Analyzing View Geometries

If a sketch contains inconsistent geometry, you cannot drag the geometry, nor change it in any way. Therefore, you may find it useful to analyze geometry in an active view through different means.

This task shows you how to:

Before you begin:
  • By default, the Sketch Solving Status and Sketch Analysis commands are not available in the Tools toolbar. To make them available, you need to customize the toolbar. Refer to Customizing a Toolbar by Adding Commands for more information.
  • Open a drawing representation.
  • Go to Tools > Options > Mechanical > Drafting, Geometry tab, and select the Create detected and feature-based constraints check box or make sure that Create Detected Constraints is active in the Tools toolbar.

Use the Sketch Solving Status

This is a quick way to analyze the sketch and detect whether a sketch is under or over constrained.

  1. Select all the circles.

  2. Click Constraints Defined in Dialog Box in the Constraints toolbar.

    The Constraint Definition dialog box appears.

  3. Select the Fix option.

    The geometry color has turned to green indicating that the view geometries are iso-constrained.

    Click OK in the dialog box.

  4. Select the two vertical parallel lines.

  5. Click Constraints Defined in Dialog Box and select the Fix and Vertical option.

    The geometry color has turned to green indicating that the view geometries are iso-constrained.

    Click OK in the dialog box.



  6. Click Sketch Solving Status from the Tools toolbar.

    This command gives you a quick diagnosis of the geometry status.

    The Sketch Solving Status dialog box appears and informs you of the general geometry status, whether it is under-constrained, over-constrained or iso-constrained.



    Meanwhile, the information given in the Sketch Solving Status dialog box is highlighted in red in the geometry area and the element that are under-constrained are highlighted.

    In this case the four points are highlighted indicating that they are under-constrained.



Use the Sketch Analysis

This method gives a detailed analysis of the sketch. It provides the status of each element and a constraint of a sketch. It allows you to hide constraints, create geometry, visualize use-edges in the sketch. You deactivate, isolate, delete and also replace a 3D geometry.

  1. The Sketch Solving Status dialog box is still displayed. Click Sketch Analysis in the Sketch Solving Status dialog box or select Tools > Sketch Analysis from menu.

    The Sketch Analysis dialog box appears. It contains three tabs: Geometry, Use-edges and Diagnostic.

    Construction elements appear with a blue color in the geometry.

    Note that you have the possibility to sort the elements displayed in the dialog box by Name, status or Type, by clicking the appropriate tab. Note that you can select elements from the dialog box and they will be highlighted in the geometry area.

  2. The Geometry tab displays information about all the connex profiles in the view.




    • General Status: global status on all the view geometries.

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

    • Corrective Actions : according to the analyzed element you select and which is not correct, you will be able to:


      • turn this element into a construction element

      • close a profile that is not

      • erase a disturbing element

      • hide all constraints in the view

      • hide all construction geometries in the view and in the detailed information area of the Geometry tab

  3. Click the Diagnostic tab. It gives information about every element of the geometry or constraint of a view.



    The information on this tab displays a full diagnosis of the view geometry. It provides a global analysis of the view as a whole, and specifies whether individual geometrical elements in the view 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)
    • Action: according to the analyzed element you select, you will be able to:
      • 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 tab
      • erase geometry

  4. Select Hide Construction Geometries from the Sketch Analysis dialog box. All the construction elements are hidden both from the dialog box.



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


    • Drafting documents do not contain any associative use-edges, so the Use-edges tab is disabled in the Sketch Analysis dialog box.
    • Driving dimensions use invisible constraints to drive geometries. So these constraints appear in the Diagnostic tab, but are not highlighted in geometry of the view because they are invisible. If such dimensional constraints (invisible constraint created for driving dimension) are deleted in the Diagnostic tab, then the dimension will turn not up-to-date. The dimension must be manually deleted.