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This topic explains how to create the CAD model for the Mill 3 Axis Pro demonstration file. The design process includes first creating a model with solid primitives and then subtracting it from a cube to create the cavity. Finally, the drill holes are created with extruded cuts.
This tutorial highlights the following functionality of the BobCAD-CAM software:
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 File menu, click Open.
Navigate to C:\BobCAD-CAM Data\BobCAD-CAM V28\Examples\Demo Files, and select Getting Started Template.bbcd.
Click Open.
2 In the File menu, click Save As.
Select or create a new folder to save to, or just use the Demo Files folder.
In the File Name box, type Mill 3XP CAD, and click Save.
The first cylinder is created along the X-axis, and we utilize the Side UCS to easily create the cylinder in the desired orientation.
1 In
the 
UCS Manager, right-click Side
(Y/Z) and click Active UCS.
2 In the View menu, point to Views, and click ISO1.
Now we create three cylinders to start defining the initial solid model.
1 In the Solids menu, click Cylinder.
Set the Data Entry parameters as follows:
Radius = 1.000
Height = 6.500
Origin Z = -3.250
To create the first cylinder, click OK.
2 Click the radius sketch handle and move it outward to increase the radius of the next cylinder.
Watch the Radius value in the Data Entry Manager change as you move the sketch handle. You can see that the snap increment is active, because the Radius value updates using the current snap increment value. The snap increment allows us to get the exact value during sketching, thus reducing data entry modifications.
3 Click to anchor the sketch handle when the Radius value is 0.1250.
Now, repeat this process to decrease the height of the cylinder.
Click to anchor the sketch handle when the Height value becomes 0.5000.
4 Click OK.
5 Click anywhere in the Workspace, to give it key focus, and press Ctrl+1 to select the Top View. (Alternatively, in the View menu, point to Views and click Top.)
6 Use the origin handle to roughly place the next cylinder.
Update the Data Entry parameters:
X = 0.000
Y = 0.000
Z = 2.750
Click OK.
7 Click Cancel.
Press Ctrl+S to save the file.
NOTE: Notice
that there are three Solid items in the 
Solids folder
of the CAD Tree. You can click each Solid item to highlight the solid
in the Workspace.
Using layers is a great way to keep your CAD files organized. One successful method is to place wireframe geometry on one layer and solid geometry on another layer. This is helpful for hiding, showing, and selecting geometry.
1 Right-click
anywhere in the 
Layers Manager window, and
click Add New Layer.
2 To name the layer, type Wireframe, and press Enter.
3 Right-click Wireframe, and click Active Layer.
Next we create an arc that is extruded to create a tapered boss in the center of the part.
1 In the View menu, point to Views, and click ISO1.
2 In the Arcs menu, click Coordinates.
Update the Data Entry parameters:
Center Z = -1.250
Radius = 1.375
Click OK.
3 In
the Layers Manager, right-click CAD
and click Active Layer.
In this part, we extrude the arc to create a tapered boss, which also merges the intersecting solids into a single solid body.
1 In the Solids menu, click Extrude Boss.
2 Click the arc to select it.
Click 
.
(The CAD preview displays.)
Under Positive Direction:
Distance = 0.375
Draft Angle = 10.000
Under Other Direction:
Distance = 0.375
Draft Angle = 10.000
3 Click OK.
Click Cancel.
NOTE: Notice that the Solids folder now contains only one Solid item.
The Extrude Boss function merges all intersecting solids into a single solid body.
4 Right-click the Wireframe layer, and click Hide.
In the File menu, click Save.
We create the next set of solid primitives using the front plane.
1 In the UCS Manager, right-click Front (X/Z) and click Active UCS.
Now we create the final three cylinders for the initial solid model.
1 In the Solids menu, click Cylinder.
2 Update the Data Entry parameters:
Radius = 0.750
Height = 4.500
Origin
X = 1.000
Y = 0.000
Z = -2.250
Click OK.
3 Update the Data Entry parameters:
Radius = 1.000
Height = 0.375
Origin
X = 1.000
Y = 0.000
Z = -2.250
Click OK.
4 Update the Data Entry parameters:
Origin
X = 1.000
Y = 0.000
Z = 1.875
Click OK.
5 Click Cancel.
Save the file.
