Back to Ganoksin | FAQ | Contact

Milling Silver


#1

Hi.

I’m hoping some kind person can give me some advice regarding
machining silver as I have failed ot find the I am
looking for online.

I have a CNC mill that I want to use to machine silver. Spindle speed
is 24000rpm. I want to use either an engraving cutter (half round and
with an 80 x 0.003" tip), or, a TCT 1mm single flute cutter. My
questions are, what feed rate and cut depth should I use and should
I use lubricant, coolant or just keep the swarf clear?

Richard.


#2

ive done it on non cnc equip if it was me i would treat it like
alumnium - goo


#3

Hello Richard Thomas,

If in doubt, I would use values close to that of silver, such as
brass or copper. I would think that silver would machine at a faster
rate so there shouldn’t be any problem. I’ll check my “Machinist"s
Bible” today.

Chris
Chris Gravenor


#4
what feed rate and cut depth should I use and should I use
lubricant, 

coolant or just keep the swarf clear?

Using a 1/32" endmill, at 10k rpm I use a rather slow feed of 3 ipm.
w/ .01" DOC. I have gone faster, but I found that it raised a burr
more dramatically than when I went slow. You could certainly go
faster. I don’t use coolant, but I do use an air blast to clear the
chips out of I feel like they are packing in the cut, sometimes I
don’t though. To date I am only milling flat sheet though.

If you can use coolant it will certainly help a lot, and allow you
to go faster/get a better finish. I don’t because I’m using double
stick tape as a fixturing method.

Ultimately this is in the realm of experimental machining, so be
prepared to break a few cutters…

Nick
www.cartertools.com/nfhome.html


#5

Richard,

I have machined thousands of ounces of sterling, maybe tens of
thousands of ounces, though none with CNC. Most of my experience is
lathe and manual milling, and with larger cutters than you are using,
so I wouldn’t attempt to speculate about feed rates. I can tell you
that your spindle speed may be too high for smooth surface finishes
and high cutting rates even with the small cutter you are proposing.
I know, I know that doesn’t seem right. Silver or copper just don’t
cut well when the cutting temperate goes up, and for what ever reason
flood cooling with aqueous solutions doesn’t seem to work well, a lot
of galling. I have learned to reduce spindle speed and use a micro
drip cooler. I personally use the Trico made in Wisconsin. I could
provide you with more about the Trico off list if you want (just a
customer).

When ever possible cutting silver I use multi flute cutters and with
your spindle speed you may want to test carbide files or nickel
deposit diamond points. I don’t know for sure, but, I suspect you
could achieve a better finish. Still with the micro drip. Milling
with a 1/4" four flute cutter I would use a spindle speed of 2500
rpm and a.010" depth of cut (feed rate will need to be tested, but
will be high) or cutting on a lathe 1/2" round piece with a single
point cutter I would use a spindle speed of 500 rpm and a feed rate
about.004" or.005" per rev. The harder the silver the easier it will
machine, so when possible order hard drawn. Machining castings can
be more difficult because of pull out any time you hit porosity. This
is were machining with diamond points is way better.

Good luck,
Daniel Culver


#6
I would think that silver would machine at a faster rate so there
shouldn't be any problem. I'll check my "Machinist"s Bible" today. 

Thanks for the reply Chris.

Did your Machinists Bible reveal anything for silver?

Richard.


#7
ive done it on non cnc equip if it was me i would treat it like
alumnium 

Thanks for your reply. I haven’t tried aluminium yet…

Richard


#8

Thanks for the info Daniel.

I think I will have to experiment some more - I now have a variable
speed spindle so can run down to 8000rpm, and I’ll just have to try
some different feed rates and cut depths until i get what I m
looking for.

Thanks,
Richard


#9

Hi Nicholas.

I’ve got to say thanks for your great Taig website too - its
certainly given me a lot of inspiration, and I couldn’t have built
my machine without my little Taig (Peatol) Lathe! I am looking at
modifying the lathe to turn it into a DC driven mill for mounting in
place of the router, but thats a little way off for now.

I have now got hold of a router with variable speed (8000-24000rpm)
which should give me a bit more flexibility.

However, so far, I have chipped the tip of the engraving cutter in
two places while engraving three small pieces of silver, using a DOC
of 0.004" and feed rate of 4.7 ipm. I’ve also chipped the 1mm TCT
cutter that I was using to cut the silver piece out with…

The first piece I cut out appeared fine, but where the cutter ran
across another groove, it drew burrs into that groove and I was
hoping to vind a way not too.

Also, although I was stepping down between cuts by 0.004", each time
I ran back along the path, I was infact removing (if my math is
right) 100 times more material on my last cut than on the first, so
each pass at a new depth was increasing the amount of work - no
wonder the finish was so poor!

Incidentally, I have a sacrificial work bed so use double sided
sticky tape to hold the work in place, then use a few self tapping
screws around the work piece as hold downs - no lost pieces yet!

Thanks for your reply.

Richard.


#10

Richard,

Thanks for the kind words about my Taig site.

The problem with the vee cutters is that the tip’s sfpm drops to
zero at the center of the tool. You want the thing spinning as fast
as possible. They do remove more material because of the shape. I
find that 90 deg cutters hold up a whole lot better than 60 or 30 deg
vee tools. Also get them with the biggest tip radius possible for
your design.

They do make burrs too, due to the zero rake angle of the cutting
edge. You could try using small ball end mills if your work can be
designed around a radiused groove. They are much freer cutting. I
have though of using the 1/4 round vee bits but figure they will snap
just from me looking at them.

I’m just glad I’m not the only nut trying this sort of work.

Nick
Nicholas Carter and Felice Luftschein.
homepage at www.cartertools.com/nfhome.html


#11

Hello Richard Thomas,

Did your Machinists Bible reveal anything for silver? 

Sorry it only had figures for industrial materials.

Chris
Chris Gravenor


#12

I found a guideline for milling Sterling silver 925, issued for a
now-defunct medallion milling machine. They suggest these
parameters, for use with their cutting bit ZEC-ARX-BAL (which is
still available from Roland DG):

Z-depth of cut up to 1.6mm
XY feedrate 10mm/sec
Z plunge rate 5mm/sec
Stepover width 0.05mm
Spindle speed 15,000rpm

and they suggest the application of “a little oil by paintbrush, you
can mill dry without oil but the burr or tool mark tends to remain,
compared to oil cutting”.

The ZEC-ARX-BAL cutting bit is an engraving-type bit, but with a
clever single spiral flute. It is solid tungsten carbide and designed
for 1/8" spindles.

Mark


#13

Many thanks for this info Mark.

I find it amazing that there is so little info on the net about
machining silver. I also had a useful reply from Nick Carter, who
reminded me that if you are using a pointed cutter, the tip speed at
the smallest diameter is virtually zero. Just have to experiment some
more.

Richard.