Suggested CNC machine parameters for copper

[KyuZo]

I'm planning on using a small CNC machine (Roland Camm2) to make the copper base plate for a waterblock and I'm wondering about what kind of machine parameters to use.

The software that comes with the machine has a number of suggested parameters for different materials (Wood, Wax, Plaster, Aluminium, Brass etc.) but none for copper.

The parameters for Brass and Aluminium are actually identicle:

Z speed (mm/sec) : 1.0
Z step (inch) : 0.002
XY speed (mm/sec): 6.0
Path spacing (inch): 0.047
Fine margin (inch) : 0.002




Just for comparison here's the parameters for Acrylic:

Z speed (mm/sec) : 4.0
Z step (inch) : 0.006
XY speed (mm/sec): 6.0
Path spacing (inch): 0.047
Fine margin (inch) : 0.005



I'm using a 2mm drill bit.

The machine supports spindle rotation speeds from 5000 rpm to 15000 rpm.

It mentions "It is only possible to machine metal with great care. Only relatively soft free machining metals should be used for milling, and the CAMM 2 must be set to very slow feedrates and small depths of cut" in the documentation.

Any feedback or suggestions for parameters that could be used to machine copper would be much appreciated.

[]JR[]

RPM as high as possible
Feeds as low as is feasible (really low feeds = really long mill times)

And youll want sharp (new) cutters (bits) and plenty of coolant/lubricant...

]JR[

[tex707]

I think that copper is much more difficult to be machined than brass. The CNC mill you are talking about is, AFAIK, a modeling machine...I even think that the spindle motor is supposed to be replaced every 700 hours of use, right? So maybe you should think twice before using that machine for copper milling…

Is there a provision for cooling on that machine?

[JFettig]

If you could post some specs of the machine, it would help a TON.
HP of the motor,
maybe even sizes of the steppers, or even a link to the machine.

do you mean a 2mm end mill?
for one, make sure you get CARBIDE for machining in that horrible material on a little mill, I have done it, and its a pain in the butt. I took off .03" per pass, and I forgot what feeds I gave it, maybe 1ipm(this was with a 3/16" end mill too)
yeah, the machine was really small that I did the above on, my mill will be completed soon

About RPMs, youll burn up your bits fast if your not careful. a 2mm HSS end mill should run at the maximum of maybe 3000rpm, carbide end mill could be run up to 12000 or so.


Jon

[jaydee]

From what I dug up on Google it is a Rotory Engraver like I use at work. Doesn't use normal endmills. You can get endmills for them but they are not cheap like normal vertical Mill endmills.

[jaydee]

Link:http://www.autoplates.com/Roland/PNC2300A.htm Damn cool little machines. Probably kill it doing Copper though. The one I got at work is it a much bigger one and I made some bases with it but it was rough on the machine. Finally gave up on it and just used my CNC mill.

[KyuZo]

Thanks for all your advice so far.

The link that Jaydee posted has comprehensive spec. for a newer variant of the machine (I think it's probably very similar). The machine I'm using is pictured there but doesn't seem to have spec.

EDIT: I've found the exact spec for the machine I'm using (PNC-2300A) and as far as I can tell they are identicle.

"Specifications:

Table size: 305 mm x 230 mm

Max cutting area: 305 mm (X) x 230 mm (Y) x 30 mm (Z)

Feed rate: X, Y-axis: Max. 3600 mm/min Z-axis: Max. 1800mm/min

Software resolution: 0.01mm/step or 0.025mm/step (XY axis only)

Mechanical resolution: X, Y and Z-axis: 0.00125mm/step (micro-step control)

Spindle motor: 30W (DC motor)

Revolution speed: 5000-15000 rpm

Tool chuck: Cutter holder and collet system

Interface: Parallel (in compliance with centronics specification) or Serial

Buffer size: 1MB

Instruction system: CAMM-GL I (mode1, mode2)

Source: 1.8 A / 117 V 0.9 A / 220-230 V 0.9 A / 230-240 V

Acoustics: During no-load operation: 60dBA or less Standby mode: 30dBA or less

Weight: 28.5kg (62.8 lb.)

Operation temperature: 5-40 deg C

Operation humidity: 35-80% (no condensation)"

There is no means for lubrication/coolant delivery inherent in the machine, would it be a good idea to intermittently spray some WD40 on the work peice (or some other lube/coolant)?

Of the 2 mm "slot drill" that I'm using the manual states: "Slot drill - These tools are excellent for making slots, cutting out, routing etc. They work well with most materials. They cut accurately and generally leave a good surface finish (depending on material, feeds, speeds and depth of cut). The fluted design ensures good waste removal. These tools are therefore suitable for deep cutting (subject to multiple passes). Being carbide tipped they should have a long service life if treated with care."

2nd EDIT: Just been looking up some links for the machine:

http://www.sanhasi.com/pnc2300a_e.html

http://www.signmaster.co.uk/Desktop_..._engravers.htm

http://www.sanhasi.com/pnc2300a_e.html



And for some more images of the machine:

http://images.google.com/images?hl=e...-8&q=pnc+2300a

(Google image search for pnc 2300a)

[]JR[]

A 30w spindle motor isnt going to cut through copper unless your using like a 3/64" cutter, or taking microscopic cuts.

]JR[

[JFettig]

you will definately kill that machine, just to give you a comparison, My motor for the spindle is 450watts.

My steppers are bigger than your motor! @96watts.

