What bits to use to engrave on brass?

I’ve had a request to use my X-carve to engrave a personal signature on a .5" wide by 3" long by .25" thick piece of brass. The requester wants to use the finished piece as a brand to burn his signature into wood items he hand-carves. Thing is, I’ve never used my X-carve to cut brass so I’m not sure what bits to use; or even if cutting such a very fine/thin raised signature into such a small brass bar is possible.

Suggestions and advice please?

Brass is actually a fairly nice material to carve in, these bits I have added a pic of are typical.
The feed&speed depend on the rigidity of your system and may vary.

I dont have an Xcarve so can’t comment further :thinking:

(brand name is irrelevant, it is the shape I am highlighting)

1 Like

I will note that the rounded V bits are very nice for metal work — but for best results, if one can’t enter the rounded tip into the CAM program, one needs to either use a feeler gauge to make up for the difference in length, or some other technique to account for it for best results.

1 Like

Hello - I do a LOT of this and use very, very cheap engraving bits like these:


My X-Carve is heavily modified and I use V-Carve Pro. But if you want to use easel, it may work to make your letters fatter than the original to make up for the 30 degree angle. If you HAVE V-carve then, you are all set!

For an UN-modified X-Carve, I would start with .002 Dept of cut and go .01" deep. Test it to see if gives you an ok brand. If not you may have to go deeper. V-Carve enables you to use a larger bit to clear material which is helpful and also accounts for the angle of the bit. Here is the reverse of what you are talking about but look inside of the M for raised detail. This was only cut .006" deep. I think for a brand, you would have to go deeper.


We do branding irons at work and the design depth is usually around 3-4mm (1/8")

When you say your X-carve is “heavily modified”, what sort of modifications have you done that would have some impact on how it carves brass?

I have a 1000mm X-carve that I’ve made some modifications to. They consist of pretty much all of the modifications and upgrades sold by Inventables.

I do have V-Carve Pro. So that is no problem.

Maybe you would share an appropriate V-carve file so I could study and learn from it about cutting brass?

I have some of the 20 degree engraving bits from Inventables. Are those sufficient and appropriate for cutting brass? Or would I be better off ordering the titanium-coated bits you recommended from Amazon?

1 Like

My X-carve is a smaller custom sized unit. The rails are integrated into the base, the x-axis is solid, I use a custom Z axis with a balls screw and a Makita router. It is driven by a Gecko G540 48volts. It is very, very rigid. I mill a pocket in MDF before the carve to true the wasteboard to the brass work piece. Still, I break the engravings into separate small pieces and re-zero the z-axis before each one for consistency of depth across the entire piece.

Engraving Details:
The 20 degree should be fine - but more likely to break. 30 degree bits are a little more robust. I use coated and uncoated - whatever is cheapest - I have not noticed a difference in performance. I set my bit to .003" tip diameter and .003" depth per pass (80% stepover) at 40 inches per minute and 30 inches per minute on the plunge. Then, if it is going well, I manually increase the speed during the cut (I use Mach 3 CAM). I also use flood coolant, which is not necessary but extends the life of the bit and provides cleaner pockets.

Milling Details:
I prefer to profile the pieces use .25" four flute bits at .01" Doc 40 IPM, if the shape allows. Bits last longer, cuts faster and deeper, etc. Otherwise, .125" two flute at .005" Doc 40 ipm. For holes, I pocket the hole rather than drilling to provide breathing room. I do not profile greater than .25" thick material with a .125" bit.

Hope that helps. Here is an old photo of the base of my smaller, rigid x-carve. The plates have all been swapped to .25" thick aluminum plates with extra wheels.2a13b0aacd5c8180b4c279beeb78fb8b834a0235_1_689x390


Here is a better shot.


This is a great post. Thanks for your info earwigger. I have some further questions.

I pocketed the hole to make sure it was true. But with the bits you recommend I get a pretty rough outcome. Is it that the 1000mm xcarve cannot do cursive like this without stair stepping at this size? the plaque is 12mm x 64mm.

Here are my settings:

How do you polish the item after? I used steel wool, do you have like a rotary buffer or dremel? Your results look much better than mine!

One thing, I had to make the text ‘bold’ in order for aspire/vcarve to carve single lines, when calculating the toolpaths for cursive, it just skipped single lines, why wouldn’t it at least make one line? Is there a setting for that?

I do suspect your 40ipm is a little too fast for your machine.

Yah, something doesn’t look right. It looks like maybe your z zero was set too deep? Also, the engraving bit should not make those marks in the bottom. I go .08mm deep and it works perfectly. I would tighten everything up, add bracing, and make sure your z 0 is set to the surface of the piece.

I use these guys in the keyless chuck in a Dremel:


I also use C360 Free Machining Brass. Here is a guide to brass below. Though I have engraved in all kinds and get great results.


1 Like

Yeah, I am engraving to 0.15mm almost double what you do, I will try 0.08 tonight and post results, thanks for all your help!

I got some better results. How do you keep it down? I was using 3m double sided tape, but it moves around a little like on jelly, that’s probably the last thing I will work out.

I am buying those polishing discs, some filling sticks, and a diamond drag tip.

Two layers of masking tape with superglue inbetween - in effect double sided tape. Very solid and rigid in function.
Also a lot less hassle to clean the waste board/carved material.

I have been getting improved results!

I decided to screw the tags down. Notice the difference between tape and screwing down, though I like the hand scratched feel of the other as well.Second, a major difference is in the wear of the bit, do you use a new bit every time? I would say every time my bit is duller, see image below, is this because 10in/min is too fast?

The difference between an engraving with each of these is very noticeable.

Can anyone recommend an engraving filler? In the images, this is just polishing compound, but the last one (in foreground) it’s not deep enough to catch the compound, so maybe it would also not catch engraving filler?

1 Like

You can use paint, but I like Art Resin, which is clear but can be colored any color with a few drops of paint (10 to 1 ratio). Slop either onto your brass and then use either:

  1. The edge of a business card to squeegee off the excess OR
  2. Open a phone book and wet the page with paint thinner or alcohol. Place engraving face down on page and drag it downward. Flip page, repeat. Works like a charm.

Let it dry and clean up the rest.

What’s a phonebook?

1 Like

You can also use any paperback that has been banned by the current administration, instead of burning it at the next rally.

It’s the same list as 1963, 1939, etc. Apparently it is a recessive gene. At least now we have an antidote.