My inspiration for this project came from a wooden
chain I made years ago using a handheld plunge router
and plans from Patrick Spielman’s New Router Handbook
(1993). Since making the chain involved routing
a bunch of the same parts, it seemed like a good project
for a CNC. Patrick used a one-link-at-a-time routing
jig setup that partly relied on the router’s base to
hold the links steady during routing—something not
possible with a CNC. So making the links on the CNC
became a good exercise in designing CNC small parts
jigging. I had three goals in mind while developing the
jigs. I wanted them to be simple to make, easy to use,
and sufficiently durable. Aft er trying various methods
involving clamps and hold-downs, I settled on a combination
of recessed cutouts, wedges and small turnbuckles.
But the real secret to these jigs came from the
CNC’s ability to easily and precisely create matching
parts that fit snugly together like puzzle pieces.
Click any image to view a larger version.
Jig 1: Routing Inside the Links
Rather than make this jig out of separate pieces of wood, I found it easier to rout it as a recess in a piece of MDF. I used three
wedges to hold the workpiece in place while routing. The bottom wedge forced the workpiece tight against the upper end of the
jig, while the two side wedges pushed the workpiece to the left. The wedges were also created with the CNC, so matching the
tapers in the recess to the angle of the wedges was a breeze. The wedges have a 1 in 20 taper, which made them easy to secure
and remove with a couple stiff mallet taps. The wedges proved very secure, as they never once vibrated loose during routing. I
also routed an undercut around the bottom of the recess with a T-slot router bit. The undercut insured that the workpiece didn’t
hang up on any stray wood chips at the bottom of the jig.
Jig 2: Routing Outside the Links
Creating the second jig required the most experimenting. I initially created it as a recess similar to jig 1, but the MDF proved
too weak and the center posts easily broke off. A piece of Baltic birch plywood glued to the top of the MDF created a much
stronger jig. I made the center posts .05" shorter than the thickness of the work piece. This made it easy to apply pressure with
the turnbuckles. The center posts were also .05" smaller in diameter than the inside of the links. This slight gap was needed so the
workpiece could slide onto the posts without binding, but was still snug enough to prevent the workpiece from shifting during
routing. A couple workpieces were slightly warped, which made them hard to slip on to the center posts. A few taps from a mallet
solved that problem. Once the links were routed into separate parts, they were easily removed.
Rounding Over the Outside
Jig 2 served a dual purpose. Once all the links were routed into
separate parts, I switched to an ovolo bit and rounded over the
outside corners. The links were flipped over to do the other side.
The snug fit on the center posts and the turnbuckles helped to
hold the link securely in place for this step.
Only Three Bits are Required
The 1/2" dia. straight bit did the heavy work of removing
stock from both the jigs and the chain links. The slotting bit
created the undercut at the bottom of jigs 1 and 2 to prevent
stray wood chips from getting in the way. The 1/4" radius
ovolo bit gave the links their round shape.
Jig 3: Rounding Over the Inside
Similar to the first jig, the third jig used wedges in a recess to hold the parts in place. This jig really took advantage of the CNC’s
ability to cut parts that fit together like a glove. The recessed pockets for the links were cut the same size as the link, without any
clearance gap. This created a very snug fit and required a couple extra mallet taps on the wedges to make sure the links were fully
seated. This snug fit insured that the links didn’t move or vibrate while I rounded over the inside corners. After the first side was
done, I flipped the links over to rout the other side.
Note: Although CNC’s are capable of precise machining, you should always test your setups and adjust the dimensions of your
jigs, parts and tool paths to accommodate slight variations in materials and bit diameters.
A Quick Sanding
Sanding each link took a minute or two per link, but
removing the machine marks at this stage was easier than
doing it after assembly. Next time I’ll use a flap sander or
inflatable drum sander and save my finger tips.
Break Every Other Link
A quick hit with a mallet was all it took to crack the links
in half. I used quartersawn boards for this project because
when broken, they tend to create flatter joints than
plainsawn wood. The flat joints made reassembly easier.
Glue and Clamp Back Together
I assembled the chain by adding two unbroken links to each broken link. Then I assembled these three link sections with
more broken links until the chain was complete. Because the links were broken on the grain, the glue joints were nearly or
completely invisible. Using a light application of glue and removing the squeeze out while it was still soft made cleanup
sanding easy. After it was done, I dipped the chain in an oil finish a couple of times and rubbed it dry with a cloth.
