VCarve Pro How-To's

Creating inlays is made possible by using the Offset Selected Vectors option. This is one of VCarve Pros more powerful and time saving tools.

To allow a male insert to fit into a female pocket the vector geometry needs to be modified to remove all external and internal corners from the shape. This requires the cutter radius to be applied to the corner regions on a design.

For this example lets use a 0.25" Endmill. The cutter radius (R) would then be 0.125"

The manual offsetting process is as follows,

1. Select and offset the original vector OUT by R (0.125")

2. Select the newly created vector from step 1 and offset it IN by 2 times R (0.25")

3. Select the vector from step 2 and offset it OUT by R (0.125")

Remember the new vector created in each step needs to be selected after each offset operation

The final new offset vector is then used to calculate 2D Machining toolpaths,

The Pocket / recessed cavity toolpath
The Profile Outside toolpath for the male / insert

Important - both toolpaths need to be created using the same diameter cutter.

The following picture shows the original vector geometry in black with the new result from the offsetting operation in dotted blue line. Notice the rounded inner and outer corners on the new vector. This is what makes it possible to create the inlay.

Click For A Larger View

One of the great features of VCarve Pro is the ability to combine VCarving with 2D machining. This can create some stunning effects, a good example is the Howling Wolf Inn sign. By combining VCarve toolpaths, flat depth machining and 2D pocketing some amazing 3D effects can be achieved.

The following video shows the steps needed to layout and machine the Howling Wolf Inn Sign in VCarve Pro.

Video Demo - Howling Wolf Inn Sign

VCarve Pro does excellent job of vectorizing image files ready for machining.

Open an existing file or create a New one.

Import the raster image - bmp, jpg, tif, gif, png

Click Twice on the image to allow the image to be moved / positioned within the design.

With the image selected open the Fit Vectors to Bitmap form and experiment with the options.

For more details about tracing / vectorizing images see,

Tracing Image Files (4.1Mb video)

Tracing Image Files (1Mb PDF)  

For this example a VCarve Pro Dinosaur cutout will be used to demostrate how to scale 2D parts to match any material thickness and in this case part slot width.

The 0.375" thick version of the Dino file can be downloaded from,

Dino design for 3/8" thick material (1MB)

In this example the original file is setup for .0.375" Thick material to scale it up for 0.5" Thick material the following steps are taken,

1. Open the 'Dino 0.375 inch matl.crv' file

s 2. Select all the vectors by Ctrl + A or clicking Top left and Bottom right corners

3. Scale the Vectors - select the Scale Selected Vectors icon

4. Select the 'Specify the exact size' checkbox

  To determine the new size we need to calculate the percent increase. In this case the material thickness is increasing from 0.375" to 0.5" or a 33.33% increase in material thickness. The current width is 38.1039", this needs to increase by 33.33%. The new width will then end up 50.804 (38.1039 X 1.3333)

4. Enter new width, In the width box enter 50.804” The height will scale automatically. Then click Apply and then Close

5. Edit the Material size - From the Main menu select

   Edit > Material Width = 52” and Height = 36”
   Thickness = 0.5”
   Check Center vectors in material

6. Edit each Toolpath in turn by double clicking on the names

   Enter Cut Depth = 0.5”
   Specify the Pass Depth and Feedrates required
   Calculate the new toopaths

7. Save the Toolpaths for your CNC machine control type.

Scaling projects up or down can come in very handy allowing you to easily and quickly adjust for a wide range of material sizes.