Analyzing View Geometries

Analyzing view geometries lets you determine whether a layout contains inconsistent geometry.

Note: You must perform the analysis in an active view.

This task shows you how to:

Before you begin:
  • By default, the Sketch Solving Status command is not available in any sections of the action bar. To make it available, you need to customize the action bar.
  • Open a 3D shape representation containing a layout and in which use edges have been created (so that you can analyze them too along with the geometry). Double-click a sheet (Sheet.1 for example) in the tree to open the layout in the 2D window.

Analyze View Geometries Using the Sketch Solving Status

You can analyze view geometries using the sketch solving status.

  1. Double-click the front view to activate it.
  2. From the customized section of the action bar, click Sketch Solving Status .

    This command gives you a quick diagnosis of the geometry status. The Sketch Solving Status dialog box appears and provides a general geometry status, whether it is under-constrained, over-constrained or iso-constrained.

    The information given in the Sketch Solving Status dialog box is highlighted in red in the geometry area and the elements that are under-constrained are highlighted. In the example, three points are highlighted indicating that they are under-constrained.



Analyze View Geometries Using the Sketch Analysis

You can analyze view geometries using the sketch analysis.

Before you begin:

The Sketch Solving Status dialog box is still displayed from the previous task.

  1. Click Sketch Analysis in the Sketch Solving Status dialog box or in the Sketch section of the action bar.
    The Sketch Analysis dialog box appears. It contains three tabs: Geometry, Use-edges and Diagnostic. Construction elements appear in blue in the geometry.

    If you click the appropriate section, you can sort the elements displayed in the dialog box by name, status or type. If you can select elements in the dialog box they are highlighted in the work area.

    In the Sketch Analysis dialog box, the Geometry section: Provides information related to all the connex profiles in the view.

    General Status: Gives a global status on all the view geometries.

    Detailed Information: Provides a detailed status/comment on each profile of the view.

    Corrective Actions: Lets you perform any of the following operations:

    • : Turn the analyzed element into a construction element

    • : Close a profile

    • : Erase an element

    • : Hide all constraints in the view

    • : Hide all construction geometries in the view and in the detailed information area of the Geometry tab.

  2. Click the Diagnostic section. It provides geometry or constraint related information of a view.

    The Diagnostic section provides a full diagnosis of the view geometry that involves a global analysis of the view as a whole, and specifying whether individual geometrical elements are under-constrained (under-defined), over-constrained (over-defined) or iso-constrained (well defined):

    Solving Status: Provides a quick overall analysis of the view geometry.

    Detailed Information: Provides a detailed status on each constraint and geometrical element of the view, and lets you know what type of element it is (geometry, constraint).

    • Name: Lists the name of the element under analysis (circle, point, line or parallelism, tangency, etc.)
    • Status: Lists the constraint status (Under-Constrained, Iso-Constrained, etc.)
    • Type: Lets you know what type of element it is (geometry, constraint)
    • Scale check: Defines the status of the element based on size and positioning according to the design range of the 3D area.

    Action: Lets you perform any of the following operations:

    • : Hide all constraints in the view and in the detailed information area.
    • : Hide all construction geometries in the view and in the detailed information area of the Diagnostic section.
    • Erase geometry.
  3. Select Hide Construction Geometries in the Sketch Analysisdialog box.

    If you select items in the Detailed Information table, they are highlighted in the view, which enables you to identify them easily. To solve constraint-based problems in the view, edit the geometry directly.

  4. Click the Use-edges section.
    It provides information on each projection or intersection, on constraints and so forth created in the view.

    You can sort the use-edges by type, build or update status or input geometry.

    Detailed Information: Provides a detailed status/comment on each use-edge of the view.

    Corrective Action: Lets you perform any of the following operations:

    • : Isolate the associative use-edge making it non-associative with geometry.

    • : Remove the associative use-edge from update process (the use-edge is still associative to geometry but is not updated).

    • : Erase the use-edge.

    • : Change the input geometrical object projected or intersected (this option is unavailable in a 2D Layout)

    • : Hide all constraints in the view.

    • : Hide all construction geometries in the view and in the detailed information area of the Geometry section.

    Important: Driving dimensions use invisible constraints to drive geometries. These constraints appear in the Diagnostic section, but are not highlighted in geometry of the view because they are invisible. If such dimensional constraints are deleted in the Diagnostic section, the dimension becomes out-of-date. The dimension must be manually deleted.

Analyze Sketch for Design Range

You can analyze if an element in the sketch is beyond the design range of the model.

  1. From the Sketch section of the action bar, click Sketch Analysis .
    appears.
  2. In the Sketch Analysis dialog box, click the Diagnostic tab.
  3. Under Detailed Information, the Scale check of each element is listed. Scale check can be:
    • Valid: inside limits: For the geometric elements within size limits and with correct positioning.
    • Invalid: exceeds limits: For the geometric elements beyond the size limits of the design range. It is also applicable for elements which are positioned so far from the origin that they fall outside the footprint. If you exit Sketcher, without scaling down these elements within the size limits of the model, a warning message appears in 3D prompting the same.
    • Ignored: not applicable: For the elements that do not appear in 3D such as construction elements, or constraints.
    • ???: For the elements whose status cannot be computed. This is an undesirable status.
  4. Resolve errors for invalid elements, if any.