Back to Ganoksin | FAQ | Contact

CNC Wax Masters


#1

I have a question for those doing CADCAM wax master patterns, How
much finishing do the patterns you send to your customers require,
Reason I’m asking is I have been getting masters that still are
showing tool marks on the back, some still have a significant degree
of flash in inside cuts, and nearly all look as though the outside
edges were filed with a checkering file!. The lines appear to be
about 60 to 75 lines per inch and have a depth of around .010 to
perhaps as much as .020 IN. These are most noticeable on rounded or
areas that have a radius. Is this type of tool marking inherent to
parts machined with a mill that uses steppers, or could this be
solved by using a faster spindle speed and a slower rate of travel?
Or would it take a different tool size accompanied by a difference in
travel lineal travel, do to the size of the tool serrations on the
edges, to me it seems as though a very small end mill is being used.
Some straight edges are reasonably free from the edge serrations
which lead me to believe that the X-Y steppers are not quite working
to insure a smooth arc. Or that the Tool is being pushed too fast, I
am doing quite a few castings for my client who is the one actually
paying for the originals, and I have broken several trying to clean
up flash and areas that were supposed to be cut all the way through
but weren’t. Fortunately until last Sunday all of the broken waxes
were easy to repair and I was able to fix and clean them up. Sunday I
broke one through a very detailed area and am not able to fix it, SO
guess what I get to eat. The originals are done on Ferris Green which
would seem to be a good material since it usually cuts and scrapes
pretty clean, so I just want to find out whether these (rough waxes)
are customary or is this just a case of operator error of trying to
hurry, I realize that tool marks can be a problem because I used to
work for Northrop aviation and spent many many shift hours in front
of Bridgeport and Lagun Milling machines, but back then NC was just
in it’s infancy and I’ve had no real NC or CNC experience so I’m not
really sure of the limitations of a table top system, I have been
studying EMC and G code and have collected some great software but I
don’t know whether to start doing the CADCAM my own self or keep
swearing at the person doing the waxes I’m having trouble with. I
have managed to get MASTERCAM 9, JewelCad, and two other top shelf
programs, I’ve been looking at Sherline mills, but they only work
with Linux and EMC I’m used to Linux, but I really don’t have the
time to write the code, and keep up my production, I’d rather let the
software do it. Does someone know if I can get a control card and box
that operates on a Windows platform and is it possible to convert a
Sherline to servos instead of steppers or are steppers even the root
of the problem? I’m hoping that I can if necessary find an
inexpensive milling machine that will work with the software that I
have accumulated, that’s why I’m really curious about a Sherline,
that and the availability of a 4th axis not to mention the initial
price. Thanks

Kenneth Ferrell
www.shadras.com


#2

Hi Kenneth,

As you surmise the surface finish on a milled wax is determined by
both the actual shape of the cutting tool, the milling strategy used,
and some basic geometric facts. In general the type of problems which
you are describing sound like the resolution used when generating
tool paths being too coarse. Additionally, different shapes of tools
are best suited for particular milling strategies. While one tool and
strategy will produce a wax resembling the design, sometimes several
different cutters and strategies are needed to best produce a
specific design. The effort to create a tool path incorporating the
best tool shapes and strategies is well spent; extra milling time
from working with sufficiently fine resolutions is just another part
of the process. I’d rather spend a couple of extra hours waiting
for the mill than spend my time removing tool marks. Hand work should
be reserved for things which can’t effectively be milled and adding
personal touches.

Jeff

Demand Designs
Analog/Digital Modelling & Goldsmithing
http://www.aztec-net.com/~jdemand


#3

The lines on the curves are an artifact of the step over of the tool
cutter and the controlling software. In ArtCAM, this can be
controlled by increasing the pixel count in relationship to the size
of the piece. I just had my mill upgraded by Modelmaster, there is
considerably less debris left on the part, and overall a better
surface to the model. I am not familiar with other systems, but
Daniel Grandi of Race Car Jewelry commented to me on the high quality
of my models in comparison to other CAD-CAM models that he has dealt
with. The development efforts of both Delcam and Modelmaster speak
for themselves. I really would not want to write and test the G code
files that ArtCAM turns out flawlessly in a matter of seconds. Some
of the files are several megabytes in size.

