## RE: [SherlineCNC] Re: True 3D milling using rotary table

Expand Messages
• Kevin:You may be correct, but I am pretty sure that SheetCAM, for instance, is described as a 2-1/2D CAM program, and it can do 3-axis interpolation with no
Message 1 of 17 , Feb 6, 2009
• 0 Attachment
Kevin:

You may be correct, but I am pretty sure that SheetCAM, for instance, is described as a 2-1/2D CAM program, and it can do 3-axis interpolation with no problem.

______________________________________
Andy Wander

-----Original Message-----
From: SherlineCNC@yahoogroups.com [mailto:SherlineCNC@yahoogroups.com] On Behalf Of Kevin Martin
Sent: Friday, February 06, 2009 11:09 PM
To: SherlineCNC@yahoogroups.com
Subject: RE: [SherlineCNC] Re: True 3D milling using rotary table

Hmmm. Not how I recall it.
The stuff you describe, undercuts and side pockets, are 4D+ as they involve rotating the part or the spindle axis as well as needing three linear motions.

If you can see it all from above it is 3D.

If you can see it all from above and each "top" surface you see is at a constant Z, *that* is 2-1/2D; essentially the machine can move in the third dimension (Z) but cannot do so smoothly (or proportionately to X and Y motion) so any sort of ramps or contours are impossible and all cutting motion must occur at constant Z.
-Kevin Martin

-----Original Message-----
From: SherlineCNC@yahoogroups.com [mailto:SherlineCNC@yahoogroups.com] On Behalf Of Andy Wander

2-1/2D is anything you can do with a standard vertical mill, using only the X-Y table, and the Z(spindle) moving up and down.

No pockets on the underside, holes in the sides of the part, or anything else that would require a rotation of the part or one of the axes.

Another way to look at it, if you can see all of the features of the part that need machining, by looking at it from above, then you can do it with 2-1/2D.

------------------------------------

This communication including any attachments, are intended
for the exclusive use of the addressee(s) and contains
distribution or reproduction is strictly prohibited by law
without written permission of Verrex
• I have come to understand (or look at) 2-1/2D milling as even more restrictive than that, specifically being able cut pockets in the z direction of an object,
Message 2 of 17 , Feb 6, 2009
• 0 Attachment
I have come to understand (or look at) 2-1/2D milling as even more
restrictive than that, specifically being able cut pockets in the z
direction of an object, or cut a curved path in the material at some
Z depth, but not having sufficient coordinate independence to machine
any curved 3D surface which could "fall away" on more than 1 axis.
Thus a linearly sloped ramp would be possible and possibly also a
a curved hump of uniform width, but NOT anything like a hemisphere.
This definition may only be a result of the CADCAM software I own,
though. I'm not sure. It is possible, that in practice, it can mean a
number of things, always a product which cannot handle a full set of
NC generation to create any shape at will.
--- In SherlineCNC@yahoogroups.com, Andy Wander <awander@...> wrote:
>
> 2-1/2D is anything you can do with a standard vertical mill, using
only the X-Y table, and the Z(spindle) moving up and down.
>
> No pockets on the underside, holes in the sides of the part, or
anything else that would require a rotation of the part or one of the
axes.
>
> Another way to look at it, if you can see all of the features of the
part that need machining, by looking at it from above, then you can do
it with 2-1/2D.
>
> ______________________________________
> Andy Wander
>
> -----Original Message-----
> From: SherlineCNC@yahoogroups.com
[mailto:SherlineCNC@yahoogroups.com] On Behalf Of tony_dspglobal
> Sent: Friday, February 06, 2009 8:52 PM
> To: SherlineCNC@yahoogroups.com
> Subject: [SherlineCNC] Re: True 3D milling using rotary table
>
> Hi Neil,
>
> I'm new to CAM so I was wondering what is meant by
> "2-1/2D"? I understand 2D and 3D, but what does the 1/2D
> refer to?
>
> Thanks
> Tony
>
>
> --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
> >
> > What is available in the way of routines that might generate G-Code
> > to run an X,Y,Z,A setup to render complex surfaces.
> > Do I really have to write the code line by line? I don't have an
> > immediate projects in mind, but I was wondering if anyone has come up
> > with any solutions to streamline the process. Someone had
> > asked my about making parts, and I mistakenly told him that I had a 3D
> > used the stuff in a while.)
> > --Neil
> >
>
>
>
>
> ------------------------------------
>
>
>
>
> This communication including any attachments, are intended
> for the exclusive use of the addressee(s) and contains
> confidential or copyrighted materials. Duplication,
> distribution or reproduction is strictly prohibited by law
> without written permission of Verrex
>
• ... Neil, Now that the discussion on 2 1/2D CAD is done, I think your question was actually about CAM programs. There are many options out there, including
Message 3 of 17 , Feb 7, 2009
• 0 Attachment
--- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@...> wrote:
>
> What is available in the way of routines that might generate G-Code
> to run an X,Y,Z,A setup to render complex surfaces.
> Do I really have to write the code line by line? I don't have an
> immediate projects in mind, but I was wondering if anyone has come up
> with any solutions to streamline the process. Someone had
> used the stuff in a while.)
> --Neil
>
Neil,

