Back to Ganoksin | FAQ | Contact

CNC Cutting


#1

Dear CNC Folks, I have been tooling wax and plastic for about eight
years now and have a few recommendations.

First, the cutters and speed of spindle are the most important parts
in any CNC Mill. I have used a Servo Impact, Wolverine, Sherline and
Max NC. Currently I use the Max with a retro fit High speed spindle.
It cuts as good as the Servo. Not quite as fast but just as accurate.
Your spindle speed should be 14,000 RPM.

When tooling carving wax the RPM should be 14,000 to 15,000 RPM.
Ferris wax works great. I like the purple. The same stuff I hand
carve. HERE IS THE KEY! Use WD40 as the cutter lubricant. It washes
away and leaves a nice clean surface. I will cut the tool path twice
sometimes but mostly with my plastic. WD40 is the key.

When tooling injection wax I use a different lubricant. This wax
does not tool larger parts very well. It does fine profile work
though like small names incised in small areas on injected waxes.
Call me about this lubricant. The lubricant is a mess so you do need
a tray of some sort to collect the spent material.

The best material I have cut so far I have developed to make class
rings and most any other style you can think of. It is a toolable
plastic that you can steam out when done. Try THAT with wax. This
material holds incredible detail and molds exactly what you tool. I
prefer silicone mold making. The plastic is a total dry cut. No
lubricant. I do use a vortex air jet to help blow the spent material
away. These plastic parts can be either a small component added to a
design or the larger master part itself. The small rectangle parts I
tool for bezels and pendants has alignment keys on each side. To do a
3D image I just cut the front, flip the part align the cutter and cut
the back. Model done!

I also have refined the cutters used for either wax or plastic. They
cut the most detail possible. I can cut approximately thirty parts
with no cutter wear. Just don’t handle them too much. I’ll step down
a rough cut with a larger cutter for larger parts if necessary. Once
the detail cutter is in the CNC leave it in. I usually don’t do
touchoffs either. With a loupe, align the part, calibrate the
position and start cutting the material. I aim for the center of the
alignment marks on my plastics. If you need to be deeper, restart the
tool path a little lower until you find the depth. The cutters are
sharpened to almost .001" with special angles designed to help flush
out material. The cutters are available on my site directly for
anyone who wants to try one. I do not cut brass or any metal. It’s
not necessary. I’ll either cast the wax and mold it, or cut plastic
part and mold that.

Now here’s the disclaimer. LOOK AT THE SAMPLES DONE. The rings on my
site are a small sample of what I do. More are being added this
Spring. I am skeptical of those who don’t make jewelry yet claim
expertise. I have a new motto about CAD CAM also. “Don’t design
beyond your ability to execute.” This goes for anyone doing jewelry
CAD. Show me the finished jewelry!! Virtual jewelry is a pretty
picture but I want more. Here’s my final comment. How much are these
parts going to cost me to make? And where if not in house?

Best Regards & Happy Holidays,

Todd Hawkinson
www.ajt-online.com


#2

Dear All, Very interesting thoughts and some good advice given,
however there are several other considerations that were not dealt
with. Many mention high RPM at the spindle, however this means little
at the end of the day if the correct chip load for the tool is not
taken into consideration. The chip load is the amount of material the
tooth will remove with each revolution. Therefore, you will feed a 4
fluted tool, 4 times faster than a single lip or single flute cutter,
and 25% faster than a 3 fluted tool.

You cannot run the spindle wide open and enter whatever you feel
like in relation to the feed rates, because at the end of the day,
the chip load means you can only remove so much material at a given
RPM and calculated feed rate. By changing the chip load especially on
fluted tools, the size of the chip changes. You can create powder or
nice big chips. In metal, big chips are the way to go. If I run a
1/2" rougher, the chips hitting the inside of the machine sounds like
hailstones on a tin roof. Love it :slight_smile:

RPM x Number of teeth x chip per tooth = Feed rate in mm/min Note
The manufacturer of the tool will provide you with the data for the
correct chip load for a given tool.

Tool geometry needs to be addressed also. End mills or cutters come
in a variety of forms and each have their place. A flat end mill with
centre cutting geometry, means that you can plunge into the material
and the cutter will cut the material at the face of the tool, as well
using the side of the tool to cut or profile. If we look at the flat
end mill, different flute configurations are also available. Straight
and similar to a reamer are usually used in very hard materials,
however for soft gummy materials you should use a tool with a high
helix or spiral. Something like a 60 degree. This will give you a
more aggressive upward motion for the cut material and will evacuate
the chips accordingly. Therefore, not only do you need to look at
coolant and air guns, but also how the tool moves the material. A
high helix tool as I mentioned will move material up and away and
more importantly, clear of the cavity. However if you were to look at
a standard 3 sided pyramid tool, which I might add, these tools do
not cut efficiently in comparison to fluted tools, because they tend
to cut a little, rub a lot and literally try to push material out of
the way. This is due to the lack of a leading edge or cutting edge
that cuts and (simply put) scoops the material away from the surface
as it does with fluted tooling. Taking a look at a pyramid tool with
a draft of lets say 10 degrees, the material is not moving up the
tool and out of the machined area because it has no spiral to do so,
but for all sense of purposes the material is now moving slightly
ahead of the tool and has a 10 degree downward push on the material
which fails to evacuate the material, and even worse compacts the
material back into the cavity. Conclusion is to remove as much of the
material as possible with fluted tools before you move to your
pyramid tool to engrave the detail, because the engraving of detail
is their designed function and they are not to be considered as a
high rate of material removal tool.