The six links started out as a board measuring 5/8" x 2" x 20". The .6" spacing between the links provided the necessary
clearance for the 1/2" dia. straight bit and the bottom end of the ovolo bit. The six links produced 11-1/2" of finished chain.
Drawings for the three jigs can be downloaded at AmericanWoodworker.com/CNC.
This story originally appeared in American Woodworker June/July 2012, issue #160.
CNC routers are opening up lots of new ways to create
textures in wood. Here are my three favorite ways
of creating textures using a CNC. Th e fi rst method uses
the repetition of shapes to create a design that is routed
using one or more bits. If you enjoy doodling patterns,
this is a technique that you will enjoy. Th e second
method uses programming built in to the design soft -
ware to generate a texture design that simulates a handcarved
pattern. Th e third texturing method starts with
a photograph and converts the light and dark areas into
the routing paths. Each method has a few basic rules to
follow, but add some imagination and the variations you
can achieve are virtually limitless. I used Vectric Aspire
CNC design soft ware to create the textures for this article,
but other soft ware packages such as ArtCAM and
EnRoute can also be used to create textures.
Shape-based textures are created by repeating
a pattern of either asymmetrical or symmetrical
shapes. Patterns can be hand-drawn or drafted with
a CAD program such as Google SketchUp. Hand
drawn designs need to be scanned or digitally
photographed so they can be imported into the
CNC design program. CNC design programs are
also capable of creating shape-based patterns. One
creative aspect of this type of texturing is that you
can rout on the lines or between them to achieve
different effects. I routed the crackle texture shown
below using a 1/4" dia. 60° v-bit. It took about 60
minutes to carve the design into this 10" cherry lid.
The dome shape of the lid was created first using a
1/4" dia. ball nose bit.
Click any image to view a larger version.
Using the built-in texturing program that comes with most CNC
design software packages is an easy way to create a simulated
hand-carved texture. As shown in the program window to the left,
there are several options to choose from when designing this type
of texture. Adjusting these variables enables you to create a wide
variety of simulated hand-carved textures, ranging from those with
long, closely spaced cuts, to those with short, widely spaced cuts—
and anything in between. Once the options are selected, the
program creates a semi-random pattern of lines (see middle image
below) for the router bit to follow. I used the settings shown here to
create texture on the walnut lid show below. I used a 1/4" ball nose
bit to create the texture, but other profiles such as straight bits or
v-bits can also be used, expanding your options even further. It
took about 60 minutes to carve the texture shown below.
Another way to create a CNC texture is to start with a photo.
Not all photos work equally well, however. That’s because
the CNC design software reads the light areas as high points
and the dark areas as low points and tells the CNC router to
carve accordingly. A good photo image is one that is evenly
lit without long shadows, but yet has good contrast. As you
can see in the alligator skin photograph below, the highlights
accent similar areas, while the dark areas are consistent in
the rest of the photo. This type of photo will create a texture
that closely resembles the contours of the original. Carving a
photo-based texture requires the use of a small ball nose bit to
attain the details. For the design below, I first roughed out the
texture and dome shape of the lid with a 1/4" ball nose bit and
then carved the final shape and details using a 1/8" ball nose
bit. It took about two hours to do the final routing and about
the same amount of time for the roughing passes.
Shape-based textures can take many forms, from low relief
to high relief, and from subtle to bold. The three textures
above are just a sampling of options that are possible with this
approach to designing textures for the CNC. The one on the left
was created using a collection of small circles that were then
routed around with a 60° v-bit. The middle design is simply an
array of concentric squares, while the one on the right uses a
grid pattern made with a 120° v-bit.
Software-based textures are the easiest—and often
the fastest—to create, and can be run on top of a shape
(left), around a shape (middle), or overlapping in different
directions (right). These options allow you to be selective
and creative in where and how the texture is applied.
Using different bits will also expand the variations you
can create with this method of texturing.
Photo-based textures are an easy way to simulate existing
textures—as seen in these three examples. The weathered
end grain (left) shows a surprising amount of detail, as
does the cloth texture (right). The stones (middle) create
an interesting pattern, although they are rendered quite
flat. Additional depth can be added to the stones through
the use of other modeling tools, if so desired. The thing to
remember about creating textures from photos is to
always start with a photo that has even contrast.