Now that the discussion on 2 1/2D CAD is done, I think your question
was actually about CAM programs. There are many options out there,
including writing your own G-code, but I think there are limits to how
intricate you might want to go. For example, I've got Gcode files
that are hundreds of k-bytes, or megabytes, thousands of lines. I
have no desire to do that by hand!

I would say to look at, in no particular order: Deskproto and
Protowizard (popular in jewelry and other intricate 3D shapes), Vector
Deskproto, and do jewelry, which is what generates the huge files, up
to several megabytes. It's what happens when you're moving a .003"
diameter cutter around a complex design.

What I'd like to see is real simultaneous use of all four axes of an
X, Y, Z, A CNC mill. I have not seen any that do.

Hope that helps,
Bob
• ... This simultaneous X-Y-Z-A is called 4 axis machining, and is usually not used, rather a 5th axis is included to assure that enough reach is available
Message 4 of 17 , Feb 7, 2009
• 0 Attachment
--- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@...> wrote:
>
> What is available in the way of routines that might generate G-Code
> to run an X,Y,Z,A setup to render complex surfaces.
> Do I really have to write the code line by line?

This simultaneous X-Y-Z-A is called 4 axis machining, and is usually
not used, rather a 5th axis is included to assure that enough "reach"
is available through the software. This software will provide
services such as the ability to insert a complex tool and holder into
a "bottle" shape, carve out the inside, and not permit the tool shank
or tool holder to come in contact with the mouth of the bottle.
Another service is to keep a constant tangential angle between a ball
nosed cutting tool and the angle of a swept surface. This permits
maximum feed rates and yields the best surface finish because the
center of the tool ( spinning at 0 SFM) is never used for cutting.
The complexity of these kind of tasks, the few potential
installations, and the heavy product support requirement make for
expensive software costs. Usually in excess of \$10,000, plus hefty
annual maintenance charges.

There are many sub-optimal ( compared to the above examples)
solutions that provide nearly the same results at a much lower cost.

1) 3D surface machining is free to inexpensive, depending on the
level of control you want to accept.

For example there is a free version of 3D surface machining called
Freemill from Mecsoft ( \$\$\$\$ Rhino Cam, \$\$\$\$ Visual Mill). It will
only make finish passes of rectangular patches, to get you to buy the
more expensive software.

3D surface machining is usually done with a ball nosed cutter, which
is used to carve a 3D shape from a solid block of material. In
jewelry making ( of wax casting patterns), the ball nosed cutter is
replaced with a Sharp V-tipped cutter with a small flat on the end (
think .005-.010 inch). A great many small incremantal passes are
made and the shape "appears" as if it had been embedded in the
substrate.

With some shapes, it is possible to machine the top and bottom,
utilizing indexing pins or vises ( or a rotary indexer that can
position 180 degrees on command). Attachment tabs are needed to
control the time that the part breaks free from the surrounding
material. Some programs provide this automatically, but it is also
very simple to add these to a 3D model.

Most hobby class 3D machining CAM programs use STL files, which are
triangulated approximations ( but accurate) of the mathematical
curves of the surfaces. Some use "polygonized" DXF files too. A few
can directly process nurbs surfaces in iges or Rhino 3dm files ( like

If you want to do 3D surface machining, you have to have 3D models.
These can be obtained from a couple of service bureaus, some freely
data, or designed with 3D cad programs. You can also combine these

Look at MOI - Moment of Inspiration for an inexpensive 3D solid
modeler. It currently sells for under \$200, and has lots of features
and capabilities that were previously only available at much higher
prices ( Rhino 3D at \$600-\$800 was a popular 3D modeling program), or
with very limited capabilities or cryptic interfaces.

