Creating a Quick Detail View / Quick Detail View Profile

This task will show you how to quickly create a detail view using either a circle as callout or a sketched profile. In this particular case, we create a quick detail view using a sketched profile as we create this detail view from an oblong part. Note that for creating a detail view using a circle, the dialog is exactly the same.
A detail view is a partial generated view that shows only what is necessary in the clear description of the object. Note that the Quick Detail view command computes the view directly from the 2D projection whereas the Detail view command uses a Boolean operator from the 3D. The representation is therefore different. As a result, if the view which defines the quick detail view profile is modified, then the quick detail view will be updated at the same time as the defining view.
Open the GenDrafting_isometric_view.CATDrawing document.

  1. In the Drawing window, click Quick Detail View Profile in the Views toolbar (Details sub-toolbar).

    To create a detail view using a circle as callout, click Quick Detail View .

  2. Select the points required for sketching a polygon.

    If you are creating a detail view using a circle as callout, click the callout center.

  3. Double click to end the cutting profile creation. Note that if you do not close the profile, it will be closed automatically.

    If you are creating a detail view using a circle as callout, drag to select the callout radius and click a point to end the selection.

  4. Click to generate the quick detail view.

    Unlike a detail view , the profile is entirely closed. You can modify the detail view profile through the Properties dialog box.
  • The default scale is 2 (twice the scale of the active view). To modify this scale, right-click the detail view, select Properties and then the View tab. Enter the desired Parameters Scale and then click OK.
  • You can insert Bill of Material information into the active view.
  • You can assign a line type to the view to be generated. To do this, go to Tools > Options > Mechanical Design > Drafting > View tab, click the Configure button next to View Linetype and select the desired option from the dialog box.