Introduction to Drawings

Task 2. Create, move, and manipulate drawing views

Let's look at how we can manipulate the views and create additional ones as needed.

Select the FRONT view so that it is outlined with a dashed red box. Make sure that you don't accidentally pre-highlight a dimension or dimension witness line and select that item. If you do, just re-pick on the view to select it.
Press and hold the Right Mouse Button over the view and uncheck Lock View Movement.
With the FRONT view still selected, Press and Hold the Left Mouse Button and drag the view outline around.
Release the Mouse Button to place the view.

Notice the intelligence of the other views as they will continue to line up and follow the FRONT view accordingly.
Return the FRONT view to its original position by using Edit > Undo from the menus (or use CTRL-Z)

Let add a projected view based off the Front view
Select the FRONT view again,
Press and hold the right mouse button and select Insert Projection View...
Move the mouse around and notice that you have 4 possible projection options.
Select a point to the left of the FRONT view. The view will look similar to the figure below.

With the new view still selected, press and hold the right mouse button and select Properties.

To change the properties on more than one view at a time, hold down the CTRL key while selecting them and then access the Properties window from the right mouse button menu. This can include determining visible areas, scaling, defining cross-sections, showing the model in various states, and aligning and setting the view origins.

Select the View Display Category in the Drawing view dialog box , change the Display Style from Follow Environment to Hidden.

Follow Environment—Uses the setting from Tools > Environment > Display Style or one of the view display style icons ( Wireframe, Hidden Line, No Hidden, Shaded) in the Pro/ENGINEER graphics window.

Click Apply from the Drawing View dialog box. The view will appear similar to the figure below. (Move the Drawing View dialog box if necessary to see the changes)

Create a cross-section of the new view we just created
Select the Sections category in the Drawing View dialog box.
Choose 2-D cross section, and click Add Section .
Select section A (which is pre-defined in the part) from the Name drop-down.
Click Apply.

You can also modify the cross-hatching for certain materials or preferences.
Scroll the section definition window all the way to the right.
Click on the empty "Arrow Display" box to activate it.
Select the TOP VIEW from the drawing window.
Click OK.

Cross-section and view arrows can also be added by selecting the view and choosing Insert, Arrows... from the drop-down menus (or by using the right mouse button menu to choose Add Arrows)