2) Now for rotary axis uses: On a Sherline about the most complicated
that you will find in general use is rotary 4th axis machining.
(There are a couple of 5 axis machines around, I know of one for sure
that appeared at last years CNC-Workshop.) This consists mostly of 2
1/2 axis machining interspersed with rotary indexing. Drill some
holes, mill a flat, pocket a shape, index 90 or 180 degrees and then
drill some more holes, mill a flat, pocket a shape, etc. Indexing
consists of a single command A90.000 or A180.000, so most people
don't need any special cam software to use this kind of setup. You
can use this method to mill features on the surface of hex stock, or
even to make hex stock.

The next most popular rotary axis application is engraving on a
cylinder. This is easily accomplished by wiring the rotary axis(A)
to the Y motor and cutting a flat layout 2 1/2 axis program. Some
mathmatical scaling is involved to set up your machine, but it's not
rocket science and you do NOT need any special CAM software.

For Sherline machines, probably the next most popular application is
to cut gears or sprocket shapes for power transmission. These are
usually a simple set of g-code commands that are repeatedly run
between indexes, equal to one tooth of motion. A bevel gear requires
2 simultaneous axes of motion ( X and A, like a thread) , but not 4

For those making jewelry with a rotary axis, DeskCNC ( \$250) has a
routine that zig-zags back and forth along the rotational axis ( X-Z
contouring) between tiny angular indexes of an stl file, creating a
3D shape.

The next step up would be to cut a 3D surface with climb milling
only, and using rotary contouring. An example part would be a liquid
flow device that required a high polish and toolmarks only in the
direction of a helix. Examples are injection molder screws, jet
engine impellors, and maybe a couple of others. You can create a
helix shaped toolpath using the Totem pole function in StlWork,and
then create 3 axis( X-Z-A) rotary toolpaths with Vector cad-cam for
under \$1000.

As you can see the rotary applications are very part specific and
most Sherline users will never use more than one or two of the
methods.

One last thing about rotary axis machining. Generally it is better
to mount your part onto the table of a mill than between a rotary
table and tailstock, because the part is more stable. This means
that you can take heavier cuts and worry less about chatter, tool
breakage, and part movement from cutting tool pressure.

3) 2 1/2 axis machining, generally refers to the ability of a CAM
program to produce X-Y contouring code, inter mixed with Z plunges
and retractions. It usually refers to drilling, flat( planar)
contouring ( like engraving), and pocketing. The processes usually
can have multiple cuts to the final depth. There should be no lines
of G-code that contain X, Y, and Z simultaneous motion. ( non-modal
code however will have all three address words on the same line, even
though one or more may not be moving)

That having been said, Sheetcam is a 2 1/2 axis program. It does
have a couple of 3D machining funcitons like corner sharpening and
tapered tabbing, but it does NOT create 3D surface machining of
sculpted surfaces with ball nosed end mills.

Another thing that tends to differentiate 2 1/2 axis machining from 3
axis machining is the actual tools used for the two processes. Again
generally, if you are using a square cornered tool like an end mill
or an angled tool like a drill or engraving bit or corner chamfering
tool, this will be referred to as 2 1/2 axis. If you are using a
full radius cutter to carve out a sculpted 3D surface, this would be
3 axis machining, even though the g-code may consist entirely of 1 or
2 axis motion per line. Most 3D surface machining consists of zig-
zag, raster patterns with X-Z codes for the contours interspersed
with small Y movements for each pass back and forth.

In most cases the original part design can be represented by a flat
drawing with no Z depth, and the programmer adds the desired Z-depth
to the g-code as part of the programming process. With 3 axis
programming, the original model is a 3D surface, and the toolpaths
are developed based on te programmer providing the radius of the ball
nosed tool tip.

Fred Smith - IMService
http://www.imsrv.com
• Thanks Bob. My thought was based on the notion that if programs were specifically designed for X,Y,Z,A CAM that certain shapes could be distilled down to
Message 5 of 17 , Feb 7, 2009
• 0 Attachment
Thanks Bob.

