How can I create a new custom tool?

If you need to create a new tool that is not one of the standard types, you would create it as a Form Tool. With this feature you can match any router bit that does not have an undercut, such as dovetail bits and Keyhole bits. 

Custom Form Cutters

In this How-To you will see how to add custom form cutters in Aspire and VCarve Pro. Ogee, Roman Ogee, and Round-Over are examples of custom form cutters that can be created, but any custom shaped tool can be created using the steps layed out in this How-To. 
 

Overview: The process for creating a custom form cutter is pretty simple; you need to create a profile of the cutter and then add it to the tool database. 

The Process: In this example you’ll create a Roman Ogee bit. On the right is a picture of the actual bit you’ll create. The key to creating custom form cutters is understanding how the node editing tools work.

  Step 1:

The first thing needed is to create a square that is the dimensions of the profile of the cutter you’re creating. In this example, the roman ogee cutter you’re making is 1.5 inches wide by 0.75 inches high. So you need to create a square 0.75 inches by 0.75 inches (one half the width of the cutter by the height). To create this click the square icon and enter 0.75 for the height and width, and then click ‘Create’ and then click ‘Close’.

 

  Step 2:

Now that you’ve created the square, you need to start editing the nodes to shape the profile of the bit. Select the node-editing icon and then click on the created square. You’ll see four black blocks in each of the corners of the square. Move your mouse over the lower right-hand block and press the ‘D’ key. This will delete the lower right-hand node.
 

 


  Step 3:

The last step will turn your square into a triangle. You need to start dividing up the diagonal line to shape the profile of the cutter you’re creating. The profile you’re creating has three parts to it - two arcs or curves and a notched section in the middle. In order to create the notch in the middle of the cutter, you need to divide the diagonal line up into three parts. To do this, put your mouse over the diagonal line and press the ‘I’ key. Next, move to a different spot on the line and press the ‘I’ key again. You should now have two new nodes on your diagonal line. Note: Notice in the picture how I’ve placed the two new nodes just a little off center on the diagonal line. The closer you can place your nodes to the actual locations they’ll end up, the easier it is the long run. This will become more obvious in the next few steps. 
  

 


  Step 4:

Creating the arcs or curves in the profile is the next step. To do this, move your mouse over the first section of the diagonal line and press the ‘A’ key. Then move your mouse to the third section of the diagonal line and press the ‘A’ key.
  


  Step 5:

This is where things start to look like the actual cutter you’re creating. Click on the different nodes to shape them so they look like the form cutter you want to create. The two arcs or curves need to be moved around and the two nodes you inserted in step 3 need to be moved to create the notch in the middle of the cutter. 
 

 


  Step 6:

When you’re happy with the profile you’ve created, it’s time to create the new tool in Aspire or VCarve Pro. Move your mouse over the top horizontal line of the profile and press the ‘D’ key. This will remove the top line. Next, move your mouse over the left vertical line and press the ‘D’ key. Again, this will remove the line. When creating form cutters in the software, you only need to have the profile of the bit drawn. This is why you removed the other lines.
 

 


  Step 7:

All you should be left with is the profile you created in step 5. Switch into ‘Selection Mode’ by clicking the selection mode icon . Then click on the cutter profile to highlight it. 
 

 


  Step 8:

With the cutter profile selected, go to the tool database by clicking the menu item ‘Edit’, and then selecting ‘Tool Database’. The tool database window should come up. Select the ‘New…’ button in the lower left corner. Now select the ‘Form Tool’ in the Tool Type dropdown box located near the top right of the tool database window.
 

 


  Step 9:

The software now creates the tool. Notice how the full image of the tool is displayed and the diameter is automatically calculated. You can now edit any of the cutting parameters and speeds and feeds for the created tool. You can also give the new tool a name that describes the tool better, for example Roman Ogee – 1.5 inch. When you’re done adjusting everything, press the ‘Apply’ button and the ‘OK’ button.

 


  Step 10:

The only thing that’s left to do is start using your new tool. You can see here what the profile looks like when cut. 

 


Tips and Pitfalls:

  • Make sure that the cutter profile doesn’t cross over the center line or the top line of the tool (the left vertical line or the top horizontal line you deleted in step 6).
  • 0.010” is the smallest diameter custom form cutter you can create in the software. There is no limit on how big the cutter can be, but the larger the cutter, the slower the preview will be.  For most common bit sizes you shouldn’t experience any performance slowdowns.