Secondly, stay away from carbide tooling and stick with High Speed
Steel. The spindles at the table top level will have what we call a
runout, which can also be made worse by poorly made collets. This run
out means that the tool tip will spin out, or off of its centre of
axis to the tune of something that is easily measured with an
indicator. This is critical for those of you who machines metal molds
in Bismuth or Aluminium. The Carbide tool has no flex to it,
therefore any runout and an incorrect feed rate means that now you
just blew the tip. A HSS tool has flex and is more forgiving, and
therefore will help to maintain a longer tool life but more
importantly that flex allows you to machine 3 times as deep at the
same RPM and Feed Rates. Ok, so in wax the flex is no big deal, but
why spend more money on carbide or cobalt tooling when HSS is all you
need.

I tried to keep it short, but as usual I ran a marathon. If anyone
needs more help on the practical side of machining, or have issues
that need to addressed, I am here to assist you anytime. Dec
19th-Jan7th I will be in Europe, so I may, or may not deal with any
e-mails during that time until I get back, but the offer is there.

Very Best regards.
Neil George
954-572-5829


#3
         stay away from carbide tooling and stick with High Speed
Steel. snip...Ok, so in wax the flex is no big deal, but why spend
more money on carbide or cobalt tooling when HSS is all you need. 

Hey Neil, hope you had a nice Thanksgiving.

You forgot to mention one thing in regards to HSS vs. carbide. HSS
can be ground to a finer, sharper edge.

I do use HSS for wax and fusible alloys, but I stick to carbide for
fine detail in brass or aluminum molds. A tip-off of .1 mm at an
angle of 7� just isn’t strong enough with HSS, yet I have super micro
grain carbide pyramidal cutters that have only needed periodic
resharpening. Maybe it’s just my lack of skill but I have to use
carbide cutters for engraving steel stamps, HSS just snaps.

I once ground a special purpose (wax cutting) parallel 3 flute
cutter with a cross section of .25 mm and 6 mm length that in carbide
that only broke over a year later because of a programming mistake.
The same cutter proved impossible to grind in HSS.

Jeffrey Everett


#4
    Hey Neil, hope you had a nice Thanksgiving. 

Yes I did Jeff, and thank you for asking. Hope you and your good
lady had a very nice day also .

    You forgot to mention one thing in regards to HSS vs. carbide.
HSS can be ground to a finer, sharper edge. 

Yes you are a 100% correct. I was too busy editing and trying to
keep it concise at the time, that in all honesty, I didn’t even think
about it . But a good note from you solved that one :slight_smile: I might add
also, that when a tool is ground to a face of 5 degrees, the actual
cutting edge is not a 5 degree edge, but may be closer to 5.5
degrees. Important when grinding a tool to understand that point
also. I know you are aware of this, so it is a general statement for
others to pay attention to.

    I do use HSS for wax and fusible alloys, but I stick to
carbide for fine detail in brass or aluminum molds. A tip-off of .1
mm at an angle of 7� just isn't strong enough with HSS, yet I have
super micro grain carbide pyramidal cutters that have only needed
periodic resharpening. 

Jeff, I will make comments that are directed towards every CAD/CAM
user, therefore when I say you, it is not directed towards you
personally, but is to be taken as a general discussion to a room full
of people:-) Secondly, I hope I explain myself clear enough, because
this can get complicated to visualize.