Jon

[killernoodle]

It could cut plexi easily. Consider making a waterblock that has a more complicated top than base (cascade design)

[hikke]

Originally posted by ]JR[
A 30w spindle motor isnt going to cut through copper unless your using like a 3/64" cutter, or taking microscopic cuts.

]JR[

How powerful should the spindle motor be if it's going to be used for cutting copper with 1/16"-1/8" cutters?

[JFettig]

I would say the minimum should be 1/2 to do a decent job, see what jaydee has on his and I woudl say thats about the bare minimum. maybe do it on a 1/5hp motor(maxnc that fixxittt has works)

But to cut them with decent speed I would say at least 1/2hp. Your not just looking for the horse power, you need the machine to be ridgid enough so it doesnt bend or break.

Jon

[jaydee]

Originally posted by JFettig
I would say the minimum should be 1/2 to do a decent job, see what jaydee has on his and I woudl say thats about the bare minimum. maybe do it on a 1/5hp motor(maxnc that fixxittt has works)

But to cut them with decent speed I would say at least 1/2hp. Your not just looking for the horse power, you need the machine to be ridgid enough so it doesnt bend or break.

Jon

The motor on ours is 1/2HP DC motor. The one Fixittt has is better than 1/5hp if I remember right. I belive he modded in a 1/2 or 1hp or better motor on it. The motor on my little sherline is equel to a 1/2"hp AC motor form what they say. It has plenty of tourque. Just wish it had more RPM.

[KyuZo]

The design for my waterblock is fairly simple and it's only 3 mm deep cut into the copper (the size of the copper stock is 50 mm x 50 mm x 6mm).

What if I had it cutting in very small increments (as suggested)? So small that the machining time was somewhere between 3 and 6 hours.

[MMZ_TimeLord]

I would say that the first run through with VERY small increments in depth is a good idea. Be cautious that you don't make the depth changes so small that you only succeed in heating up your cutting edges more.

There is a known balance on cutting blades of any type and the rate of cut that keeps them sharper and cooler. I don't have the figures for copper as I do most of mine by hand.

I would very much like to see simple forumla's or table for RPM, end mill size, flute number, rake angle with recommended feed rates.

That to me would be a GEM of information.

[]JR[]

Originally posted by KyuZo
The design for my waterblock is fairly simple and it's only 3 mm deep cut into the copper (the size of the copper stock is 50 mm x 50 mm x 6mm).

What if I had it cutting in very small increments (as suggested)? So small that the machining time was somewhere between 3 and 6 hours.

Say the tool path is 50" in total (lots of passes, your using a small cutter) and youll probably cut at 2"/min @ 4 thou depth, and your total depth is 3/8"

50/2 = 25min tool path

94 passes to reach depth

25 x 94 ~ 39 hours machine time

Youll have to see what speeds it will comfortably cut at, but i should imagine my estimates are not too bad.

]JR[

[jaydee]

Originally posted by ]JR[
Say the tool path is 50" in total (lots of passes, your using a small cutter) and youll probably cut at 2"/min @ 4 thou depth, and your total depth is 3/8"

50/2 = 25min tool path

94 passes to reach depth

25 x 94 ~ 39 hours machine time

Youll have to see what speeds it will comfortably cut at, but i should imagine my estimates are not too bad.

]JR[

Where are you getting 3/8" from? 3mm is less than 1/8", 0.1181102" to be exact. Our engraver could do that in one pas in Brass or 2 passes in Copper with up to a 1/8" cutter. At 10IPM to boot. But it is a $14,000 machine and made very well.

With that small machine of his it would be slower but not much., He hs RPM to make up for tourque and engraving cutters are made for high speed cutting.

Give it a shot. If it kills the machine it's your loss, but if it works your golden.

[]JR[]

250mm/m with a 3mm cutter @ 3mm depth is a bit optimistic through metal imo. A proper mill @ the correct speed would do it, but one of these little machines the ratio of shear force on the cutter to turning torque would be too high.

]JR[

[jaydee]

Originally posted by ]JR[
250mm/m with a 3mm cutter @ 3mm depth is a bit optimistic through metal imo. A proper mill @ the correct speed would do it, but one of these little machines the ratio of shear force on the cutter to turning torque would be too high.

]JR[

You need to start reading posts better I guess.

[]JR[]

Ok you lost me

you said your engraver could do a 3mm depth, with a 3mm cutter @ 250mm/m

depends on how big the spindle motor is. the nc machine in this thread would never do it, infact it tells you the aluminium parameters...

1mm/s = 60mm/m
0.002" cut depth = 0.005mm/pass

Assuming we want to go 3mm deep thats 600 passes, with lets say a 200mm tool path (rater optimistic imo)

((200/60) * 600)/60 = 33hrs

I may be guilty of not reading the original thread, although my gestimates arent too bad, the feed i guessed just about right, but i got double the z feed over twice the distance. The toolpath length is shorter in this guesstimate but its almost certainly too short. Depends on the block design.

]JR[

[jaydee]

I said 2 passes in copper, not one pass.

Also he said he will be using a 2mm bit.

Also you have no clue what his design is. Could be 4 stait cuts, could be 8 strait cuts, could be non of the above.


But I agree that machine will get it's ass kicked. The one I used was designed for METAL, this one is not as it says to be very careful in metal. Copper is a bitch. Copper is like cutting a frozen stick of butter with a butter knife, and brass and alumium is like cutting a thawed stick of butter with a butter knife.

I personally wouldn't do it on that little machine. It costs to much to tear up for a water block.