My thought was based on the notion that if programs were specifically
designed for X,Y,Z,A CAM that certain shapes could be distilled
down to relatively simple routines, when the desired goal was a
carefully chosen subset of the whole specrum of possible shapes.
Certainly, it seems easier to me to write G-Code by hand to machine a
hemisphere, for example, if one of the axes were rotary. Your work on
jewelry sounds like you accomplish some pretty fancy stuff, and I will
indeed look into DeskProto, DeskCNC, etc.

Thanks again,
Neil
--- In SherlineCNC@yahoogroups.com, "montanaaardvark"
<boblombardi@...> wrote:
>
> --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
> >
> > What is available in the way of routines that might generate G-Code
> > to run an X,Y,Z,A setup to render complex surfaces.
> > Do I really have to write the code line by line? I don't have an
> > immediate projects in mind, but I was wondering if anyone has come up
> > with any solutions to streamline the process. Someone had
> > asked my about making parts, and I mistakenly told him that I had a 3D
> > used the stuff in a while.)
> > --Neil
> >
> Neil,
>
>
> Now that the discussion on 2 1/2D CAD is done, I think your question
> was actually about CAM programs. There are many options out there,
> including writing your own G-code, but I think there are limits to how
> intricate you might want to go. For example, I've got Gcode files
> that are hundreds of k-bytes, or megabytes, thousands of lines. I
> have no desire to do that by hand!
>
> I would say to look at, in no particular order: Deskproto and
> Protowizard (popular in jewelry and other intricate 3D shapes), Vector
> Deskproto, and do jewelry, which is what generates the huge files, up
> to several megabytes. It's what happens when you're moving a .003"
> diameter cutter around a complex design.
>
> What I'd like to see is real simultaneous use of all four axes of an
> X, Y, Z, A CNC mill. I have not seen any that do.
>
>
>
> Hope that helps,
> Bob
>
• One of the issues, it seems to me, that is confusing the discussion is the Subject: True 3D using the rotary table . 3 Dimensional milling means machining
Message 6 of 17 , Feb 7, 2009
• 0 Attachment
One of the issues, it seems to me, that is confusing the discussion is the
Subject: 'True 3D using the rotary table'. 3 Dimensional milling means
machining with moves in 3 axis. These are usually the x, y, and z axis. The
rotary table adds an axis, not a dimension. In certain situations, the y
axis is mapped to the rotary, this is still 3D, X, A, and Z, again 3 axis
moving. There is true 4 axis machine as well as 5 axis units. There are
some interesting youtube videos of 5 axis machining.
Now the problem is for 3 axis machining, there are many CAM programs
to generate the G Code. However, a CAM package that generates true 4 axis G
code, is usually outside the budget range of a Sherline CNC user. I have
seen small shop packages in the past that advertises they supply 4 axis
moves, but usually in small print, there is a disclaimer that it is
'underdevelopment'. I would like to be proven wrong. Now once up in the
commercial area, \$4,000 and up (way up) there are many CAM programs
available.
I do some '4 axis' machining on a CNC mill (Tormach) by mounting a
part blank on a rotary table and performing 3 axis machining on one face of
the part then rotating the part, doing some more machining, rotating the
part, etc. Technically this is 3 and 1/2 axis machining and is done by
concatenating chunks of code for each face into one long part program.

