Siemens NX

Constraints on Sketch

Constraints determine the relations between drawn objects like curves, points, lines, arcs, circles in the sketch through other objects in the sketch, or out of the sketch.

Constraints in the sketches can create automatically or manually.

In the figure, you can see the two different constraints symbols created automatically when creating lines in the sketch. The symbols changes according to the constraint type.

If you want to activate or deactivate automatic constraint creatin in the sketch environment, change the selection of the “Create Inferred Constraint” in the sketch.

Home => Constraints Group => Constraints Tools Drop-down => Create Inferred Constraint (In the sketch application created with “Sketch in Task Environment”)

There are several methods to assign constraints on the curve after they created.

  • Quick Pick commands;
    1. Click the left mouse button on the curve.
    2. “Quick Pick”  will open in the graphics window.
    3. Select constraint to apply on the curve.
      Also, you can select these constraint commands from the list opened by right-clicking on the curve.
  • Dragging Method on a single curve;
    1. Click and hold the left mouse button on a point on the curve
    2. Drag the point on the curve
    3. The constraint symbol will be appeared like vertical or horizontal.
    4. Release the left mouse button.
  • Dragging method to create a constraint between two curves;
    1. Click and hold the left mouse button on a point on the curve
    2. Drag the point to the other curve or object
    3. The constraint symbol will appear on the screen. This symbol changes due to the location of the dragged point on the other curve. In the figure below you can see three different constraint symbols. (Point on Curve, Coincident, Midpoint)
  • Geometric Constraints command: This command is used for special constraints. Normally this command is not required. My advice is to use method 1,2,3 for creating constraints. If you can not create constraints by using these methods you can use the Geometric Constraints command.
    1. Click on the “Geometric Constraints” command in the Home => Constraints Group => Geometric Constraints.
    2. Select the constraint type inside the “Constraint” tab in the dialog box. If you can not see the constraint type in the tab, look the “Enabled Constraints” in the Settings tab.
    3. Select objects in the sketch to create constraints

Deleting constraints: 

There is no delete constraint command in the NX continuous release. (If I’m not mistaken, there was a “Remove Constraints” command in the previous versions.)

To delete constraints, you must select the constraint then press the “Delete” key in the keyboard. 

The selection of the constraints might be a problem for you. To solve this problem.

  1. Hold the mouse cursor on the constraint. Three dots will appear near the mouse cursor. Click the left mouse button. The selection list will open. Select the constraint in the list. Press “delete” on the keyboard.
  2. Click on the “Type Filter” in the top border bar. Change the selection rule as “Sketch Constraint”. Now, you can only select the constraints in the sketch. Select constraints that you want to delete.

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