spacer}
How to Make Your Own Brass Branding Iron on a CNC Machine
- Jan 16, 2024
- 5 min read
Updated: Mar 9
A brass branding iron is one of those things most CNC woodworkers either have or wish they had. The problem? They can get pretty pricey.
But if you’ve got a CNC machine, all you really need is a small piece of brass, the right bits, and a bit of patience.
In this guide, we’ll walk through the entire process of designing, tool-pathing, and machining a custom brass branding iron on a 1nfinity CNC.
What You’ll Need
Material
• A piece of brass – 3/4″ thick, 2″ wide, cut to roughly 6″ long (you can trim excess later)
Bits
• 2-1/2″ diameter flattening bit (for surfacing)
• 1/8″ O-flute upcut bit (primary waste clearing)
• 1/16″ O-flute upcut bit (fine detail clearing)
• 60° V-bit (engraving fine details)
• 1/4″ O-flute upcut bit (post hole on the back)
Other Supplies
• Painter’s tape and CA glue (work holding)
• Hot glue (optional extra security around the edges)
• 1/2″ diameter machine screw and matching tap
• Touch probe for zeroing
• A heat source (stovetop, torch, etc.)
Step 1: Setting Up the Design
Open your design software (Vcarve was used here) and import your logo by dragging and dropping it in. Scale it down to fit your brass blank, centre it on the material, and join any open vectors.
A branding iron works like a stamp, so you must mirror your design. If you skip this step, the burnt image will come out backwards.
Once mirrored, set up your material dimensions in the software to match your brass blank.
Step 2: Flattening the Brass
Before cutting any detail, flatten the top surface of the brass to make sure it’s perfectly parallel with the Z-axis.
This step matters for two reasons:
First, even slight variation on the surface means the design won’t even make contact when you brand, resulting in a patchy image. Second, the fine details in most logos require a truly flat engraving surface – any inconsistency and those details will be lost.
Using a 2-1/2″ flattening bit, one or two passes along the X-axis should do the job. You can jog the machine manually for this. The result should be a beautiful mirror finish on the brass.
Step 3: Tool-Pathing the Design
Here’s where the real work happens. Remember: you’re not engraving the logo itself. You’re engraving the space around the logo so that the design stands proud as a raised surface. The negative space gets recessed by about 1/8″.
Pass 1 – Rough Clearing (1/8″ O-Flute Upcut)
Draw a rectangle around the outside edge of the material in your software, then set up a pocket toolpath to remove the waste around the lockup. Recommended settings for brass: spindle speed at 18,000 RPM, feed rate of 20 inches per minute, and a depth of just 0.015″ per pass. That sounds conservative, but the density of brass and the geometry of the bit demand it.
Pass 2 – Interior Clearing (1/8″ O-Flute Upcut)
Run a second pocket tool path with the same bit and settings to clear the negative space inside the logo – all the gaps within the design itself.
Pass 3 – Fine Detail Clearing (1/16″ O-Flute Upcut)
After the 1/8″ bit has done the heavy lifting, you’ll notice some tight corners it couldn’t reach. Switch to a 1/16″ O-flute upcut bit and run another pocket toolpath over the same area. Take your time with this one – it’s a tiny bit, so keep passing light and feed rates slow to avoid snapping it.
Pass 4 – Engraving (60° V-Bit)
The final tool path on the design side is an engraving pass to capture all the sharp corners and fine details that the pocket bits missed.
Run a 60° V-bit at 16,000 RPM with a feed rate of 40 inches per minute. This pass goes quickly since it’s only hitting the remaining tight spots.
Step 4: Milling the Post Hole
You’re obviously not going to handle a red-hot branding iron with your bare hands, so you’ll need a way to attach it to a handle or post. Flip the brass over and mill a hole slightly smaller than 1/2″ in diameter so it can be tapped for a 1/2″ machine screw.
Using a 1/4″ O-flute upcut bit, cut a pocket 0.453″ in diameter and 3/8″ deep. That 0.453″ figure might seem oddly specific, but it’s the correct tap drill size for a 1/2″ thread. Settings: 80 inches per minute feed rate, 12,000 RPM spindle speed, with a depth of 0.013″ per pass.
Once milled, use a 1/2″ tap to thread the hole.
You can then thread in a machine screw with the head chopped off using a grinder – this gives you a post you can chuck into a drill press or plunge router collet for applying nice, even pressure when branding.
Step 5: Running the Job on the CNC Machine
Secure the brass blank to your waste board using painter’s tape and CA glue, with a bit of hot glue around the edges for extra safety. Then use your touch probe to zero X, Y (bottom-left corner), and Z.
Run the tool paths in order:
1. Load and run the 1/8″ rough clearing pass. Probe Z for the new bit.
2. Switch to the 1/16″ bit, re-probe Z, and run the fine detail clearing pass. This one takes a while due to the conservative settings.
3. Install the 60° V-bit, probe Z, and run the engraving pass. This goes quickly.
4. Flip the piece, switch to the 1/4″ O-flute, probe Z, and cut the post hole. Then tap the hole by hand.
Step 6: Heating and Branding
With the machining done and the post screwed in, all that’s left is to heat it up. A stovetop, torch, or dedicated heating element will work. Once the brass is hot enough, press it firmly and evenly into your wood for a clean brand.
Using a drill press or plunge router to apply the brand helps keep everything straight and applies even pressure, especially helpful if you don’t have the steadiest hands
Final Thoughts
This project might seem intimidating at first, but it’s honestly not that hard. Just like anything else on the CNC, the key is getting your feeds and speeds dialled in, using proper work holding, and choosing the right bits for the job.
Do that, and it’s a walk in the park. The end result is a professional-quality branding iron made on your own machine, for just the cost of a small piece of brass. Not bad for an afternoon’s work.
Download the free files from the user forum and make your mark in style!
Bits & Bits 1/8" O-flute upcut bit - https://bitsbits.com/product/425-up125/ - Full Depth: .125" - .015” per pass - 200 IPM - Spindle speed: 18,000 RPM
Bits & Bits 1/16" O-flute upcut bit - https://bitsbits.com/product/425-up062/ - Full Depth: .125” - .015” per pass -160 IPM - Spindle speed: 18,000 RPM
Bits & Bits 60 degree V-bit: https://bitsbits.com/product/60-degre… - Max Depth: .125” - .0312” per pass - 40 IPM - Spindle speed: 20,000 RPM