Rick Hamilton


#4

Ken, There are several issues going on with the parts you are
receiving, and I will at this point eliminate the machine as the
issue, because from what you are describing, there are other
fundamental issues at work.

    I have a question for those doing CADCAM wax master patterns,
How much finishing do the patterns you send to your customers
require, Reason I'm asking is I have been getting masters that
still are showing tool marks on the back, some still have a
significant degree of flash in inside cuts, and nearly all look as
though the outside edges were filed with a checkering file!. 

The flash on the inside cuts are due to the fact that the machinist,
finished the through cut precisely to the required depth, and when
the item was flipped and the rest material was removed to bring the
material to thickness, they were both pretty much at zero. The tool
could not cut that material cleanly away because it was probably
being pushed away from the tool tip. Conclusion is to always machine
through cuts beyond that of the finished part thickness, ensuring
that all material when you flip the part is cut away efficiently and
limits any idiosyncrasies in the material moving.

    The lines appear to be about 60 to 75 lines per inch and have
a depth of around .010 to perhaps as much as .020 IN. These are
most noticeable on rounded or areas that have a radius. 

I will assume that the witness lines are on a 3D surface. First of
all, 60 to 75 lines per inch (LPI) are very course step overs. At 60
LPI, the step over equals .01666" recurring, and for those working
in mm’s it equates to a step over of .423mm which is really
unacceptable. At 75 LPI, the step over equals .01333" recurring, and
for those working in mm’s it equates to a step over of .338mm which
is also unacceptable. The depth of the grooves are the direct result
of the step over, and is referred to as the cusp height. In many
software packages, you can select step over or cusp height, which
means that the cusp height needs to be set to zero for a mirror
finish, and that setting will automatically calculate the correct
step over to achieve the desired surface finish. Step overs for
really sharp and super clean surfaces should be anywhere from
.0001-.0005" or .0025-.0127mm. Using the conical engraving tools and
ball end mills will not guarantee a super finish either even if the
step over is very tight, due to their cutting geometry. Forget
getting a nice finish at the surface with an engraving tool. A ball
end mill, although a better choice, is still with problems that need
to be addressed. The tip of the ball, does not cut the material
efficiently, but rather rubs it out of the way. This is due to the
fact that the optimum cutting edge on a ball end mill is slightly
off of centre. Therefore whenever the centre of the ball end mill is
engaging material that needs to be removed, it can, and most likely
will, leave witness marks appertaining to its path direction. This is
why the best surface machining in 3D applications are done via 5 axis
because it rotates either the tool or the part into a position that
allows for the optimum cutting edge to engage the material and not
the tip. The best tool for the job, is a flat end mill with corner
radii. Granted, the pieces I machine these days are larger, therefore
I have more room to work with, but they do have miniature end mills
with corner Radii which are called bull nose tools. The beauty of the
bull nose tool, is that from the face of a centre cutting end mill
around the radii and up to the profiling flutes are all optimized
cutting edges which means that regardless of where the tool engages
the material, the cut is efficient. Also, with a bull nose, the step
over will be greatly reduced when compared to ball end mill and still
achieve the desired finish.

    Is this type of tool marking inherent to parts machined with a
mill that uses steppers, 

You can get the same problems using servos. Although servos are
superior, at this point, the real issues are not fundamentally the
fault of the drive components, but more so, the lack of the clear
understanding of machining strategies.

    or could this be solved by using a faster spindle speed and a
slower rate of travel? Or would it take a different tool size
accompanied by a difference in travel lineal travel, do to the size
of the tool serrations on the edges, to me it seems as though a
very small end mill is being used. 

Speeds and feeds are important and critical, however, changing those
parameter alone, will not change the fact that the step overs where
too aggressive, and tool geometry was not considered.

