Mill Express CAD Tutorial

Introduction

This topic explains how to create the CAD model for the Mill Express demonstration file. The design process includes using the Shape Library, 2D Boolean, and other wireframe functions to create the profile, pocket, and holes for the model. The wireframe is then extruded to create a boss, and the pocket and holes are removed from the boss using extruded cuts.

This tutorial highlights the following features of the BobCAD-CAM software:

• Using the Shape Library

• Utilizing entity colors and CAD layers to aid in geometry selection

• Creating Hole Patterns

• Creating and managing CAD layers

• Deleting geometry

• Using 2D Boolean to add wireframe chains

• Using Quick Trim

• Using Extrude Curve

• Using the Snap Increment to eliminate data entry changes

• Using Extrude Cut

• Creating chamfers with Solid Chamfer

• Using Tangent Propagation to your advantage

Part 1) Open the Template File and Save As

A template file is provided so that you can have the same system colors as shown in this tutorial. We start by opening the template file and renaming it to keep the original file unchanged. It is good practice to always begin a file by saving it with an appropriate name and location and then saving often.

1. In the Quick Access Toolbar, at the top left of the application, click Open an existing document.
   
   
2. Navigate to C:\BobCAD-CAM Data\BobCAD-CAM **Current Version**\Examples\Demo Files, and select Getting Started Template.bbcd.
   
   
3. Click Open.
   
   
4. In the Quick Access Toolbar, click Save As.
   
   
5. Select or create a new folder to save to, or just use the Demo Files folder.
   
   
6. In the File Name box, type Mill Ex CAD, and click Save.

Part 2) Create Wireframe with the Shape Library

We use the Shape Library to quickly create wireframe geometry that is modified later.

1. In the Shapes group of the Create 2D ribbon, click Shape Library.
   
   The Data Entry Manager is populated with the data for the default shape.
   
   
2. Click the image of the Disk shape in the Data Entry Manager.
   
   A dialog presenting the available shapes appears.
   
   
   
   
3. Select the ring shape.
   
   The Ring parameters open in the Data Entry Manager.
   
   
4. In the Data Entry Manager, update the parameters as follows:
   
   
   • 1 = 4.000
   • 2 = 2.250
     
     

Note: Notice that the CAD preview of the shape updates as you define the Data Entry parameters. The CAD preview allows you to confirm the desired result before creating the shape.

5. Click OK to create the shape.
   
   The Shape Library feature is added to the CAD Tree.
   
   
6. Click Cancel to close the Data Entry Manager.
   
   

Part 3) Create a Layer with a Different Color

Next we create a layer and assign a color to it. This assists in geometry selection later in the tutorial.

1. Select the Use Layer Attributes toggle button in the quick access toolbar of the Layers Manager.
   
   
   
   
2. Right-click in the Layers Manager, and select Add New Layer.
   
   
   
   A new layer is created with the name, Layer-1, highlighted to allow for edits, and is set to the active layer automatically.
   
   
3. To name the layer, type Outer.
   
   The name is automatically updated once focus is placed on another area, or function.
   
   
4. In the Color column of the Outer layer, click the down arrow on the icon.
   
   
5. In the color palette, select the purple color from the Standard Color row.
   

Tip: With Use Layer Attributes selected, the color and line style set for an individual layer will automatically be set as the active attributes when that layer is active.

Part 4) Create a Hole Pattern

Now we use a hole pattern to easily create a circular pattern of holes.

1. In the Pattern group of the Create 2D ribbon, click Hole Pattern.
   
   

2. Update the Data Entry parameters:
   
   

   • Diameter = 4.000

   • Number of Holes = 6

   • Hole Diameter = 0.500

   • Select the check box for Break Arc
     
     

3. Click OK to create the hole pattern.

Change the Active Layer

Before creating another hole pattern, we change back to our original layer.

1. In the Active Layer column, click the CAD row to set that as the active layer.
   
   The active color automatically updates to match that of the CAD layer.
   
   

Tip: New layers are created with attributes matching that of the active layer. By quickly switching to this layer prior to making another layer, we save ourselves the time of having to change the active color after creating the layer.

Part 5) Create a CAD Layer

Using CAD layers is a great way to keep your drawings organized. This helps with geometry selection and provides a convenient way to hide and show geometry.

1. In the quick access toolbar of the Layers Manager, click the New Layer button.
   
   
   
   A new layer is created with the name, Layer-2, highlighted to allow for edits, and is set to the active layer automatically.
   
   

2. To name the layer, type Holes.
   
   The name is automatically updated once focus is placed on another area, or function.
   

Part 6) Create a Hole Pattern

Now we create the second hole pattern, which is later used to extrude cut holes into the model.