The strength of the tool has merit, but in reality it should not
pose a problem as a finishing tool only. The problem that I find with
most users, is that they do not change their way of thinking when it
comes to machining metal molds or stamping dies. When machining a
male, or a positive model in wax, you need to use the smallest tool
possible with minimal draft. This will create nice crisp details and
enable the tool tip to reach the desired depth of lets 0.5mm. The
detail to the front of the piece is the most important aspect and
simply put, the detail needs to stand up high enough, so that when
the high spots are polished, the attention to detail, and the
fineness of the engraving/machining comes into play. Because of this,
the draft of the tool is important. The smaller the draft, the
smaller the tool diameter will be at a depth of lets say 0.5mm. For
a 7 degree per side cutter, the tool diameter at a depth of 0.5mm
will be 0.12278mm. This measurement is given with a zero tip radius
and is therefore a point, just to make the calculations easier for me
:slight_smile: Because of 3D engraving, the machinist has the ability to use
all of the tool from the tip to the profiling angle in simultaneous 3
axis to create very sharp details in lettering. What complicates
this, is the ability to gauge the minimal draft and tip radius
required to create crisp detail at the surface and clean out the
background of the medallion accordingly. Having said that, it does
not make any sense, at least to me, why anyone would use the same
sized tools to machine a metal mold. We have already established the
reason why smaller tools are required to machine a male part, and
those reasons being at least in part, the need to reach the desired
depth, the need to create sharp detail at the surface, and the need
to get the tool in deep to clear the background and separate the
detail as much as possible. In machining a metal mold, you do not
need to worry about the background of the medallion, because you
will area clear that portion with a large flat end mill. All that is
left to engrave is the lettering. Therefore what is important here is
the tool tip and not the draft angle. If you were to use the same
sized tip radius tool, the detail will reflect the same information
as you would in machining the male model at the surface irrespective
of the tool draft. The only difference will be in where the corner
radii are on the finished part. Think about it :slight_smile: Therefore, if the
background is already clear of material, then instead of a 7 degree,
0.1mm tip tool, use a 15 degree 0.1mm tip tool. The diameter of the
tool using the same config as mentioned above would now be
0.26794mm. The difference in the tool radius between the 2 would be
0.07258mm, and not easily measured. The conclusion, is that the
lettering on the finished part would have a slightly larger base
where it meets the background. This in my opinion is not important,
because at the end of the day, the at the surface is of
the same quality and detail as the male counterpart. Also, because of
the increased angle, the part will release much easier and with less
distortion than a smaller draft out of the mold. Less surface to
grab the part. All of my parts that are not mechanically ejected, are
simply hit with air and out they come without inducing stress into
the piece. Note…7 degrees per side. If the tool is a total of 7
degrees, meaning 3.5 degrees on either side, then the measurements I
provided will be much smaller than indicated. If that is the case,
the oooohs just became wows :slight_smile:

Using the bigger draft philosophy, the tool will last longer and
more aggressive speeds and feeds can be implemented. The real issue
is that, most individuals see the difference between 7 and 15 degrees
as a huge diametric problem, without realizing that the diameter
changes little enough to not even be a factor at a depth of 0.5mm.
Yes, they may well be situations where a smaller tool can add a
little more sharpness to the mold, but during the course of
manufacturing, some of that extra machining will be lost during the
whole finishing process. Additionally, using a small drafted tool,
can cause other severe problems in metal molds. If we where to take
the centre portion of a letter A for example. Using a small draft on
a tool would essentially leave a tall, wobbly, thin triangle at the
pinnacle. These pinnacles can move around during injection causing
discrepancies and differences from one injection to another.
Therefore, a larger draft will bring these pinnacles down to a
manageable height. In a nutshell, you do not want to leave thin walls
that can move or get damaged during operations, and the way to do
that is to pay attention to where the important detail is, and reduce
any unnecessary metal that can cause problems.

 Maybe it's just my lack of skill but I have to use carbide cutters
for engraving steel stamps, HSS just snaps. 

Not lack of skill, carbide is the right tool for steel.

    I once ground a special purpose (wax cutting) parallel 3 flute
cutter with a cross section of .25 mm and 6 mm length that in
carbide that only broke over a year later because of a programming
mistake. The same cutter proved impossible to grind in HSS. 

Lets face it, you can grind the tools you need using whatever
material is easiest. Grinding carbide is by no means a simple task
either to do it well. However, there are individuals that can provide
the exact same tooling in HSS and carbide, because they are set up to
do it professionally. Can’t beat a man at his own game. Hope all was
clear, I know how difficult it is to follow things sometimes, but
it’s even worse trying to explain.:slight_smile:

Very Best Regards.
Neil George
954-572-5829


#5

Neil,

I am a lurker and a newby to orchid and to jewelry. I have just
purchased an engraving/milling machine and will be setting it up and
beginning to learn how to use it this week. My question is this:
Would you be willing to answer some basic questions as they come up?
I feel that your experience could save alot of trial and error. I
saw that you left your telephone number. If you are willling to
offer advice, is phone best? If so what time and days of the week?
If email is better, would you prefer on orchid or off?

Thanks,
Mike Buckner
Creative Engraving
865-599-3358


#6

Mike, The answer to your question is yes. I would be more than happy
to do so, therefore start dialing :slight_smile: Usually here 7 days a week from
6am till around 8pm. However, best time to call is after 10am,
because usually by then, all of the machines are setup and running.
Prefer phone, because that means I can walk around and monitor the
machines whilst I am talking :slight_smile:

Best Regards
Neil George
954-572-5829