    Some straight edges are reasonably free from the edge
serrations which lead me to believe that the X-Y steppers are not
quite working to insure a smooth arc. Or that the Tool is being
pushed too fast, 

Not a stepper problem for the most part, but due to the fact that
the linear moves are clean, and the arcs are not, points me to the
software. When machining from data that was derived from a solid
model, this is most likely the culprit. Because of system resources
and the amount of computations going on, most software solutions will
default to a low resolution display to speed up redraws and
calculations etc unless otherwise specified. This is fine when you
are working and time is of the essence, however when it is time to
export that file, you had better crank up that resolution because
what you see on screen, will be exactly what is machined. This
flexibility is there for computing power, but also to reduce and
enlarge export file sizes accordingly for specific tasks. You may
e-mail a colleague a file in a low res, because the file will be
smaller, and once he brings it into the native environment on his
side, he can crank up the res either for display purposes or for the
critical part of machining. 2D DXF files generated from a solid model
will export the lines and curves and simply put as point to point. A
circle in a solid model is in fact faceted. The res level will
determine if it has 6 facets at a low res or hundreds at a high res.
These facets are then transposed to the machine and the result is
faceting on a part. What needs to happen here, is in the CAM package,
replace all of the arcs with new clean arcs that are smooth vectors.
The DXF from the solid model are also vectors, but they bring too
much baggage and way too much Circles when looking at
them in point node will most likely show hundreds of points to
reflect that circle. In Type3, we can select that circle and convert
it into a 3 point circle which is all you need to define a circle.
When you have a super clean arc, the code will reflect this cut as a
starting point, an end point, and an R value for a radius move. This
will now be machined as a true arc and not as a point to point linear
move. Even with steppers, this will reflect a huge improvement in the
quality of the surface. With 3D surfaces, well there’s not much you
can do about that, it is what it is. However increasing the res will
most definitely result in better quality machined surfaces.

    The originals are done on Ferris Green which would seem to be a
good material since it usually cuts and scrapes pretty clean, so I
just want to find out whether these (rough waxes) are customary or
is this just a case of operator error of trying to hurry, 

Sloppy machining.

     I realize that tool marks can be a problem because I used to
work for Northrop aviation and spent many many shift hours in
front of Bridgeport and Lagun Milling machines, but back then NC
was just in it's infancy and I've had no real NC or CNC experience
so I'm not really sure of the limitations of a table top system, 

The trick is understanding what causes tool marks and how to avoid
them. I manufacture 5 point harnesses for the Aviation and Motor
Sports industries and one part in particular is 2.75" in Diameter. On
the prototype I finished the top surface with a .5" flat end mill
with a .375" step over. The surface was smooth as silk, however to
the eye you could see the evidence of the toolpath. It wasn’t a
problem because they were to be polished anyways. But being an anal
perfectionist I wanted the delivered part to look better. The
conclusion was that I spent $600 on a 3" Mitsubishi face mill that
cut it in one pass and left close to a mirror finish. Because the
tool was larger than the part, there was no step over and therefore
no evidence of a tool of any given diameter being involved with the
cut.

    I have been studying EMC and G code and have collected some
great software but I don't know whether to start doing the CADCAM
my own self or keep swearing at the person doing the waxes I'm
having trouble with. 

You can continue along the present path and nothing will change,
except for more grief, or you can take the plunge and take care of
the parts yourself. It is apparent to me, that you have the right
thought pattern and the resolve to want to improve on the elements
that are causing you grief which is a 3rd party. I think you know
what you need to do.

  I  have managed to get MASTERCAM 9, JewelCad, and two other top
shelf programs, I've been looking at Sherline mills, but they only
work with Linux and EMC I'm used to Linux, but I really don't have
the time to write the code, and keep up my production, I'd rather
let the software do it. Does someone know if I can get a control
card and box that operates on a Windows platform and is it
possible to convert a Sherline to servos instead of steppers or are
steppers even the root of the problem? I'm hoping that I can if
necessary find an inexpensive milling machine that will work with
the software that I have accumulated, that's why I'm really curious
about a Sherline, that and the availability of a 4th axis not to
mention the initial price. 

Andrew Werby can answer these issues. He knows this stuff inside and
out.

If you need more help, give me a call.
Best Regards.
Neil George
954-572-5829


#5
 have a question for those doing CADCAM wax master patterns, How
much finishing do the patterns you send to your customers require,
Reason I'm asking is I have been getting masters that still are
showing tool marks on the back, some still have a significant
degree of flash in inside cuts, and nearly all look as though the
outside edges were filed with a checkering file!. The lines appear
to be about 60 to 75 lines per inch and have a depth of around .010
to perhaps as much as .020 IN. These are most noticeable on rounded
or areas that have a radius. 