Dennis in Houston

> -----Original Message-----
> From: SherlineCNC@yahoogroups.com [mailto:SherlineCNC@yahoogroups.com]
> On Behalf Of Neil Albert
> Sent: Saturday, February 07, 2009 5:24 PM
> To: SherlineCNC@yahoogroups.com
> Subject: [SherlineCNC] Re: True 3D milling using rotary table
>
> Thanks Bob.
>
> My thought was based on the notion that if programs were specifically
> designed for X,Y,Z,A CAM that certain shapes could be distilled
> down to relatively simple routines, when the desired goal was a
> carefully chosen subset of the whole specrum of possible shapes.
> Certainly, it seems easier to me to write G-Code by hand to machine a
> hemisphere, for example, if one of the axes were rotary. Your work on
> jewelry sounds like you accomplish some pretty fancy stuff, and I will
> indeed look into DeskProto, DeskCNC, etc.
>
> Thanks again,
> Neil
> --- In SherlineCNC@yahoogroups.com, "montanaaardvark"
> <boblombardi@...> wrote:
> >
> > --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
> > >
> > > What is available in the way of routines that might generate G-Code
> > > to run an X,Y,Z,A setup to render complex surfaces.
> > > Do I really have to write the code line by line? I don't have an
> > > immediate projects in mind, but I was wondering if anyone has come up
> > > with any solutions to streamline the process. Someone had
> > > asked my about making parts, and I mistakenly told him that I had a 3D
> > > used the stuff in a while.)
> > > --Neil
> > >
> > Neil,
> >
> >
> > Now that the discussion on 2 1/2D CAD is done, I think your question
> > was actually about CAM programs. There are many options out there,
> > including writing your own G-code, but I think there are limits to how
> > intricate you might want to go. For example, I've got Gcode files
> > that are hundreds of k-bytes, or megabytes, thousands of lines. I
> > have no desire to do that by hand!
> >
> > I would say to look at, in no particular order: Deskproto and
> > Protowizard (popular in jewelry and other intricate 3D shapes), Vector
> > (has CAD and CAM), BobCAD/CAM and DeskCNC. I'm currently running
> > Deskproto, and do jewelry, which is what generates the huge files, up
> > to several megabytes. It's what happens when you're moving a .003"
> > diameter cutter around a complex design.
> >
> > What I'd like to see is real simultaneous use of all four axes of an
> > X, Y, Z, A CNC mill. I have not seen any that do.
> >
> >
> >
> > Hope that helps,
> > Bob
> >
>
>
>
>
> ------------------------------------
>
>
>
>
• Fred, Thank you for such a marvelous tutorial. I am going to copy it right away to my PC for my reference. An extremely valuable piece I would say, your
Message 7 of 17 , Feb 7, 2009
• 0 Attachment
Fred,

Thank you for such a marvelous tutorial. I am going to copy
it right away to my PC for my reference. An extremely valuable
piece I would say, your explanation.

