Detail Angled Cuts With Ease in Alibre Design

14 Feb, 2005 By: Michael Todd

Master using angled planes and custom views for quick and easy creation of associated detailed drawings

One of the most frequently asked questions I receive as the Alibre Assistant is how to create angled cuts such as holes and slots. The next question is always, "Great. Now how do I generate a drawing view that I can use to properly detail the cut for manufacturing?" This month's Tech Tip will show you how to insert and use a plane that you can then use to create angled features. Plus, you will learn how inserting a simple custom view in the part workspace makes creating an associated detailed drawing view a snap. Follow these steps to create angled features. Start by creating a simple part.
  • In a new part workspace, select Tools / Options. On the General tab, make sure that Snap To Working Plane is selected.
  • Select Sketch / Activate 2D Sketch to enter 2D Sketch Mode. Then use the Line tool to create a sketch similar to the one shown here (figure 1).

Figure 1. This simple sketch is the first step to creating angled features.

  • Select the Dimension tool and apply an angular dimension of 45 degrees as shown (figure 2). You may also apply other linear dimensions as desired. Note: Dimension values do not have to match the example shown.

Figure 2. Select the Dimension tool and apply an angular dimension of 45 degrees.

  • Select the Extrude Boss tool (figure 3). For Type, choose Mid Plane and enter a depth of 12.00". Click OK.

Figure 3. Applying the Extrude Boss tool.

To insert angled holes, first we need to insert an angled plane.

  • Rotate the part as shown (figure 4), then right-click the Work Area and choose Insert Plane. The Insert Plane dialog box appears. Note: To create an angled plane, you can use an existing plane or any surface and/or edge. Different combinations will create different planes. You can select the object(s) before selecting Insert Plane and they will prepopulate the dialog box.

Figure 4. Inserting an angled plane.

  • Select the back face of the part as shown highlighted in blue.
  • Press the Control key and select the Z-Axis from the Design Explorer. In the dialog box, the Distance option has been replaced with Angle.
  • Enter 45 as the value and click OK. Note: To change the angle of the plane, right-click the plane and select Edit. Objects associated with the plane will also change. Because Snap To Working Plane is on (from our first step), we can create a Custom View that can be used in a 2D Drawing.
  • Right-click the angled plane and select Activate 2D Sketch.
  • Select View / Orientations (figure 5). Click Add. Enter Angled View and click OK.

Figure 5. Specifying the view orientation.

We can now create objects (including holes) associated with the angled plane.

  • Select the Circle tool and insert three circles approximately as shown (figure 6).

Figure 6. Insert three circles using the Circle tool.

  • Select the Dimension tool and insert dimensions as desired.
  • Select the Extrude Cut tool, choose Through All, then click OK .

Figure 7. The holes are now associated with the angled plane.

Note the angle of the holes (figure 7). They are associated with the angled plane. Any change in the plane angle will change the angle of the holes.

  • Save the part with the name "Angle Bracket."
We will now use the custom view of the angled plane to create drawing views in which the holes may be dimensioned.
  • Open a new drawing workspace. Select ANSI C for the Template and enter any text you would like in the Fill In Text dialog box.
  • In the Standard Views Creation dialog box, click the Workspace Orientation button.
The custom view we created previously appears in the Orientations dialog box.
  • Double-click Angled View and click Close.
In the Standard Views Creation dialog box (figure 8), note that the Front View preview has changed. Because the Top and Right view are also selected by default, those views will fold in a third angle projection based on the Front View, which is now our custom view.

Figure 8. Note that the Front View preview has now changed.

  • Click OK.
  • Click the work area to place the three views (figure 9). Note: If you have Design Dimensions checked on in the Properties dialog box (File / Properties / Detailing tab), dimensions created in the part workspace will appear when you place the views.

Figure 9. The three views placed in the work area.

You can dimension the views as needed, but notice that the view is oriented to allow a planar view of the holes (figure 10). Note: Auxiliary views will be dependant on the parent view and can be created from any of the existing views.

Figure 10. The view is oriented to allow a planar view of the holes.

Next month we'll look at a unique tool that allows you to easily apply linear dimensions to circular figures in part modeling and drawing workspaces. Until then, look for me as the Alibre Assistant online in Alibre Design.

About the Author: Michael Todd

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