A pattern should have very little need for finishing other than
light sanding and polishing. It sounds like the machine operator is
using very coarse settings typically used in roughing passes. When
milling wax, all roughing steps may be eliminated and only finishing
toolpaths used. Finishing toolpaths typically have much smaller
step-over distances (more passes) and can produce very smooth
surfaces. The cutting tool used should be appropriate to the surface
being machined i.e., curved or very fine tools for curved surfaces,
flat tool for flat surfaces, etc.

Is this type of tool marking inherent to parts machined with a mill
that uses steppers, or could this be solved by using a faster
spindle speed and a slower rate of travel? Or would it take a
different tool size accompanied by a difference in travel lineal
travel, do to the size of the tool serrations on the edges, to me
it seems as though a very small end mill is being used. 

This type of tool marking is more a result of using step-over
distances that are relatively large, and possibly using a cutting
tool not appropriate for the desired surface. The difference between
steppers and servos is most likely not an issue here. The issue at
hand is possibly related to the inexperience of the machine operator
in producing smooth wax patterns.

If a very small endmill is being used, then very small step-over
distances are required if cutting curved surfaces.

Some straight edges are reasonably free from the edge serrations
which lead me to believe that the X-Y steppers are not quite
working to insure a smooth arc. Or that the Tool is being pushed
too fast, 

Possible but very unlikely. Even an inexpensive machine tool like
the MaxNC is capable of producing smooth surfaces if the machine is
work well and appropriate working parameters are used. I’ve seen
stepper motor mills produce surfaces completely void of tool marks.

I am doing quite a few castings for my client who is the one
actually paying for the originals, and I have broken several trying
to clean up flash and areas that were supposed to be cut all the
way through but weren't. 

There shouldn’t be any flashing. A jewelry wax pattern should be
produced within certain specifications; rough surface finish and
flashing are unacceptable.

Fortunately until last Sunday all of the broken waxes were easy to
repair and I was able to fix and clean them up. Sunday I broke one
through a very detailed area and am not able to fix it, SO guess
what I get to eat. The originals are done on Ferris Green which
would seem to be a good material since it usually cuts and scrapes
pretty clean, so I just want to find out whether these (rough
waxes) are customary or is this just a case of operator error of
trying to hurry, I realize that tool marks can be a problem because
I used to work for Northrop aviation and spent many many shift
hours in front of Bridgeport and Lagun Milling machines, but back
then NC was just in it's infancy and I've had no real NC or CNC
experience so I'm not really sure of the limitations of a table top
system. 

Ferris green is a good wax, no problem there. You haven’t mentioned
the machine being used to produce the waxes, but I doubt the machine
is the problem here. Tabletop systems range in price from about $2K
to $100K with most in the $10K to $20K range. The limitations of the
very low end systems relate largely to accuracy and speed, but even
the very lowest end system should be producing useable waxes.
Operator inexperience is most likely the issue here.

I have been studying EMC and G code and have collected some great
software but I don't know whether to start doing the CADCAM my own
self or keep swearing at the person doing the waxes I'm having
trouble with. 

CAD/CAM is an area of specialization and requires a substantial
investment of both time and money. More simply, if your vendor will
not produce a quality of wax that works well for you, maybe it’s time
to find another vendor.

I have managed to get MASTERCAM 9, JewelCad, and two other top
shelf programs, I've been looking at Sherline mills, but they only
work with Linux and EMC I'm used to Linux, but I really don't have
the time to write the code, and keep up my production, I'd rather
let the software do it. Does someone know if I can get a control
card and box that operates on a Windows platform and is it possible
to convert a Sherline to servos instead of steppers or are steppers
even the root of the problem? I'm hoping that I can if necessary
find an inexpensive milling machine that will work with the
software that I have accumulated, that's why I'm really curious
about a Sherline, that and the availability of a 4th axis not to
mention the initial price.

