[Jewelry making - Article 01150] - Re: [Orchid] CNC Wax Masters

[Neil George]

========[ Invite a Friend - http://www.ganoksin.com/invite.htm  ]========


    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 information. 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


____________________________________________________________________
T h e   O r c h i d   L i s t
Open Electronic Forum for Jewelry Manufacturing Methods and Procedures
____________________________________________________________________
Orchid FAQ:
~ http://www.ganoksin.com/orchid/faq.htm
Orchid Archives:
~ http://www.ganoksin.com/orchid/archive
Orchid Galleries:
~ http://www.ganoksin.com/orchid/gallery.htm
Invite a Friend:
~ http://www.ganoksin.com/invite.htm
____________________________________________________________________
Tips From The Jeweler's Bench - Article Archive
~ http://www.ganoksin.com/borisat/tip_sear.htm
The Jeweler's Selected Bibliography List
~ http://www.ganoksin.com/jewelry-books
Buy Orchid Jewelry:
~ http://www.ganoksin.com/shop
____________________________________________________________________
-Unsubscribe:
-Email: orchid-request AT ganoksin.com Body=unsubscribe subject=blank
____________________________________________________________________