Thanks again,
Neil
--- In SherlineCNC@yahoogroups.com, "Fred Smith" <imserv@...> wrote:
>
> --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
> >
> > What is available in the way of routines that might generate G-Code
> > to run an X,Y,Z,A setup to render complex surfaces.
> > Do I really have to write the code line by line?
>
> This simultaneous X-Y-Z-A is called 4 axis machining, and is usually
> not used, rather a 5th axis is included to assure that enough "reach"
> is available through the software. This software will provide
> services such as the ability to insert a complex tool and holder into
> a "bottle" shape, carve out the inside, and not permit the tool shank
> or tool holder to come in contact with the mouth of the bottle.
> Another service is to keep a constant tangential angle between a ball
> nosed cutting tool and the angle of a swept surface. This permits
> maximum feed rates and yields the best surface finish because the
> center of the tool ( spinning at 0 SFM) is never used for cutting.
> The complexity of these kind of tasks, the few potential
> installations, and the heavy product support requirement make for
> expensive software costs. Usually in excess of \$10,000, plus hefty
> annual maintenance charges.
>
> There are many sub-optimal ( compared to the above examples)
> solutions that provide nearly the same results at a much lower cost.
>
> 1) 3D surface machining is free to inexpensive, depending on the
> level of control you want to accept.
>
> For example there is a free version of 3D surface machining called
> Freemill from Mecsoft ( \$\$\$\$ Rhino Cam, \$\$\$\$ Visual Mill). It will
> only make finish passes of rectangular patches, to get you to buy the
> more expensive software.
>
> 3D surface machining is usually done with a ball nosed cutter, which
> is used to carve a 3D shape from a solid block of material. In
> jewelry making ( of wax casting patterns), the ball nosed cutter is
> replaced with a Sharp V-tipped cutter with a small flat on the end (
> think .005-.010 inch). A great many small incremantal passes are
> made and the shape "appears" as if it had been embedded in the
> substrate.
>
> With some shapes, it is possible to machine the top and bottom,
> utilizing indexing pins or vises ( or a rotary indexer that can
> position 180 degrees on command). Attachment tabs are needed to
> control the time that the part breaks free from the surrounding
> material. Some programs provide this automatically, but it is also
> very simple to add these to a 3D model.
>
> Most hobby class 3D machining CAM programs use STL files, which are
> triangulated approximations ( but accurate) of the mathematical
> curves of the surfaces. Some use "polygonized" DXF files too. A few
> can directly process nurbs surfaces in iges or Rhino 3dm files ( like
>
> If you want to do 3D surface machining, you have to have 3D models.
> These can be obtained from a couple of service bureaus, some freely
> downloaded from the internet, can be created from 3D surface scanned
> data, or designed with 3D cad programs. You can also combine these
> techniques to create your model.
>
> Look at MOI - Moment of Inspiration for an inexpensive 3D solid
> modeler. It currently sells for under \$200, and has lots of features
> and capabilities that were previously only available at much higher
> prices ( Rhino 3D at \$600-\$800 was a popular 3D modeling program), or
> with very limited capabilities or cryptic interfaces.
>
> 2) Now for rotary axis uses: On a Sherline about the most complicated
> that you will find in general use is rotary 4th axis machining.
> (There are a couple of 5 axis machines around, I know of one for sure
> that appeared at last years CNC-Workshop.) This consists mostly of 2
> 1/2 axis machining interspersed with rotary indexing. Drill some
> holes, mill a flat, pocket a shape, index 90 or 180 degrees and then
> drill some more holes, mill a flat, pocket a shape, etc. Indexing
> consists of a single command A90.000 or A180.000, so most people
> don't need any special cam software to use this kind of setup. You
> can use this method to mill features on the surface of hex stock, or
> even to make hex stock.
>
> The next most popular rotary axis application is engraving on a
> cylinder. This is easily accomplished by wiring the rotary axis(A)
> to the Y motor and cutting a flat layout 2 1/2 axis program. Some
> mathmatical scaling is involved to set up your machine, but it's not
> rocket science and you do NOT need any special CAM software.
>
> For Sherline machines, probably the next most popular application is
> to cut gears or sprocket shapes for power transmission. These are
> usually a simple set of g-code commands that are repeatedly run
> between indexes, equal to one tooth of motion. A bevel gear requires
> 2 simultaneous axes of motion ( X and A, like a thread) , but not 4
>
> For those making jewelry with a rotary axis, DeskCNC ( \$250) has a
> routine that zig-zags back and forth along the rotational axis ( X-Z
> contouring) between tiny angular indexes of an stl file, creating a
> 3D shape.
>
> The next step up would be to cut a 3D surface with climb milling
> only, and using rotary contouring. An example part would be a liquid
> flow device that required a high polish and toolmarks only in the
> direction of a helix. Examples are injection molder screws, jet
> engine impellors, and maybe a couple of others. You can create a
> helix shaped toolpath using the Totem pole function in StlWork,and
> then create 3 axis( X-Z-A) rotary toolpaths with Vector cad-cam for
> under \$1000.
>
> As you can see the rotary applications are very part specific and
> most Sherline users will never use more than one or two of the
> methods.
>
> One last thing about rotary axis machining. Generally it is better
> to mount your part onto the table of a mill than between a rotary
> table and tailstock, because the part is more stable. This means
> that you can take heavier cuts and worry less about chatter, tool
> breakage, and part movement from cutting tool pressure.
>
> 3) 2 1/2 axis machining, generally refers to the ability of a CAM
> program to produce X-Y contouring code, inter mixed with Z plunges
> and retractions. It usually refers to drilling, flat( planar)
> contouring ( like engraving), and pocketing. The processes usually
> can have multiple cuts to the final depth. There should be no lines
> of G-code that contain X, Y, and Z simultaneous motion. ( non-modal
> code however will have all three address words on the same line, even
> though one or more may not be moving)
>
> That having been said, Sheetcam is a 2 1/2 axis program. It does
> have a couple of 3D machining funcitons like corner sharpening and
> tapered tabbing, but it does NOT create 3D surface machining of
> sculpted surfaces with ball nosed end mills.
>
> Another thing that tends to differentiate 2 1/2 axis machining from 3
> axis machining is the actual tools used for the two processes. Again
> generally, if you are using a square cornered tool like an end mill
> or an angled tool like a drill or engraving bit or corner chamfering
> tool, this will be referred to as 2 1/2 axis. If you are using a
> full radius cutter to carve out a sculpted 3D surface, this would be
> 3 axis machining, even though the g-code may consist entirely of 1 or
> 2 axis motion per line. Most 3D surface machining consists of zig-
> zag, raster patterns with X-Z codes for the contours interspersed
> with small Y movements for each pass back and forth.
>
> In most cases the original part design can be represented by a flat
> drawing with no Z depth, and the programmer adds the desired Z-depth
> to the g-code as part of the programming process. With 3 axis
> programming, the original model is a 3D surface, and the toolpaths
> are developed based on te programmer providing the radius of the ball
> nosed tool tip.
>
> Fred Smith - IMService
> http://www.imsrv.com
>
• Hi Guys, I have been using a Sherline lathe (manual not CNC) for a few months and am now interested in getting a mill as I now see that a lathe on its own has
Message 8 of 17 , Feb 8, 2009
• 0 Attachment
Hi Guys,

I have been using a Sherline lathe (manual not CNC) for a few months and am
now interested in getting a mill as I now see that a lathe on its own has a
limited area of work.

