Creating Constraints via a Dialog Box

This task shows you how to set various geometrical constraintsusing a dialog box. For example, you can use the Constraint command to finalize your profile and set constraints consecutively.

You may define several constraints simultaneously using the Constraint Definition dialog box, or by means of the contextual command (right-click).
If you want the constraints to be created permanently, activate Dimensional constraints and/or the Geometrical constraints (depending on the type of constraint you want to create) from the Sketch Tools toolbar. If you do not activate these icons, the constraints will only be created temporarily.
Open the Constraint_DialBox.CATPart document.

  1. Multi-select the elements to be constrained. For example, two lines.

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

    The Constraint Definition  dialog box appears, indicating the types of constraints you can set between the selected lines (selectable options). 

    These constraints may be constraints to be applied either one per element (Length, Fix, Horizontal, Vertical) or constraints between two selected elements (Distance, Angle, Coincidence, Parallelism or Perpendicular).
    Multi-selection is available.
    If constraints already exist, they are checked in the dialog box, by default.
Note that, by default, a diameter constraint is created on closed circles when checking the Radius/Diameter option. If you need a radius constraint, you just have to convert this constraint into a radius constraint by double-clicking it and choosing the Radius option.

  1. Check the Perpendicular option to specify that you want the lines to always remain perpendicular to each others, whatever ulterior modifications.

  2. Click OK.
    The perpendicularity symbol appears.

 

 

   

  1. Now, select the bottom line and click Constraints Defined in Dialog Box .
    The Constraint Definition  dialog box indicates you can set the line as a reference.

  2. Check the Fix option in the dialog box and click OK.
    The anchor symbol appears indicating that the line is defined as a reference.

  

  1. Select the corner on the left of the profile and click Constraints Defined in Dialog Box .
    The Constraint Definition  dialog box indicates you can choose the Radius/Diameter or Fix option.

  2. Check Radius/Diameter in the Constraint Definition dialog box and click OK.
    The radius value appears.

  3. Multi-select both vertical lines and click Constraints Defined in Dialog Box .

  4. Check the Distance option in the Constraint Definition  dialog box and click OK.
    The distance between both lines appears.

 
At any time after the constraint was created, you can modify the constraint measure direction and/or reference. See Defining Constraint Measure Direction for more details.