American Woodworker

Free Product Guide >>

Syndication

 


 

 

 

Woodwork 

Winter 2013-2014

Preview this issue

 

V-Carving in 10 Easy Steps

RATE THIS:

V-Carving in 10 Easy Steps

By Randy Johnson

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.


Step 1

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 shapes.

Click any image to view a larger version.



Step 2

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.



Step 3

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.



Step 4

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.



Step 5

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.



Step 6

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.



Step 7

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.



Step 8

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.



Step 9

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.



Step 10

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.




This story originally appeared in American Woodworker April/May 2011, issue #153.

April/May 2011, issue #153

Purchase this back issue.