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Zoom-In
to the FRONT and RIGHT views as shown (Click the Right Mouse Button to cancel the zoom function).
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Following any zoom action, always click the Right Mouse Button (or choose Select Items ) before selecting a dimension, view, drawing note, etc.. . This cancels the zoom function and returns to the selection cursor. |
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Select the vertical 7.00 dimension on the front view (it will highlight in red).
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Hold down the Right Mouse Button and choose Move Item to View.
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Select the RIGHT view to move the dimension to the Right view.
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Select the vertical height dimension of 10.00.
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Hold down the Left Mouse Button and drag 10.00 dimension farther away from or towards the geometry.
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Select and drag the 10.00 dimension up and down (notice the center snapping).
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Center Gravity: Dimensions are automatically centered between the witness lines and when dimensions are moved, they snap to this centered location. This "gravity" location aids in placement. |
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With the 10.00 unit dimension still highlighted, press and hold the Right Mouse Button and select Flip Arrows from the pull down to change the direction of the arrows.
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Repeat the Flip Arrows command to switch the arrows back.
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With the 10.00 unit dimension still highlighted, hold down the CTRL key and select the 8.13 dimension (the height of the protrusion).
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Multi-select items by holding down the CTRL key and selecting the items. |
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Press and hold Right Mouse Button and select Align Dimensions from the pull down.
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Select the FRONT view.
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Press and hold Right Mouse button and select Cleanup Dimensions from the pull down. A dialog box will pop-up similar to the figure below.
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Choose the options and type in the values as shown in the figure above.
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Clidk Apply and Close. Notice how this view can be quickly cleaned up.
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To use this technique on multiple views, by first multi-selecting the views and then doing a Cleanup Dimensions to drastically reduce the amount of manual effort normally involved. |
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Select Info from the pull down menu at the top of the window and choose
Switch Dims. This shows the symbol, or "parameter", for the dimensions.
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Repeating Switch Dims will toggle the display of dimensions back and forth from numeric to symbolic. Every dimension (and its tolerance values) are represented inside Pro/ENGINNER by these symbols that can be used in relations or in parametric notes. |
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Now let's add a parametric note that calls-out the wall thickness. |
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Select Insert -> Note... from the drop-down menus.
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Select Make Note from the menu manager and accept all the defaults.
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Click a spot anywhere under the Left cross-section view as the desired note location and middle-click
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Type THE WALL THICKNESS IS &D21 INCHES and click Accept
or press Enter.
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This symbolic name may be different than shown above. If so ensure you enter in the correct symbolic name in the note creation box. |
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Select Accept
again as you are not creating another sentence.
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Click Done/Return from the menu manager.
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You can also add Ordinate Dimensions that use a single witness line with no leader, and are associated with a baseline reference. They are used mostly for flat plate or sheetmetal designs but we will illustrate an example of this capability on our box part. |
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Insert, Dimension, Ordinate... from the drop-down menus.
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Select the bottom edge as a baseline from the Right view as shown in the figure below.
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Select the two edges as shown below to create ordinate dimensions.
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Place the cursor to the right of the view and click the Middle Mouse Button to place the dimensions.
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Click Return from the menu manager.
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You can convert linear dimensions to ordinate dimensions and vice-versa. You can also have ordinate dimensions automatically created under Insert -> Dimension -> Auto Ordinate... as opposed to picking the individual entities in our exercise. This is extremely invaluable for flat plate and sheetmetal parts. |
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Click Save
from the main toolbar.
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Click OK.
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Congratulations! You have successfully created your first part drawing.
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