I think that CNC is the way I should be thinking for the mill and I would

5410A-CNC Mill
Gecko G540 controller
?? Stepper motors

I have an early copy of Corel Draw (Ver 6) which I know reasonably well. Is
this the sort of thing that I need?.

I would like a European source for the Stepper Motors if possible for lower
shipping costs.

I have a range of possible laptops/Desktop computers as I am in that

Is there anything else I should include? Any other accessories from Sherline
as its much cheaper to get it in one shipment.

Regards,
Hamilton
• Not to belabor the subject, but perhaps my question would have been better served had I said A,Y,Z which would be cylindrical coordinates. If programs which
Message 9 of 17 , Feb 9, 2009
• 0 Attachment
Not to belabor the subject, but perhaps my question would have been
better served had I said A,Y,Z which would be cylindrical coordinates.
If programs which maintained these axes in trigonometric (sin, cos,
etc.) relationships, then a means to create (some)3D surfaces could be
accomplished relatively mimimal resources.
--- In SherlineCNC@yahoogroups.com, "Fred Smith" <imserv@...> wrote:
>
> --- In SherlineCNC@yahoogroups.com, "Neil Albert" <neil@> wrote:
> >
> > What is available in the way of routines that might generate G-Code
> > to run an X,Y,Z,A setup to render complex surfaces.
> > Do I really have to write the code line by line?
>
> This simultaneous X-Y-Z-A is called 4 axis machining, and is usually
> not used, rather a 5th axis is included to assure that enough "reach"
> is available through the software. This software will provide
> services such as the ability to insert a complex tool and holder into
> a "bottle" shape, carve out the inside, and not permit the tool shank
> or tool holder to come in contact with the mouth of the bottle.
> Another service is to keep a constant tangential angle between a ball
> nosed cutting tool and the angle of a swept surface. This permits
> maximum feed rates and yields the best surface finish because the
> center of the tool ( spinning at 0 SFM) is never used for cutting.
> The complexity of these kind of tasks, the few potential
> installations, and the heavy product support requirement make for
> expensive software costs. Usually in excess of \$10,000, plus hefty
> annual maintenance charges.
>
> There are many sub-optimal ( compared to the above examples)
> solutions that provide nearly the same results at a much lower cost.
>
> 1) 3D surface machining is free to inexpensive, depending on the
> level of control you want to accept.
>
> For example there is a free version of 3D surface machining called
> Freemill from Mecsoft ( \$\$\$\$ Rhino Cam, \$\$\$\$ Visual Mill). It will
> only make finish passes of rectangular patches, to get you to buy the
> more expensive software.
>
> 3D surface machining is usually done with a ball nosed cutter, which
> is used to carve a 3D shape from a solid block of material. In
> jewelry making ( of wax casting patterns), the ball nosed cutter is
> replaced with a Sharp V-tipped cutter with a small flat on the end (
> think .005-.010 inch). A great many small incremantal passes are
> made and the shape "appears" as if it had been embedded in the
> substrate.
>
> With some shapes, it is possible to machine the top and bottom,
> utilizing indexing pins or vises ( or a rotary indexer that can
> position 180 degrees on command). Attachment tabs are needed to
> control the time that the part breaks free from the surrounding
> material. Some programs provide this automatically, but it is also
> very simple to add these to a 3D model.
>
> Most hobby class 3D machining CAM programs use STL files, which are
> triangulated approximations ( but accurate) of the mathematical
> curves of the surfaces. Some use "polygonized" DXF files too. A few
> can directly process nurbs surfaces in iges or Rhino 3dm files ( like
>
> If you want to do 3D surface machining, you have to have 3D models.
> These can be obtained from a couple of service bureaus, some freely
> downloaded from the internet, can be created from 3D surface scanned
> data, or designed with 3D cad programs. You can also combine these
> techniques to create your model.
>
> Look at MOI - Moment of Inspiration for an inexpensive 3D solid
> modeler. It currently sells for under \$200, and has lots of features
> and capabilities that were previously only available at much higher
> prices ( Rhino 3D at \$600-\$800 was a popular 3D modeling program), or
> with very limited capabilities or cryptic interfaces.
>
