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How to fully define a sketch in SolidWorks?

Fully defined sketches are fundamental when working with 3D CAD programs.  They ensure that geometry does not change, avoids errors when creating features, and allow for easy editing.

To fully define a sketch use dimensions and sketch relations to restrict movement of sketch entities.  There are many ways to fully define a sketch.  Where possible, place constraints to reduce overcrowding the sketch with dimensions.  Consider what you are designing and what dimensions in one part can affect another.  In some cases sketch entities will automatically have relations applied to them (e.g. Polygons having sides of equal length).  By default, under defined segments/entities will appear as blue and fully defined segments/entities will appear black.  You will also see a “Fully Defined” message in the bottom left of the screen when editing a sketch.

This tutorial will cover fully defined points, lines, circles and polygons in 2D sketches.  All tools used can be found in the sketch tab of the SolidWorks CommandManager.

Creating a new sketch

To begin, select the “Sketch” button from the Sketch tab of the SolidWorks CommandManager.  By default this will start the command for the creation of a 2D sketch.  Refer to the screenshot below for the tab and button selection for starting a sketch.  After clicking the sketch button, select a plane, in this case select the Front Plane to begin the sketch.

Constraining sketch entities

Points

Starting with a point, select point from the SolidWorks CommandManager and place a point into the sketch.  Place a point anywhere in the modeling window (apart from the origin) and notice the blue colour, the point is under defined and can be moved in either direction.

There are three ways to fully define the position of the sketched point.  The point can either be placed on the origin, have two dimensions providing the X and Y coordinates, or a using single dimension and a sketch relation.

Point Definition – X,Y Dimensions

Use the dimension tool, select the origin and the point to place a dimension in the X-axis.  Use the modify window  to set “Distance” to 100mm.  To set the dimension value either click on the green check mark in the “modify” window or press “Enter” on your keyboard, once you have input the desired value.

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Follow the same steps to place a dimension on the Y-axis and set the value to 75mm.  Once both dimensions have be placed, the colour of the point will change to black.

Point Definition – Sketch Relation

To show that a sketch relation can also be used to fully define this sketch, delete the 75mm dimension and then select the origin and sketch points.

The “Properties” window will now appear, as we have deleted the dimension in the Y-axis, a horizontal relation between the sketched point and the origin must be applied.  The addition of this relation will fully define our sketch as shown below.  The sketch relation will appear in green with the instance number.  It will appear on both the origin and sketched point to indicate the pair of entities the relation is applied to, the symbol shown in the green box will vary depending on the selected relation.

Point Definition – Coincident

To constrain the point onto the origin, delete the 100mm dimension and the horizontal relation.  To delete the relation, click either instance of the green symbol and press the delete button.

Once the relation is deleted, select both the origin and the sketch point, and select coincident from the relation options.

The relation symbol now shows as coincident and the point is now fully constrained at the origin.  The same result could be achieved by using both a horizontal and a vertical relation, or by placing the point on the origin initially.

Select the point and press delete, the next topic will be lines.

Lines

Select the line button from the SolidWorks CommandManager and left click once to place the start point and again to apply an end point.  By default, a line segment will have a start/end points as well as a midpoint.  To select the midpoint, right click on the line and select the “Select Midpoint” option.

Fully defining any two of these points will fully define this line segment.

Alternatively relations and dimensions can be applied to the line itself.  Left click the line that was sketched to show the line properties window.

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In the “Add Relations” section, the orientation of the line can be set by applying either a horizontal or vertical relation, in this case select a horizontal constraint.  Now use smart dimension, left click the line and set the length as 100mm.

The length and orientation of the line have been constrained, however the line can be moved anywhere around the origin.  To move the line click and drag either end point or the line itself.  We can now consider a single point on the line, fully defining any one of the three points will fully constrain the sketch.  Select the midpoint and the origin, then select the vertical relation.  Set the distance from the origin to the line as 50mm using smart dimension.

The line is now fully defined.  Follow the same procedure when fully defining a vertical line or a line at an angle.

Circles

To sketch a circle, select the circle button from the SolidWorks CommandManager.  Left click once to place the center point and again to set the radius/diameter.  Select smart dimension and left click the circle to set the diameter to 60mm.

Fully defining the center point will fully define the sketch of the circle.  This can either be done by dimensioning the position of the center point in both the X and Y directions, or by adding a coincident constraint.  In this case, set the center point to coincident with the origin.

Polygons

To sketch a polygon, select the polygon button from the SolidWorks CommandManager.

There are two options when drawing polygons, one is for the number of sides, the other is whether it is inscribed (construction circle tangent to all edges) or circumscribed (construction circle coincident with all vertices).  When placing the polygon, select the origin as the starting point and left click a second time to set it to a similar orientation as shown below.  Set the polygon to 6-sided and inscribed.

Note that relations have been automatically applied to the polygon.  All of the line segments are of equal length and the inscribed circle is tangent to one of the line segments.  Fully defining the orientation of one of the line segments and the size of the polygon will fully constrain the sketch.  There are many options for the size of the polygon (e.g. dimension a line segment, dimension the width across flats or corners, dimension the diameter of the circle).  In this case a 75mm dimension will be applied between to two of the parallel lines of the polygon (width across flats).  The final step will be to apply a horizontal constraint to one of the line segments.

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The polygon is now fully defined.

Fully Define Sketch

SolidWorks has a feature that will fully define a sketch. This feature will automatically apply dimensions and sketch relations to sketch geometry.  This tool can be helpful when it is difficult to identify what is required to fully define a sketch, however the dimensions applied are based on the current position/length of the sketch entity.  These dimensions may not have the desired value applied or may not be the most ideal for making changes to geometry in future editing.

To use the tool, click the arrow under “Display/Delete Relations” and choose “Fully define Sketch”.  The user can select to fully define all entities or selected entities to fully define them.  For this part of the tutorial, create a rectangle with the bottom left corner constrained to the origin.  Now use the fully define feature with the “All entities in sketch” option.

The “Selected entities” option can be used to fully define selected entities within a sketch.  This feature is useful, but exercise caution when relying too heavily on the fully define sketch feature, as these dimensions may not have the desired value applied or may not be the most ideal for making changes to geometry in future editing.

Exit Sketch

When a sketch is complete and fully defined, select the “Exit Sketch” button from the SolidWorks CommandManager to continue modeling.

Example

Try to fully constrain the sketch shown below.

As this tutorial has shown, there are many ways to fully define a sketch.  Fully defining sketches is critical to avoid errors when using SolidWorks features, will save time when changing part geometry, and ensure that parts fit together properly when creating assemblies.