working with brass

Post Reply
Greg47
Posts: 1
Joined: Sat Jul 20, 2019 5:18 pm
Model of CNC Machine: New wave shark

working with brass

Post by Greg47 »

I am relatively new to the CNC world and never posted before. I have made hundreds of things all in 2D, all in wood. I have a design in mind that will use some brass inlay ed in wood. My problem or question is where can I go to get a better idea on tools, feeds and speeds for brass. i could destroy some bits to figure it out but has anyone else tried this?

User avatar
TReischl
Vectric Wizard
Posts: 3820
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: working with brass

Post by TReischl »

Well, I do not have it all figured out but do have a few suggestions.

Brass is grabby, will try to pull the tool into it or pull the work.

Doing any metal work on a router is testy. The spindle speeds are typically way too high. Our routers are typically not as rigid as a machine tool. When doing brass and aluminum I have used very slow feed rates, in the neighborhood of 20-25 IPM, sometimes slower for small cutters below .125 dia. Clearing the chips helps a lot. A lot of heat can be generated so if you can have an air line blowing a bit of air it really helps out.

Generally for all metal work I use HSS bits on the router. Couple of reasons, they can be had cheaply these days so when one breaks it is not a big deal, but more importantly they are much sharper.

When doing profile work I use the ramp/spiral option rather than plunging to depth of cut. Usually take about .010 - .015 per pass. Like I said, slowwww.

Another tip is to remove metal using conventional means whenever possible. If you can rough drill a hole, do it. If you have a cut out and have a scroll saw, remove most of the material that way, much faster. If you can rough saw the profile on a bandsaw and still fixture the part, do it that way.

In my shop I run a metal working lathe and mill. Those little machines can cut aluminum, brass, and steel much faster and easier than my router. In other words, most any machine tool is better at it. But boy, can the router come in handy! Later today I need to cut a hex shape in the end of some aluminum round stock to build a die holder for the lathe. So I will rough drill and bore out the piece to waste the bulk and then use the router to create the hex shape.

One other thing, all brass is not created equal. Pay attention to the grade you want to cut, make sure it is free machining.
"If you see a good fight, get in it." Dr. Vernon Jones

User avatar
Bob Jr
Vectric Wizard
Posts: 379
Joined: Thu Aug 13, 2009 2:13 am
Model of CNC Machine: Axiom, Shark

Re: working with brass

Post by Bob Jr »

Here's some more information from Vectric's last Users Group Meeting:
https://ugm.vectric.com/session/advance ... -and-brass
"Be accurate."
W. Tell

User avatar
Bob Jr
Vectric Wizard
Posts: 379
Joined: Thu Aug 13, 2009 2:13 am
Model of CNC Machine: Axiom, Shark

Re: working with brass

Post by Bob Jr »

Popular Woodworking (December 2020 #256) just included an article on routing aluminum and brass with a CNC Router.
"Be accurate."
W. Tell

Tailmaker
Vectric Wizard
Posts: 345
Joined: Sun Jun 16, 2013 4:40 am
Model of CNC Machine: Home Built 4-axis Router
Location: Fort Collins, CO

Re: working with brass

Post by Tailmaker »

I have done a few projects with brass and found it WAY easier to machine than aluminum. I used the common 360 alloy with some lead content that machines nicely, almost like some super hard hardwood. It does not stick, needs no lubricant or cooling but obviously the feed rate and depth of cut must be reduced to avoid bit breakage for smaller bits. Plunge moves should be ramped but I did not reduce speed (rpm) much. An air jet may help clear chips from narrow cut channels and avoid pulverizing them. Also, brass does not leave sharp swarf on the floor that gets stuck in your shoes.

User avatar
TReischl
Vectric Wizard
Posts: 3820
Joined: Thu Jan 18, 2007 6:04 pm
Model of CNC Machine: 8020 Build 48X36X10 RP 2010 Screenset
Location: Leland NC

Re: working with brass

Post by TReischl »

Yup, aluminum can be nasty. Gum up on the cutter, snap!

I have only cut brass once on the cnc, it went well. I would love to cut brass a lot more, but the cost, YIKES!
"If you see a good fight, get in it." Dr. Vernon Jones

GEdward
Vectric Craftsman
Posts: 126
Joined: Wed Jul 05, 2017 9:13 pm
Model of CNC Machine: Romaxx WD-1
Location: Ipswich, South Dakota

Re: working with brass

Post by GEdward »

I agree that machining brass is much easier than machining aluminum. Both metals need to have very sharp cutters for the best results. I have found that bright finished HSS with a high inclusion angle works best for both. While you can do a descent job on brass with coated bits, coated cutters do not typically work very well at all on aluminum. The main reason being most coatings have some aluminum, AlTiN for instance, in their formulation which causes aluminum to stick to the cutter; unless you are using a coolant formulated for machining aluminum. Aluminum has a nasty trait in its transition temperature between solid and liquid states which causes it to behave like a paste. That property is great for making thin walled aluminum cans, die casting and other forming processes but it is a pain in the butt for machining. High spindle speeds, especially without coolant, cause aluminum to reach that temperature at the cutter interface and stick to the cutter.

Machining any metal works best with spindle speeds much slower than a typical router or 2 pole spindle are capable of achieving. If I were to do metal work with my CNC router to any great extent I would invest in a 6 pole spindle. That would allow spindle speeds slow enough to be more in line with best practices for metal working. An off shore water cooled 80mm dia. 2.2Kw 4 bearing ER20 collet unit can be had for around $900 and on Amazon, a domestically labeled unit is about twice that. That is less expensive than a CNC mill and would allow me to get by.

Ed

Post Reply