> 2) Now for rotary axis uses: On a Sherline about the most complicated
> that you will find in general use is rotary 4th axis machining.
> (There are a couple of 5 axis machines around, I know of one for sure
> that appeared at last years CNC-Workshop.) This consists mostly of 2
> 1/2 axis machining interspersed with rotary indexing. Drill some
> holes, mill a flat, pocket a shape, index 90 or 180 degrees and then
> drill some more holes, mill a flat, pocket a shape, etc. Indexing
> consists of a single command A90.000 or A180.000, so most people
> don't need any special cam software to use this kind of setup. You
> can use this method to mill features on the surface of hex stock, or
> even to make hex stock.
>
> The next most popular rotary axis application is engraving on a
> cylinder. This is easily accomplished by wiring the rotary axis(A)
> to the Y motor and cutting a flat layout 2 1/2 axis program. Some
> mathmatical scaling is involved to set up your machine, but it's not
> rocket science and you do NOT need any special CAM software.
>
> For Sherline machines, probably the next most popular application is
> to cut gears or sprocket shapes for power transmission. These are
> usually a simple set of g-code commands that are repeatedly run
> between indexes, equal to one tooth of motion. A bevel gear requires
> 2 simultaneous axes of motion ( X and A, like a thread) , but not 4
>
> For those making jewelry with a rotary axis, DeskCNC ( \$250) has a
> routine that zig-zags back and forth along the rotational axis ( X-Z
> contouring) between tiny angular indexes of an stl file, creating a
> 3D shape.
>
> The next step up would be to cut a 3D surface with climb milling
> only, and using rotary contouring. An example part would be a liquid
> flow device that required a high polish and toolmarks only in the
> direction of a helix. Examples are injection molder screws, jet
> engine impellors, and maybe a couple of others. You can create a
> helix shaped toolpath using the Totem pole function in StlWork,and
> then create 3 axis( X-Z-A) rotary toolpaths with Vector cad-cam for
> under \$1000.
>
> As you can see the rotary applications are very part specific and
> most Sherline users will never use more than one or two of the
> methods.
>
> One last thing about rotary axis machining. Generally it is better
> to mount your part onto the table of a mill than between a rotary
> table and tailstock, because the part is more stable. This means
> that you can take heavier cuts and worry less about chatter, tool
> breakage, and part movement from cutting tool pressure.
>
> 3) 2 1/2 axis machining, generally refers to the ability of a CAM
> program to produce X-Y contouring code, inter mixed with Z plunges
> and retractions. It usually refers to drilling, flat( planar)
> contouring ( like engraving), and pocketing. The processes usually
> can have multiple cuts to the final depth. There should be no lines
> of G-code that contain X, Y, and Z simultaneous motion. ( non-modal
> code however will have all three address words on the same line, even
> though one or more may not be moving)
>
> That having been said, Sheetcam is a 2 1/2 axis program. It does
> have a couple of 3D machining funcitons like corner sharpening and
> tapered tabbing, but it does NOT create 3D surface machining of
> sculpted surfaces with ball nosed end mills.
>
> Another thing that tends to differentiate 2 1/2 axis machining from 3
> axis machining is the actual tools used for the two processes. Again
> generally, if you are using a square cornered tool like an end mill
> or an angled tool like a drill or engraving bit or corner chamfering
> tool, this will be referred to as 2 1/2 axis. If you are using a
> full radius cutter to carve out a sculpted 3D surface, this would be
> 3 axis machining, even though the g-code may consist entirely of 1 or
> 2 axis motion per line. Most 3D surface machining consists of zig-
> zag, raster patterns with X-Z codes for the contours interspersed
> with small Y movements for each pass back and forth.
>
> In most cases the original part design can be represented by a flat
> drawing with no Z depth, and the programmer adds the desired Z-depth
> to the g-code as part of the programming process. With 3 axis
> programming, the original model is a 3D surface, and the toolpaths
> are developed based on te programmer providing the radius of the ball
> nosed tool tip.
>
> Fred Smith - IMService
> http://www.imsrv.com
>
Your message has been successfully submitted and would be delivered to recipients shortly.