Using the Show/Erase Dialog Box in Pro/ENGINEER

The Show/Erase dialog box in Pro/ENGINEER allows you to easily show or erase multiple items at one time. It also allows you to view items that have been previously erased, and to preview a drawing after making the desired selections. Follow the simple steps below to obtain the desired display of items.

1. When clicking View > Show and Erase, the dialog box in Figure 1 displays. Selections for dimensions, reference dimensions, geometric tolerances, notes, balloons, axes, symbols, surface finishes, datums, cosmetic features, and datum targets appear and the Show button will be selected by default (or whatever the settings were when the dialog box was last used).
2. Once the icon for the detail item is selected, the constraints in the Show By portion of the dialog box become selectable. For example, if the length of the key feature should be shown in the lower right view, click the dimension button and then Feature and View (Figure 2).
3. You have the ability to preview the detail items which will be shown. To enable this functionality, click With Preview from the Preview tab. The dimensions to be shown are highlighted in cyan (Figure 3).
4. Once the key feature in the lower right view is picked, click OK or the middle mouse button to finish. The options Accept All, Erase All, Sel To Keep, and Sel to Remove become available. Click Select to Keep, select the "388.14" dimension and click Done Sel. The config.pro option "show_preview_default" can be used to control whether Sel to Keep or Sel to Remove is the default. The valid values are "remove" and "keep" (Figure 4).
5. The selected dimension will display and all other previewed dimensions will be erased (Figure 5).
6. The Show/Erase dialog box can also be used for modifying the display of other entities. Another technique for using this dialog box involves the prevention of re-displaying items which have been explicitly erased at one time. The settings Erased and Never Shown in the Options portion of the dialog box control this ability. Figure 6 displays axes shown for the bolt plate model.
7. The axes can then be erased to finish detailing work. If axes were to be shown again and the Erased option was selected, only the axes that were previously shown and then erased would appear. If the Never Shown option is selected, the axes shown in Step 6 would not appear. Only axes which had never been shown would appear. The Never Shown option prevents the user from having to re-erase items which have already been erased (Figure 7).
8. The Switch to ordinate selection in the Options portion of the dialog box will allow Pro/ENGINEER to automatically convert any unshown linear dimension to ordinate. When clicking Switch to ordinate, the Pick Bases button will be depressed. Select on an existing zero baseline in a view, click Done Sel, select the appropriate entity specified in the Show By portion of the dialog box (Feature, Part, View, etc.), and then select the feature, part, view, etc. Pro/ENGINEER will then convert any unshown linear dimensions to ordinate as long as they have a witness line which lines up with the existing baseline.

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