This story originally appeared in American Woodworker April/May 2012, issue #159.
A rotary indexing head allows a CNC machine to
create 3-dimensional shapes in the round. It’s an accessory
that can be added to most CNC machines. Some companies
even make it as a stand alone machine. A rotary
indexing head looks similar to a standard woodturning
lathe, but its approach to shaping wood is quite different.
In fact, it’s more like milling than woodturning. One
of the best features of a rotary indexing head is its ability
to create shapes that aren’t easily turned on a standard
wood lathe, such as this hexagonal chisel handle. Intricate
round relief carvings are also possible. Because it’s CNC
based, a rotary indexing head is capable of great precision
and easy repeatability. However, since the shaping is done
with a router bit in small increments (as small as 1/50" per
pass), the milling process can take a while to complete.
Machining this chisel handle took about 2-1/2 hours, but
its unique shape was intriguing to design and mill. It also
makes an attractive addition to my tool box.
You need to think a little differently.
CNC turnings usually start out as a flat design, so the first step is to “unwrap” the cylindrical profile. CNC design software
uses a variety of drawing tools that assist this process. One tool automatically calculates the flat design’s width, based on the
maximum diameter you specify for the turning. Another tool takes complex shapes such as the hexagonal cross section of
this handle and converts it into the flat shape.
Click any image to view a larger version.
The design software converts (wraps) the flat design into its cylindrical shape to give you a preview of the final piece.
Each part of a CNC turning is created separately. The parts are then joined to create the final design. The basic steps used to
design this chisel handle appear below.
Basic Parts Creation
Each 3-dimensional part is created using a line drawing of its cross section to extrude (or “sweep”) the shape along a path. The
tapered tenon and the round pommel are extruded across the width of their designs, while the body of the handle is extruded
along the length of its design. The handle’s contoured hexagonal body is created using three different cross sections and a
software tool (or “gadget”) that automatically unwraps the hexagonal shape into its corresponding flat shape.
Parting tabs are added to the ends of the final design to connect the part to the unmachined ends of the billet. The tabs are
created using the same drawing tools used to create the tapered tenon and the round pommel.
Basic Machine Steps
Step 1: Create a cylinder
The first step is to round off corners of the
billet to create a cylinder. The CNC design
software includes a gadget that automatically
calculates the cutting paths needed to
remove the corners, based on the dimensions
of the square billet and the finished diameter
of the cylinder. To create the hexagonal chisel
handle I started with a 2" square billet and
rounded it to 1-3/4" diameter using a 1/4" dia.
bullnose bit. Rounding this 22" long cylinder
takes about 20 minutes.
Rough rout the shape
The same 1/4" bullnose bit roughs out the
handle’s hexagonal shape. In this case, the
cutting passes are programmed to run the
length of the cylinder and remove a 1/8"
deep x 1/8" wide a strip of material with each
pass. The last pass leaves 1/32" of material to
be removed in the next step. Roughing out
this shape takes about 25 minutes.
Finish rout the final shape
The final (finishing) pass removes the last
1/32" of material and leaves a smooth
surface. To do this, the 1/4" bullnose bit is
programmed to “step over” each previous
pass by only 1/50". This tiny step-over
leaves a surface that’s easy to clean up
with 180 grit sandpaper. This finishing pass
takes about 50 minutes to complete.
The surface of a CNC turning can be
embellished with additional details, including
lettering. For this chisel handle I combined
a 60° V-bit and a script-style font to create
a look similar to metal engraving or laser
etching. These finely detailed 3/4" tall
letters demonstrate the precision of a CNC’s
operation. Routing them takes only a minute.
This story originally appeared in American Woodworker February/March 2012, issue #158.
V-carving is one of the simplest ways to create
attractive carvings on a CNC router. With special
software and a little practice, it’s possible to transform
almost any lettering style or 2D design into a
carving that requires only minimal cleanup before
finishing. I use V-Carve Pro software from Vectric,
but the steps are similar with other v-carving programs.