Important: Generally, when you modify the Data Entry settings for a CAD function, such as Hole Pattern, they are retained until you change them again or close the file or software. After closing a file and/or the software, the Data Entry settings return to their default values. In this example, we only instruct you to change values as needed, based on this understanding. So, when defining the Hole Pattern explained next, all settings should be the same as the previous Hole Pattern, and you should only update the values as explained. (For example, Break is still selected from the previous pattern.)

1. Change the Hole Diameter to 0.250, and press Tab to update the CAD preview.
   
   

2. Click OK.
   
   

3. Click Cancel.
   
   
   
   

4. In the Quick Access Toolbar, click Save.
   
   

Part 7) Delete Geometry

This part shows you how to delete existing wireframe geometry.

1. In the document toolbar, click Select Mode to enter selection mode.
   
   

2. Click, or drag a window, to select the small ( 0.250 diameter) circle at the three o' clock position.
   
   
   
   

3. Press the Delete key. (Alternatively, in the Home ribbon, click Delete).
   
   

Change the Active Layer

We only want the second hole pattern on the Holes layer, so now we set the CAD layer as active.

1. In the Layers Manager, click in the Active Layer column of the CAD row to make this the active layer.

Notice the check mark () indicates the active layer.

Part 8) Add Wireframe Chains with 2D Boolean

Next we boolean two closed wireframe chains to begin defining the outside profile for the model.

1. In the Boolean group, of the Create 2D ribbon, click 2D Boolean.
   
   Notice that Add is selected in the Data Entry Manager, and the First Geometry Group list has focus.
   
   

2. Click to select the largest circle as the first closed chain.
   
   
   
   The geometry is added to the First Geometry Group list.
   
   

3. Click in the Second Geometry Group list to give it focus.
   
   

4. In the Quick Selection group of the Home ribbon, click the down arrow under Pick By Layer, and click Pick By Color.
   
   The Select Color dialog appears.
   
   

5. Click the purple color.
   
   

6. Click OK.
   
   Notice that all matching geometry is selected, and added to the Second Geometry Group list.
   
   Notice that the preview is updated as well.
   
   
   
   

7. Click OK.
   
   
   
   

8. Click Cancel.
   
   

9. Press Ctrl+S to save the file.
   

Part 9) Create Rectangles

The next steps involve creating two rectangles that are used to complete the outer profile and the pocket.

1. In the Shapes group of the Create 2D ribbon, click Rectangle.
   
   
2. The Rectangle dialog appears in the Data Entry Manager with the Rectangle Center Creation Option selected.
   
   

• In the Dimensions group:
  
  
  • Length = 4.000
  • Width = 2.500
    
    
• In the Base Point group: 
  
  
  • X = 0.000
  • Y = 0.000
  • Z = 0.000
    
  • Option = (Left)
    
    
• In the Corner Type group:
  
  
  •   (Radius) = 0.250
    
    

3. Click OK to create the first rectangle.
   
   
   
   
4. Update the Data Entry parameters:
   
   
   • Length = 3.000
   • Width = 1.750
     
     

5. Click OK to create the second rectangle.
   
   
   
   

6. Click Cancel.

Part 10) Add Wireframe Chains with 2D Boolean

We use 2D Boolean again to finish creating the outer profile.

1. In the Boolean group, of the Create 2D ribbon, click 2D Boolean.
   
   The 2D Boolean dialog launches in the Data Entry Manager with the Add Type selected.
   
   

2. By default, the Picking Manager is set to Auto-Connection, make sure the Tangent Propagation option is off, and click the outer arc to select the entire chain.
   
   
   
   The entities are added to the First Geometry Group list.
   
   
3. Click in the Second Geometry Group list to give it focus.
   
   
4. Chain select the larger rectangle.
   
   
   
   
5. Click OK.
   
   The Wireframe updates in the graphics area, and a 2D Boolean is added to the CAD Tree.
   
   

Part 11) Use Quick Trim

Now we take a moment to use the wireframe trimming tool, Quick Trim. Quick Trim is one of the many useful trimming tools in BobCAD-CAM, and it allows you to delete whole entities or trim them to the intersection of other entities.

1. In the Trim Extend group, of the Utilities ribbon, click Quick Trim.
   
   Click all of the entities that are inside of the circle and rectangle, in the center of the part, until you have created a single profile for the pocket. (There are seven total selections.)
   
   
   
   
   
   

2. Click Cancel.
   
   

3. Save the file.

Part 12) Create a Solids Layer and Set Active Layer

In this part, we create a layer place our solid model on. One method of utilizing layers is to create them as needed for certain entities, or groups of entities, to organize your drawings.

1. Right-click in the Layers Manager, and click Add New Layer.
   
   The layer is created as the active layer, with the name highlighted to allow for edits.
   
