How to Create a Drill Hole Feature

Introduction

This tutorial explains how to create a Drill Hole feature, simulate the program, and post NC program or G-code. A few important tips are provided help you get the most out of the BobCAM for SolidWorks CAM system.

Example

Part 1) Open the Example File

1. Click File > Open.
   
   

2. Select HoleExample.SLDPRT (C:\BobCAM Data\BobCAM V**\Examples\HoleExample.SLDPRT).

Part 2) Create a New CAM Job

1. Click the BobCAM Manager tab.
   
   

2. Right-click CAM Defaults, and click New Job.
   
   

3. In the Machining Job dialog box, leave Milling selected as the Job Type.
   
   Click to select the Start Stock Wizard check box.
   
   For this example we use the BC 3X Mill machine.
   
   

4. Click OK to create the Milling Job and open the Stock Wizard.
   
   

5. Click to skip assigning a Workpiece to the job and move to the Stock Specification page.
   
   

6. Under Stock Type, click Cylindrical.
   
   The Auto from Workspace option automatically detects the solid body and creates a bounding stock.
   
   Click Next to go to the Machine Setup.
   
   

7. For this example we use the default settings with the machining origin at the top and center of the stock.

 

Click OK to finish the Machine Setup.

Part 3) Add a Mill Counterbore Hole Feature and Select Geometry

1. In the CAM Tree, right-click Stock and select Blank/Unblank to hide the stock.
   
   

2. Right-click Machine Setup, and click Mill Drill Hole.
   
   The Hole Wizard displays.
   
   

3. Click Select Geometry.
   
   

4. For this example, you could select the lower edge or the cylindrical face of each of the 0.375 drill holes around the perimeter of the part, or you could select CAD features from the Feature Manager design tree.
   
   The benefit of using either of these methods is that a feature is only created for the items you select. There is another method that you can use.
   
   Instead, click the Select Whole Bodies check box, and then select the model.
   
   
   
   

5. To confirm the selection, click OK.

 

When you use Select Whole Bodies for a Mill Drill feature, the software extracts all applicable features and creates a separate feature for each unique hole size.

 

Notice that there are three hole sizes listed in the Hole Sizes list. You can select a hole size in the list to update the Diameter and Depth for each feature as needed.

 

Notice that the Diameter and Depth were automatically set for all features

 

Tip: After inserting a Counter Bore feature, you can modify the assigned feature geometry by right-clicking Geometry and clicking Re/Select from the CAM tree. You can also click the Geometry item to highlight the selected geometry in the graphics area.

 

6. Click Next>> to go to the Feature settings.

Part 4) Define the Feature Parameters

1. Set the desired Rapid Plane and Feed Plane values for the first feature.
   
   

2. You can use the Pick buttons to select geometry to set the Depths and Top of Feature when needed, but no changes are needed for this example.
   
   

3. Through Hole is selected because the Drill hole goes through the part.

 

Click Next>> to go to the Machining Strategy.

Part 5) Define the Machining Strategy

1. Under Template, select Hole.
   
   The default Operation Template contains two operations: Center Drill, and Drill.
   
   

2. To add a chamfer operation, first click to select the Drill operation in the Current Operations list.
   
   

3. In the Available Operations list, select Chamfer Drill, and click (Add Operation).

    

Note: When you add an operation from the Available Operations to the Current Operations, it is added below the currently selected operation.

 

4. Click Apply to All Features.

 

This sets all features in the wizard to use the same operations that were in the Current Operations list. You can see the operations update in the tree on the left.

 

Click Next>> to go to the Postingsettings.

Part 6) Define the Posting Parameters

1. Confirm that the proper Work Offset Number is selected for the feature.

 

Click Next>> twice to go to the Center Drill tool settings.

Part 7) Define the Tool  and Operation Parameters

1. Notice that the System Tool check box is selected.
   
   When using System Tool, the software searches the Tool Crib for a matching tool to set the Center Drill parameters.
   
   If the tools in the Tool Crib have a tool holder assigned in the Tool Library, it is automatically assigned in the wizard.
   
   You can clear the System Tool check box to modify the tool parameters.
   
   

2. For this example we use the default tool holder assignments and tools that are installed with the software.
   
   

3. You can set the Tool Number, Offset Registers, and Feeds and Speeds manually by clearing the check box and typing the values, or you can use the automatically assigned values.
   
   To learn more about setting up the system defaults, view The CAM Defaults.
   
   

4. Click Next>> to go to Parameters.
   
   

5. Set all parameters and repeat this process for the remaining operations making any necessary changes.

 

Tip: You may want to clean up the automatically detected features before and/or after finishing the wizard. For example, there are currently three features in the wizard, if you want to keep the feature to drill the large center hole before pocketing the material, you can delete the Chamfer Drill operation for the 1.5" Diameter feature and update the tool parameters. If you don't want to keep this feature at all, you can delete it from the CAM Tree after finishing the wizard.

 

For this example, the Use Cutting Conditions check box is selected for the Drilling operations to automatically calculate the parameters using the Job Cutting Conditions.

 

6. After defining all of the operation parameters for all features, click Compute to create the toolpath.

 

 

Notice now after finishing the wizard, that three separate features are added to the CAM Tree.

 

7. If any features were created that you don't want to keep, right-click that Feature Mill Hole and click Delete.

 

Editing a Feature

After finishing the wizard, you can right-click Feature Mill Hole and click Edit to modify the feature.

Part 8) Simulate the Program

1. To view the program simulation, right-click Milling Job and click Simulation.
   
   For help with using simulation, view Getting Started With Simulation.
   
   

2. To finish the simulation, in the BobCAM menu, click Exit Simulation.

Part 9) Post the NC Program

1. In the CAM tree, right-click Milling Job, and click Post.

 

The NC program displays in the Posting Manager.

 

You can right-click anywhere in the Posting Manager to access Save As or NC Editor.

Related Topics

Milling Features Overview