NOTE: Notice that there are now four Solid items in the Solids folder.
In this part, we add the four separate solids to make a single solid body. This part finalizes the initial solid model so it can be used with solid subtract to create the cavity.
1 In the Solids menu, click Add.
TIP: It is important to select the solid that was created first, as this assists when rebuilding the CAD Tree.
2 Click the longest cylinder first (the solid created with Extrude Boss).
Click to select the last three cylinders.
Click OK.
Click Cancel.
NOTE: Check the Solids folder and notice that we now have one Solid body.
Now we create a cube from which our initial solid model is subtracted.
1 In the UCS Manager, right-click Top (X/Y), and click Active UCS.
2 In the Solids menu, click Cube.
Update the Data Entry parameters:
Length (X) = 6.500
Width (Y) = 4.500
Height (Z) = 2.000
Origin
X = 0.000
Y = 0.000
Z = -1.000
Click OK.
3 Click Cancel and save the file.
In this part, we subtract the initial solid model from the cube to create the cavity.
1 In the Solids menu, click Subtract.
2 Click the cube first, and then click other solid.
Click OK.
In this part, we apply fillets to the surface edges of the cavity. Note that these steps show you how to create different size fillets at the same time (which results in a single feature).
1 In the Solids menu, click Fillet.
Press Ctrl+1.
2 With the default Radius of 0.250, select the four edges as shown next.
3 Double-click in the Radius box, and type 3/16.
Press Tab and notice that the value is automatically calculated.
4 Select the surface edges as shown next. (There are eight selections.)
Rotate the view as needed, and be sure to select the edges at the bottom of the cut outs, not the top.
Press S to turn off the Shaded view. (Alternatively, in the View menu, click Shaded.)
TIP: Turning off the Shaded view is not required to make the following selections, but there are many benefits, for all types of selections, that come from utilizing the Shaded view.
Rotate the model if needed to select the edges on the opposite side of the model.
Click OK.
Press S.
Save the file.
The last remaining features for the model are the holes. As an easy way to create a grid of holes, instead of drawing them individually, we utilize hole patterns.
1 Press Ctrl+1 to select the Top view.
2 In the Other menu, click Hole Pattern.
3 Update the Data Entry parameters:
Click Grid
Width = 1.750
Height = 3.750
Hole Diameter = 0.1875
Click Break.
Number of Holes
X = 3
Y = 2
Origin
Click Center.
X = -1.250
Y = 0.000
Z = 0.000
Click OK.
4 Update the Data Entry parameters:
Width = 0.000
Number of Holes
X = 1
Origin
X = 2.375
Click OK.
5 Update the Data Entry parameters:
Width = 5.750
Hole Diameter = 0.375
Number of Holes
X = 2
Origin
X = 0.000
Click OK.
Save the file.
In this part, we extrude the hole patterns to cut the holes into the model.
1 Press Ctrl+7 to select the ISO 2 view.
2 In the Solids menu, click Extrude Cut.
Update the Data Entry parameters:
Under Other Direction
Distance = 1.000
Draft Angle = 0.000
TIP: The Positive Direction values can be set to zero or left alone. For this cut they are not important as we are cutting in the negative direction.
3 In the Edit menu, point to Select Entities, and click Pick+Match Radius.
Press S.
4 Click to select any one of the larger circles.
Click OK. (The CAD preview displays.)
Click OK.
5 Under Other Direction, update the Distance to 0.500.
6 Click to select any one of the smaller circles.
Click OK.
7 Click OK.
Click Cancel.
Click anywhere in the Workspace, and press S to turn on the Shaded view.
For the final part of this tutorial, we show you one way to move existing geometry to another CAD layer. This helps to keep our drawing organized as we forgot to create the hole patterns on the Wireframe layer.
1 In the Edit menu, click Select Mode.
2 On
the Selection Mask toolbar, click 
to remove
the ability to select solids.
3 Drag a window to select all of the geometry (only wireframe is selected.)
4 Right-click anywhere in the Workspace, point to Modify Attributes, and click Layer.
5 In the Select Layer dialog box, click Wireframe, and click OK.
6 Save the file.
Congratulations! You have finished the Mill 3 Axis Pro demonstration CAD model.
To learn how to machine the model, view the Mill 3 Axis Pro CAM Tutorial.