   

2. Type Solids to name the layer.
   

Part 13) Create an Extrude Boss

We now extrude our wireframe profile to create the main body of our solid model.

1. Press Ctrl+7 to select the ISO2 view. (Alternatively, in the Document Toolbar, click the icon.)
   
   

2. In the Extrude group of the Create 3D ribbon, click Extrude Curve.
   
   

3. Chain select the outer profile.
   
   
   
   The Preview updates.
   
   
   
   

4. Click the upper (positive) sketch handle to activate sketching.

Move the sketch handle down past the selected geometry and into the negative (other) direction.

Tip: In this step, we are dragging the extrusion preview from the positive direction down into the negative (other) direction. When you reach the geometry, the positive distance becomes zero, and BobCAD-CAM automatically switches from the positive sketch handle to the negative sketch handle to allow you to easily change the extrusion direction.

Notice that the Data Entry parameters automatically update while moving the sketch handles. Now we utilize the snap increment to get the exact value without the need for data entry.

5. Move the sketch handle until the Distance value (under Other Direction) becomes 0.750, and click to anchor the sketch handle.
   
   
6. Click OK.

The solid is created in the graphics area, and an Extrude Curve feature is added to the CAD Tree.

Part 14) Create an Extrude Cut

The next steps show how to use Extrude Cut to cut the pocket and holes into the model.

Cut the Pocket

1. In the Extrude group of the Create 3D ribbon, click Extrude Cut.
   
   
2. In the Positive Direction group, update the Distance to 0.000.
   
   The Distance, in the Other Direction group, is automatically given a value of 1.000.
   
   
3. Update the Distance, in the Other Direction group, to 0.500.
   
   

4. Click in the graphics area to give it focus, and press S to turn off the shaded view.

Tip: The Shaded and Transparent view options can be utilized to aid in the selection of surface edges, or as in this example, wireframe that is on a surface. You can press S or T to toggle these view options.

3. Select the wireframe profile of the pocket.
   
   The Preview updates automatically.
   
   

4. Press S to turn on the shaded view.
   
   
   
   

5. Leave the Scope setting to All Bodies and click OK.
   The solid is updated, and an Extrude Cut feature is added to the CAD Tree.
   
   

   
   

Note: The Extrude Cut dialog is left open for the following step.

Cut the Holes

1. In the Quick Selection group of the Home ribbon, click the down arrow for Pick By Layer, and select Pick By Layer.
   
   The Select Layer dialog appears, allowing you to choose which layers entities you would like to select.
   
   

2. Select Holes, and click OK.
   
   
   
   The CAD preview is updated automatically.
   
   

3. Use the lower sketch handle to extend the extrude completely through the part.

    

Tip: When creating through holes with Extrude Cut, it is generally not important that the Distance values are exact. You can either type the exact value, or use sketch handles to extrude up to, or past, the surface you are cutting.

4. Click OK.
   
   The solid is updated, and an Extrude Cut feature is added to the CAD Tree.

Part 15) Create a Solid Chamfer

The final step of creating our model is to apply a small chamfer to the internal pocket edge using solid fillet.

Hiding Layers

We hide the layers that contain our wireframe geometry as it isn't needed anymore, and because we need to select the surface edges of the pocket (not the wireframe used to create it).

1. Click the CAD layer to highlight it.
   
   
2. Hold down Ctrl and select the Outer, and Holes layer to highlight them as well.
   
   
3. Right-click one of the highlighted layers and select Hide Layer.
   
   All highlighted layers are hidden, leaving the Solids layer as the only visible layer.
   

Using Tangent Propagation

When creating solid fillets or chamfers, you can reduce the number of selections needed by using Tangent Propagation. Tangent Propagation automatically applies (propagates) the fillet to any edges that are tangent to your selections. In this part, we show that you only need to select two of the six edges to apply a chamfer around the entire pocket.

1. In the Corner group of the Create 3D ribbon, click Solid Chamfer.
   
   

2. Change the Chamfer value to 0.050.
   
   Notice that Tangent Propagation is selected by default.
   
   

3. Click to select the circular edge at the top of the model.

Tip: The circular edge is selected because it forms sharp corners with the edges on either side of it. Any other edge can be selected next, and Tangent Propagation automatically applies the chamfer to the entire pocket. (If the sharp corners were made with a small radius instead, only one edge would need to be selected.)

5. Select any other surface edge at the top of the pocket.
   
   
   
   

6. Click OK.
   
   The solid is updated, and a Solid Fillet feature is added to the CAD Tree.
   
    
   
   

7. Click Cancel.
   
   

8. Save the file.

Congratulations! You have finished the Mill Express CAD model.

Next Topic

To learn how to machine the model, view the Mill Express CAM Tutorial.