The software tells the machine to raise the
bit at the inside corners; the machine then uses the
tip of the v-bit to create corners that are clean and
crisp—as opposed to the rounded corners made by
a handheld router guided by a template. For more
examples of v-carving visit AmericanWoodworker.com/CNC.
Layout your design. All it takes is a
simple hand sketch or photograph.
This can be imported directly into the
program and then outlined using the
drawing tools in the v-carve design
program. Since both letters and shapes
can be carved, there are not many limits
to the kinds of designs you can v-carve.
You also have the choice of carving
on the inside or outside of letters or
Click any image to view a larger version.
Make sure all shapes are closed.
This is one of the cardinal rules of
v-carving design. A circle, square or the
outline of an object qualifies, but a single
line or parallel lines with open ends will
not work. The v-carve programs need
a continuous outline to follow. Some
outlines may look continuous, but even a
little break in the line will cause problems.
Fortunately, v-carve programs are able
to recognize shapes that have small
openings and will automatically close
them for you.
Set the cutting depth for the
background of your carving and
the inside of the letters (as needed).
This cutting depth is mainly a design
decision, and of course it cannot
exceed the thickness of your board.
The cutting preview (example at
right) will show you how your chosen
cutting depth looks.
Select your router bits. Use a straight bit first to rout flat areas. The diameter of this bit
determines how much cleanup the v-bit will need to do inside a corner. A large diameter
straight bit removes material faster but leaves more for the v-bit to cleanup. A small
diameter straight bit leaves less material inside a coner but takes longer to clear the flat
areas. I typically use a 1/4" diameter end mill for drawer front or cabinet door carvings.
The three most common v-bit angles are 60°, 90° and 120°. I prefer using a 90° and
120° v-bit for wide or large letters and a 60° v-bit for small or fine letters. If possible, I also prefer to use a v-bit with a cutting radius that’s slightly wider than the width of the final bevel. This allows me to make one final cleanup pass (if needed) to remove any step
marks left by the initial passes.
Create cutting paths for the recessed background and export them from your v-carving design program
to your CNC machine. The cutting paths (shown above in red with tiny arrows) show the areas that will be
routed. Here I’m using a 1/4" end mill bit to rout the flat background area. I’m accomplishing this with 1/8"
wide passes (shown by the distance between the red lines). This dimension is referred to as the “stepover”
measurement. The cutting depth per pass can also be programed, as can the feed (travel) rate of the router,
expressed in inches per minute.
Rout the recessed background area. To ensure a smooth background on
this plaque, I used a couple techniques. First, I routed the background area
in two .06" (about 1/16") deep passes, plus a light .01" pass to reach the final
depth of .013". Three passes take more time than one, but create a surface
that requires only light sanding. Second, I programed the router to cut with
the grain (see Step 5). This reduces sanding, too. Milling the background for
this plaque took about 20 minutes.
Create cutting paths for the bevels around the shapes (the hand plane and perimeter rectangle in this
case) and export them to your CNC machine. For this design, I will be using a 90° v-bit, which produces a
45° bevel. The shaded areas above the handle and below the depth-adjustment knob are closely-spaced
tool paths where the v-bit needs to make many close passes to mill the background flat. These areas are too
narrow for the 1/4" end mill bit to get into.
Rout the bevels around the shapes. This requires removing the straight bit and installing the
appropriate v-bit. I used a 1/2" diameter 90° v-bit. It has a 1/4" tall bevel—more than enough for the
carved bevel, which will be only 1/8" tall. This step took about 20 minutes to rout. Except for some light
hand sanding and a little touch-up with a carving chisel, this part of the carving is now complete.
Create tool paths for the lettering. This requires a separate step because I’m changing to a 60° v-bit. I
prefer a 60° bit for small letters such as these because it creates a deeper, more distinctive v-groove than a
90° bit. The tool paths above show how v-carving requires two lines to carve between. The two lines are
parallel in these letters, but they can be any shape or spacing. For example, the outline of the hand plane
and outer rectangle represents the pair of lines that were used to create the hand plane carving.
Rout the lettering. Notice that “No. 4” is routed into the surface of the plane whereas as the logo is
carved into the background. I programed the difference in cutting depth into the cutting paths while
designing the plaque. This final carving step took about 8 minutes. To view a video on how I designed
and machined this plaque from start to finish, visit AmericanWoodworker.com/CNC.