Use this command to analyze the current sketch geometry and add constraints and dimensions automatically. The text position of the sketch dimensions created can be adjusted for clarity with the Edit Dimension Text Point command.

 

Required Inputs

 

• Base point- Select a base point or middle-click to use the default sketch plane origin.  A 2D Constraint (Anchor) will be placed at this point.

 

Optional Inputs

 

• Baseline - Select a base line to dimension from.

• Tolerance - Sets the distance tolerance for assigning constraints.

 

 

 

Create an anchor constraint and attach it to a point so that it remains anchored at its current X and Y location. The point will remain anchored until the constraint is deleted.

 

 

Optional Inputs

 

• Coordinate - Specify the coordinates of the point to constrain. By default, both the X and Y coordinates are constrained.

 

 

 

Create a point horizontal constraint and attach it to a point(s) so that it remains horizontal to the Y value of a base point. The constrained point(s) will remain horizontal at that Y value until the constraint is deleted.

 

• Select a base point for constraining Y values to and then select the points to constrain.
   

 

 

Create a point vertical constraint and attach it to a point(s) so that it remains vertical to the X value of a base point. The constrained point(s) will remain vertical at that X value until the constraint is deleted.
 

• Select a base point for constraining X values to and the select the points to constrain.
   

 

 

Use this command to constrain a point to be located at the midpoint between two selected points. If either of the two points are moved, the constrained point will remain at the midpoint of the two points until the constraint is deleted.

 

Required Inputs

 

• 1st point - Select the first outer point.

• 2nd point - Select the second outer point. The point will be constrained at the midpoint between these two points.

• Mid Point - Select the points to constrain.

 

Optional Inputs

 

• Coordinate - Specify the coordinates of the point to constrain. By default, both the X and Y coordinates are constrained.

 

 

 

 

Create a horizontal constraint and attach it to one or more lines so that they remain horizontal. The constrained lines will remain horizontal until the constraint is deleted. Select the lines to constrain.

 

 

 

Create a vertical constraint and attach it to one or more lines so that they remain vertical. The constrained lines will remain vertical until the constraint is deleted. Select the lines to constrain.

 

 

 

Create a point on curve constraint and attach it to one or more points so that they remain on a base curve. The base curve can be an arc, circle, or curve. If the base curve is modified, the constrained points will remain on it until the constraint is deleted.
 

1. Select a base curve to constrain points to. 

2. Select the points to constrain.
    

 

 

Create a point to line constraint and attach it to one or more points so that they remain co-linear with a base line. If the base line is modified, the constrained points will remain co-linear with it until the constraint is deleted.

 

Required Inputs

 

• Line - Select a base line to constrain points on.

• Points - Select points to constrain.

 

Optional Inputs

 

• Base point - Specify a base point that the constraining line should pass through. The symbol will be displayed at the constrained point(s).

• Direction - Specify that the constraining line should be parallel or perpendicular to the base line.

 

 

 

Create a point intersect constraint and attach it to one or more points so that they remain at the intersection of two base curves. The base curves can be arcs, circles, or curves.

 

• Select the two intersecting base curves and then select the points to constrain.
   

 

 

Create a parallel constraint and attach it to a line(s) so that it remains parallel to a base line.

 

• Select a base line and then select the lines to constrain parallel to it.

 

 

 

Create a perpendicular constraint and attach it to a line(s) so that it remains perpendicular to a base line.
 

• Select a base line and then select the lines to constrain perpendicular to it.
   

 

 

Create a tangent constraint and attach it to two lines, arcs, circles, or curves so that they remain tangent. If either is modified, the other will remain tangent to it until the constraint is deleted.
 

• Select the first line, arc, circle, or curve near the tangent point and then select the second.

 

 

 

Create a concentric constraint and attach it to one or more points so that they remain concentric to a base arc or circle. If the base arc or circle is modified, the constrained points will remain concentric to it.

 

• Select a base arc or circle and then select the points to constrain.
   

 

 

Create a symmetrical constraint and attach it to pairs of points to locate them symmetrically about a base line.

 

Required Inputs

 

• Line - Select the line of symmetry.

• Points - Select pairs of points to constrain symmetrically about the base line.

 

Optional Inputs

 

• Partial - Use this option to partially constrain points. Selected Both (constrain both distance and angle), Dist (constrain distance only) or Angle (constrain angle only).

 

 

 

Create an equal distance constraint and attach it to an entity so that it remains an equal distance from another entity. For example, the length of one line may be constrained to equal the length of another.

 

This constraint may also be used with radii of circles. Two circles may be constrained to have the same radius (this is done automatically in the sketcher when multiple circles are created with a single radii), or a line may be constrained to have a length equal to the radius of a circle.
 

• Select a base entity and then select the entities to constrain equal distance with it.
   

 

 

Analyze the current sketch and display information about the constraint system. When this command is selected entities are displayed in various colors that describe their current constraint level:

 

• Blue - entity is fully constrained

• Yellow - entity is partially/under constrained

• White - entity has no constraints and will not be affected by a solve

• Red - entity has redundant or inconsistent constraints. (Dimensions and constraints that appear in red are ignored during the solve).

 

The sketch is analyzed and the results are displayed in the Inquire Constraint System Form.

The form may be left up while you make further modifications to the current system. The entity colors are dynamically updated as new entities are added or deleted. Pick OK to close the form.

 

 

 

Analyze and solve the constraint system of the current sketch and display theresults in the Inquire Constraint SolveForm. When solving a constraint system, the constraints are collected into separate groups for solving called Blocks.

 

This form highlights the members (constraints and vertices) of each block. This is useful for isolating problem areas in a constraint system down to a few entities and constraints.
 

1. You may step through all the blocks using the +/- buttons or jump directly to the blocks that are having problems by selecting the NextIrreg button. Each constraint block is highlighted in the sketch for easy identification

2. Pick OK to close the form.
    

 

 

Analyze a dimension, constraint, or geometry and display information about its associations. The associated entities are highlighted in blue. For example, selecting geometry will highlight its associated dimensions and constraints. Selecting a dimension will highlight its associated geometry, etc. The information is displayed in one of three forms depending on the item selected.

 

The dimension, constraint, or geometry is analyzed and information concerning its associations is displayed in either the Inquire Sketch Dimension Form, Inquire Sketch Constraint Form, or the Inquire Sketch Geometry Form, whichever applies.

 

 

 

• When Constraining to other Base Lines, Arcs, Circles, or Curves (see CAD Tips & Techniques).

• Use Erase Entities to delete a constraint.