OH boy… I’d dump any pirated software that are just taking up
space on your hard drive and wasting your time (there’s no way you’re
ever going to learn to use them all anyway) and buy one design
program to begin with. I suggest Rhinoceros because it’s affordable,
and become a capable modeler. There is enough of a commitment
required to learn Rhino well enough to use for jewelry work to keep
you busy for a long time. You’re FAR better off concentrating on just
one capable program to begin with. Sorry if my frankness bothers you.
Been there, done that… If you are truly serious in setting up a
CAD/CAM system in-house, set a budget and fit the software and
machine into that budget. Consider a package you can afford to
lease-to-own. Probably your best low-end bet is the Taig mini-mill
(www.microproto.com). It can be purchased with a 4th axis and control
software/hardware for under $3000. DeskProto is a decent and
inexpensive CAM program that has 4 axis capability. For about $5000,
you can set up a useable and complete introductory system that will
get you by Then you can dump the downloads.

Jeffrey Everett


#6

It sounds to me as if the milling was set up too coarse. I use Rhino
to create my designs and Desk Proto to generate the tool paths. If
you choose very high resolution your tool paths can be as close as
one hundredth of a millimeter. The milling would take a lot longer
to do than with wider tool path separation. Time is money so I
suppose the people who are doing your milling are setting the tool
paths too coarse to save time in milling. With a ball mill you
should be able to mill a surface which looks almost polished.

If you’re looking for a reasonably priced system I would recommend
the one I am using. I have a Taig mill with with the longer x-axis
and a forth axis. The mill and controller plus controller software is
around $2100, the forth axis was $650. This is a very rugged and
dependable little rig. Desk Proto is awesome software and very easy
to use. I use BobCad (an older version) for simple planimetric
milling jobs. I’ve looked into the more expensive software like
ArtCam and Matrix but didn’t feel they were worth the money. Rhino
takes some time to get on to but it is a very versatile program and
I believe I can produce better designs with it than I could with
these high end programs.

If you’re handy you could buy the motors and controller separately
and save quite a bit of money. If you think you need servo drivers,
you can buy the whole set up for around $1300 minus the milling
machine.

Check out Micro Proto Systems for the Taig setup. Any questions?
e-mail me.

Robert Hood
@hoods1


#7

I want to thank every one for their input on the wax finish
question, Jeffery my Mastercam isn’t a pirated piece I bought it at a
School surplus auction I have the box, two manuals and could register
it I believe. Not that I ever register software any way, and the
jewlecad is their evaluation copy, We won’t discuss the other
programs I’ve been considering Cad/Cam for several
years, and this fiasco with this vendor is probably going to get me
off my hind side and step into the fire, Last year I experimented
with Rhino’s demo and that does seem to have a pretty steep learning
curve. I spoke with the wax vendor and he said that well the models
were just for silver so … Well I guess if he were the one that had
to do the casting, and clean up and the waxes were for Platinum or
Karat Gold he could do a better job. Unfortunately I’m the slob that
gets the honor of trying to explain to my client why the job is going
slowly and that well yeah they are a bit thinner than I’d like to
have them too. and so on and so on. I guess I’m a bit anal when it
comes to sending the best I can to my clients and when I have to
scrap a very high percentage of my waxes due to someone else’s
uncaring quality then it’s time for a change. The waxes in question
were done on a 3D wax mill to me it seems like an OK machine for the
money, but I think I’m going to set up a Taig either that or the Max
cnc 10 open loop, I wish I could afford the Max 10 closed loop but
I’ll still have to grab some tooling and LOT’S of wax blocks to
practice with, I’m going to have to start producing waxes in about
two weeks that will pass my criteria and my client’s, unfortunately I
think I’m harder to please than most stone age casters. Fortunately
for me there is a pretty friendly teacher at a vocational school near
by, He’s willing to help me with the CAD end. I’m very grateful for
the help and advice from every one that responded to my question, I
was really starting to wonder if I was being unreasonable. Or being
had, I guess that question got answered big time.

Thanks
Kenneth Ferrell


#8
    I want to thank every one for their input on the wax finish
question, Jeffery my Mastercam isn't a pirated piece I bought it at
a School surplus auction I have the box, two manuals and could
register it I believe. Not that I ever register software any way,
and the jewlecad is their evaluation copy, We won't discuss the
other programs <Argh Matey> 

Hi Kenneth

Sorry about certain comments, I regret them. At any rate, a
MasterCam license is not transferable. Just the same, you can play
with it, but you’ll find you may be wasting your time. It’s a VERY
difficult program. You’ll be far better off with programs such as
VisualMill, DeskProto, XCam, etc. At any rate, I’m available to help
you get running with whatever program you run, or to mill some
pieces. I don’t currently have a 4th axis, but I have friends who do.

