Cutting brass on a desktop CNC router/mill

[Hawk]

I am testing a desktop CNC miller router to see if it is possible to use it for producing parts in brass.

The machine is a standard Heiz High-Z 400 with a Kress 1050W spindle with a top speed of 30.000 RPM.

 

I have seen some excellent work done in brass on machines like this, so I know they have potential, even if they are lightly built and rather basic.

 

I did my first serious tests this weekend, the subject was a end beam for a mineral wagon in 0-scale (meter gauge)

 

The brass is 2mm thick CZ120 engravers brass. I use double-sided carpet tape to fasten the sheet of brass to a piece of MDF.

 

All milling was done with a flat tip (fishtail) 2-flute 2mm cutter.

 

The best results was obtained with a feed speed of 4mm/s, full speed on the Kress and shallow cuts of 0.3mm. It also seems that the cuts became a bit smoother after some milling time, could it be that the carbide cutters are a bit too aggressive when new?

 

Here are some pictures. The pictures are fresh from the machine, I smooth out the parts with files and emery cloth before assembly.

 

 

 

 

 

(The coupler pocket in the last picture is a brass part from Shapeways, by the way)

 

I would love to hear from others that have tried out machines like this.

[Nimbus]

The brass is 2mm thick CZ120 engravers brass. I use double-sided carpet tape to fasten the sheet of brass to a piece of MDF.

 

All milling was done with a flat tip (fishtail) 2-flute 2mm cutter.

 

Were the holes drilled in the same machine session?

 

The Nim.

[Hawk]

Nimbus, on 16 Feb 2014 - 15:22, said:

 

Were the holes drilled in the same machine session?

 

The Nim.

Yes, the holes were drilled at the same time. Compared to milling, the drillling is trivial.

 

I divide the work into separate nc- files, so the procedure was like this:

 

1. Drilling all the holes with a 0,5mm bit. Just to be safe, I used "peck drilling", the drill goes down 0,3mm, retracts entirely from the hole, drills another 0,3mm, repeat until final depth of 2,5 mm is reached. Downward speed around 2mm/s. I know, this is probably far slower than neccesary, but I had just one 0,5mm drillbit, and I really did not want to break it. RPM was around 2000o, me thinks.

 

2. Milling the slot of the beam. This takes three parallell passes with the 2mm cutter. I got cleaner results with the 2mm cutter than a 3mm one.

 

3. Milling the contour of the part

 

I know that I probably could have rolled the last two jobs into the same nc-file, but I really try to keep things simple and systematic.

 

Some professional machinists will probably roll their eyes in horror at the way I behave myself, but I am entirely self/google trained in this field, so bear with me!

[raymw]

Hi Hawk,

 

Looks fine to me, but I guess you'd like to do better..

 

There are useful speed/feed tables for various types of cutter - here's one http://www.cutweltools.co.uk/files/ww/UC%20A30-32.pdf . I now get nearly all my cutters from Cutwell. If your spindle doesn't take the 6mm weldon/throwaway cutters, then maybe you could get an adapter for them - it will save you a fortune.  Although carpet tape does the job, you can get different results depending on the tape, and if you're profiling, it will wear your cutter.(as will mdf). Although it is more difficult, sweating the sheet to a metal block would be a far better option, or just use a larger piece and clamp it down, leaving tabs on the profile path, so the work-piece doesn't break free on the final cut, or leave a thin web all the way round.. On a light machine, you will get the pattern/ridges at the base of the endmill cuts, try a finishing cut at right angles, also try hand crafting the g-code, I expect your machine is not rigid enough to handle climb milling, which generally gives a better finish (on the edges, but you haven't got much of those...).

 

For brass, hss cutters are best, but they don't last as long as carbide. Never use a brass cutter on anything else, and a cutter, once used on steel, will be rubbish on brass.

 

You can get reground small carbide drills, for not much money, you have to treat them as disposable. For thin sections, use a diamond 'stone', and make spade drills out of sewing needles - even cheaper.   I think your drill rpm is far to slow, and generally I think you are taking all your cuts 'too gingerly', Your swarf should be chips, thrown well away from the cutting area, not dust clogging up the tools...............

 

Best wishes,

 

Ray

[Hawk]

Thanks for an informative reply, Ray!

