Vectric Forum

Visit the User Forum where both existing and prospective customers discuss Vectric software. More>



Determine which of the Vectric software products is best suited for your CNC requirements More>

Aspire & VCarve Pro How-To's


3D Bevel Profile Machining

In this How-To, you’ll see how to create 3D Bevel Profile machining. You’ll see how to create cut-out beveled objects along with pocketed beveled objects in Aspire and VCarve Pro.

Overview: 3D Bevel Profile machining in Aspire and VCarve Pro allows you to create a bevel or a chamfer around vectors, with sharp internal and square external corners.
 

Example 1:


The Process: In this example, you’ll create the text ‘VCP’, add a 3D Bevel Profiling on the letters, and then cut them out. On the right is a picture of what you’re going to create.

  Step 1:

For this example, create a new project with a material size of 15 inches by 10 inches and a thickness of 0.5 inches.


  Step 2:

Click the ‘Draw Text Within A Vector Box’ icon . In the text area type ‘VCP’, and set the text alignment to ‘Center’ and the margin size to ‘Normal’. Notice how VCarve Pro has automatically entered the width and height as the dimensions of the material size set in Step 1. Click ‘Apply’ and then ‘Close’.


  Step 3:

With the text vectors from Step 2 selected, click the ‘Create Profile Toolpath’ from the toolpaths tab. Select to use a 0.5 inch 90 degree V-bit for the tool, with a cut depth of 0.2 inches. Click to machine ‘Outside’ the vectors and make sure you’ve checked both the ‘Sharp external corners’ and ‘Sharp internal corners’ check boxes. Note: Notice the amount in the ‘Allowance for cut out tool’ box. 0.2 inches is the distance you’ll need to have the cut-out tool be offset from your beveling. By offsetting the cut-out tool, you avoid cutting into your beveling.
 


  Step 4:

You’ll now see the 3D View screen and the beveling toolpath. Click back to the 2D view and select the vectors for the text you created in step 2. You need to create a toolpath around these vectors to cut them out. Click the ‘Create Profile Toolpath’ icon . The cut depth for this example should be 0.5 inches, and the tool will be a 0.25 inch end mill bit. Make sure you select to machine ‘Outside’ the vectors and to check the ‘Sharp external corners’ box. Also, you must enter the ‘Allowance offset’ of 0.2 inches that you got from Step 3. Click the ‘Calculate’ button to create this tool path.
 


  Step 5: If you haven’t already, you can preview the entire job in the 3D view by clicking ‘Preview All Toolpaths’.
 

 
 

Example 2:


The Process: In this example, you’ll create the text ‘VCP’, add a 3D Bevel Profiling on the letters, and then pocket cut around them. On the right is a picture of what you’re going to create.

  Step 1:
For this example, create a new project with a material size of 15 inches by 10 inches and a thickness of 0.5 inches.

  Step 2:

Create a boundary or a square to define where you want the texturing to be. To do this, click the square icon and enter 14 inches for the width and 9 inches for the height, then click ‘Create’ and then click ‘Close’.


  Step 3:

In ‘Selection’ mode , select the square you created in Step 2. Click the ‘Draw Text Within A Vector Box’ icon . In the text area, type ‘VCP’, and set the text alignment to ‘Center’ and the margin size to ‘Normal’. Notice how VCarve Pro has automatically entered the width and height as the dimensions of the square from Step 1. Click ‘Apply’ and then ‘Close’.
 


  Step 4:

With the text vectors from Step 3 selected, click the ‘Create Profile Toolpath’ from the toolpaths tab. Select to use a 0.25 inch 60 degree V-bit for the tool with a cut depth of 0.2 inches. Click to machine ‘Outside’ the vectors and make sure you’ve checked both the ‘Sharp external corners’ and ‘Sharp internal corners’ check boxes. Note the amount in the ‘Allowance for cut out tool’ box. 0.1155 inches is the distance you’ll need to have the cut out tool be offset from your beveling.
 


  Step 5: You’ll now see the 3D View screen and the beveling toolpath. Click back to the 2D view and select the vectors for the text you created in step 2. You need to create a toolpath around these vectors to create the square external corners. Click the ‘Create Profile Toolpath’ icon . The cut depth for this example should be 0.4 inches and the tool will be a 0.125 inch end mill bit. Make sure you select to machine ‘Outside’ the vectors and to check the ‘Sharp external corners’ box. Also, you must enter the ‘Allowance offset’ of 0.1155 inches that you got from Step 4. Click the ‘Calculate’ button to create this tool path.
 

  Step 6: Next you need to create an offset around your text, to prevent the pocketing toolpath from cutting into the 3D Bevel Profile. To create the offset, select the text you created in Step 3 while in ‘Selection Mode’ , and then click the ‘Offset’ icon . Select offset ‘Outwards’, enter 0.115 for the distance, press ‘Offset’, and then click ‘Close’.
 

  Step 7: Creating a pocketing toolpath is next. Select the square vectors and the offset vectors text you created in Step 6. The easiest way to do this is to press ‘CTRL-A’, and then while holding the ‘Shift’ key down, click on the original text vectors. Now you should have just the offset vectors and the square selected. Click the ‘Pocket Toolpath’ icon . Set the cut depth to 0.4 inches and the tool to a 0.125 inch ball nose bit. Click ‘Calculate’ to generate the toolpath.
 

  Step 8: If you haven’t already, you can preview the entire job in the 3D view by clicking ‘Preview All Toolpaths’
 

 
 

Tips and Pitfalls:

  • The key to successful 3D Bevel Profile machining is to set the correct ‘Allowance Offset’. VCarve Pro calculates this for you when you create your beveling toolpath, which makes it pretty easy.
  • The smaller the bit you use to do your cutout path, the better detail you’ll get for your internal corners.
  • Notice how in Example 1, the ‘Allowance offset’ was 0.2 inches for a 90 degree v-bit at 0.2 inches cut depth. But at the same cut depth of 0.2 inches, the ‘Allowance offset’ for a 60 degree v-bit was 0.1155 inches. As the angle of the bit changes, so should the ‘Allowance offset’.

Final Thoughts: There are two key steps to both of these examples. One is using the ‘Allowance offset’ that is automatically calculated by the software. The second is to make sure you check the ‘Sharp external corners’ and ‘Sharp internal corners’ boxes when creating your beveling toolpath and ‘Sharp external corners’ on your offset toolpath.

< Go Back


© Copyright Vectric Ltd. All rights reserved.