    I've been considering Cad/Cam for several years, and this
fiasco with this vendor is probably going to get me off my hind
side and step into the fire, Last year I experimented with Rhino's
demo and that does seem to have a pretty steep learning curve. I
spoke with the wax vendor and he said that well the models were
just for silver  so ... Well I guess if he were the one that had to
do the casting, and clean up and the waxes were for Platinum or
Karat Gold he could do a better job. Unfortunately I'm the slob
that gets the honor of trying to explain to my client why the job
is going slowly and that well yeah they are a bit thinner than I'd
like to have them too. and so on and so on. I guess I'm a bit anal
when it comes to sending the best I can to my clients and when I
have to scrap a very high percentage of my waxes due to someone
else's uncaring quality then it's time for a change. The waxes in
question were done on a 3D wax mill to me it seems like an OK
machine for the money, but I think I'm going to set up a Taig
either that or the Max cnc 10 open loop, I wish I could afford the
Max 10 closed loop but I'll still have to grab some tooling and
LOT'S of wax blocks to practice with, I'm going to have to start
producing waxes in about two weeks that will pass my criteria and
my client's, unfortunately I think I'm harder to please than most
stone age casters. 

I think the better of the two mills is the Taig, purchased from
www.microproto.com. I mill pieces for silver with just as much care
as pieces for platinum. Maybe if you tell your vendor to re-mill the
unacceptable jobs he will. Anality is a good thing when it
represents a caring attitude about your work. At any rate, two weeks
really isn’t sufficient to set up and learn to use the mill. There’s
a bit of a learning curve in milling. The good news is help is
available. You’re welcome to email me privately
(@Jeffrey_Everett3).

Jeffrey Everett


#9

Kenneth,

I just wanted to put in my $.02 here. I have had the setup from
ModelMaster for about 4 years now. I read in you email that you are
in a hurry to get setup. ModelMaster is the way to go man!!

I know that their turnkey setup costs a prety penny, but I’ll have
you know that wihtin 3 hours of having the machine shipped to me. I
was making USEABLE waxes. Try and pinch pennies all you want, just
email me after you;ve had your TAIG for a day and tell me how many
waxes you’ve milled.

I know it’s not cheap, but its a complete setup. The Hardware is
there, the software is there, and the training and support is there.

Please email if there is something I can clarify

Zach (recovering RHINO user, now satisfied ArtCAM user)


#10

Kenneth,

   I know that their turnkey setup costs a prety penny, but I'll
have you know that wihtin 3 hours of having the machine shipped to
me. I was making USEABLE waxes.  Try and pinch pennies all you
want, just email me after you;ve had your TAIG for a day and tell
me how many waxes you've milled. 

I don’t think it’s necessary to disparage the Taig mill in order to
convey your enthusiasm for the Modelmaster, Zach. Many people make
perfectly usable wax models with Taigs, and the setup isn’t
difficult. People’s learning curves may differ, but there’s no reason
one can’t be up and running with it in short order.

   I know it's not cheap, but its a complete setup. The Hardware
is there, the software is there, and the training and support is
there. 

Taig also offers hardware, software, and support. One can also buy 5
of them for the price of one Modelmaster.

Please email if there is something I can clarify Zach (recovering
RHINO user, now satisfied ArtCAM user) 

Rhino can do some things that ArtCAM cannot, although ArtCAM makes
other things easier, notably producing a typical sort of relief from
2d art. Again, you can get quite a few seats of Rhino (and throw in a
few CAM programs too) for the price of one copy of ArtCAM. While it’s
nice that you’ve got a system you’re happy with, there are plenty of
happy Taig (and Rhino) users as well. There’s no one way to do this;
the choice of tools really depends on what one is trying to
accomplish, and how much one has to spend.

Andrew Werby
www.computersculpture.com


#11

Andrew I agree there is more than one way to skin a cat. That’s why
at the beginning of me reply I said it’s my two cents, cause that’s
what it is. BTW I’ve got Rhino and I use it from time to time, but
more oftem than not, I’m in front of ArtCAM. Zach