 

But there are a couple of things I do not understand. You say my rpm is far too low, but I am going full blast on the Kress wich means 32 000 RPM. The driling was done on 20 000, and you might have read that as 2000 RPM for all jobs?

 

Regarding feed speed, I am using 4mm/s wich is exactly 240mm pr minute. Just as the charts you linked to says.

 

Do you have an opinion on "fishtail" endmills vs. regular flat ones, by the way?

[raymw]

Hi Hawk,

 

I don't think I've any fish tail mills. Usually I'm using 3 flute slot drills, and chewing up lumps of ali. I read your drill speed as you wrote it - 2000o, (thinking that the 'o' was a foreign way of writing rpm  ). iirc you never mentioned the milling speed, only the maximum speed your spindle was capable of. Be aware that the cutting speeds are only guides, and of course the actual speed is related to the number of flutes, clearance for chips and so on and so forth. I had some complex formula for calculating feed rates, etc, but or the low level messing about we do, the juice isn't worth the squeeze,  I think you'll find lots of sums on the Cutwel site, and others, but generally for fancy materials. Vibration is the killer on small machines, and the recommended settings may not work out for you - experience will tell.

 

I think what you have done is good enough. If you are entering into mass production, then maybe you'd need something else. Depending on the size of your brass sheet/rod stock, I'd most likely mill the slot first, then profile and finally drill all the pieces held in a simple jig/vice. But, whatever works for you.

 

These guys have some smallish reground carbide drills - http://www.megauk.com/carbide_drill_bits.php but hss is less brittle, but I'm not sure not sure if they still supply hss.

 

 

Best wishes,

 

Ray

[billbedford]

I divide the work into separate nc- files, so the procedure was like this:

 

1. Drilling all the holes with a 0,5mm bit. Just to be safe, I used "peck drilling", the drill goes down 0,3mm, retracts entirely from the hole, drills another 0,3mm, repeat until final depth of 2,5 mm is reached. Downward speed around 2mm/s. I know, this is probably far slower than neccesary, but I had just one 0,5mm drillbit, and I really did not want to break it. RPM was around 2000o, me thinks.

 

There is no need to drill all the way through the block. The holes only need to be slightly deeper than the finished thickness of the component.

 

2. Milling the slot of the beam. This takes three parallell passes with the 2mm cutter. I got cleaner results with the 2mm cutter than a 3mm one.

 

This sounds like the you were running the 3mm cutter too fast. The important variable is the peripheral speed of the cutter, so running the 3mm cutter a 2/3 the speed of the 2mm now should give a similar result. 

[flubrush]

I would love to hear from others that have tried out machines like this.

 

Hawk,

 

Not with the same type of machine,  but having similar trials and tribulations milling brass.  I use a CNC mill - a KX1 -  and my problem is trying to use small carbide cutters with a spindle speed which is probably too slow.  The maximum speed of my spindle is 7000rpm and I am normally using 0.5mm and 1mm diameter two-flute slotting cutters.   I get reasonable finishes which clean up quite nicely with a glass fibre brush,  but my main problem is cutter breakage when the load on the cutter is probably just a bit too much for the brittle carbide.   At the moment I am getting down to 90 - 120mm/min with cutter depths of 0.1mm with a 1mm cutter,  and 60mm/min and cutter depths of 0.05mm for 0.5mm cutters and tool life is reasonable.   I have got away with higher settings than these in the past,  but I've got a pile of broken 3mm carbide shanks as an indicator of when I haven't. :-)  Here's a picture or two of what I've been doing - the bits for a cylinder assembly for a Caledonian dock tank in S scale

 

 

 

 

 

These are in "off the machine" condition with no cleaning up with the glass fibre brush.

 

For holding down,  I tend to cut from sheet with tabs to hold the piece in place until the cutting is complete.   This means the sheet can be clamped firmly to the table.    I don't think double sided tape would hold small pieces against the cutting tool forces.  I do use double sided tape when cutting styrene where it does work well.   The only exception in the above pictures were the cylinder covers which were machined on circular stubs turned up in the lathe to close to finished diameters.

 

I am quite envious of your higher speed spindle and I'm tempted to purchase something similar for the KX1 - there's enough meat on the KX1 head to bolt one on but you would lose a lot of available X travel because of its offset to the side of the current spindle.

 

Jim.