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 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
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
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 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
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.
Very Best Regards.