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Sketch Relations – SolidWorks Guide

Sketches are the building block of SolidWorks. You can either create a 2D or 3D sketch as per your requirements. Relations are used to define sketches. Relations between sketch entities and model geometry are an important means of building in design intent.

How To Add A Sketch Relation in SolidWorks?

SolidWorks automatically adds certain relations as you sketch. If this is not the case for you then go to Options -> System Options -> Relations/Snaps. You can enable or disable the automatic snapping of sketch entities. You can even define which type of snappings you want. You can also disable the Automatic Relations option if you don’t want SolidWorks to assign relations to the snapped entity automatically.

Tip: Automatic Relation for Angle snap will not be added because it needs to be defined by a dimension and not a relation.

To manually add a relation, while holding the Ctrl key on your keyboard, select the entities between which you want the apply the relation and then select the relations you want to add from the options provided under the Add Relations menu. You can also add relations using tooltips. Select the entities you want to add the relation between while holding the Ctrl key and as soon as you let go of the Ctrl key on your keyboard the tooltip will appear. You can then click on the relation you want to add.

You can also use the Add Relation tool to add relations manually. Click on the drop-down arrow below the Display/Delete Relations tool and select the Add Relation tool. Or you can let SolidWorks automatically add all the necessary relations by using the Fully Define Sketch tool.

While sketching and adding relations you will find that the entities change their color. There are 4 types of color that a sketch entity can have:

  1. Sketch entities that are Black in color mean that these entities are fully-defined and you cannot drag them.
  2. Sketch entities that are Blue in color mean that these entities are under-defined and so you can drag them.
  3. Sketch entities that are Yellow in color mean that these entities are over-defined and you cannot drag them. Delete relations that are not needed to make it either fully defined or under-defined.
  4. Sketch entities that are Red in color mean that these entities have relations that are not possible to achieve. Delete relations that are not needed to make it either fully defined or under-defined.

Tip: Endpoints of segments also have their own relations. For example, you may notice that a line may be black in color but its endpoints are still blue stating that you cannot drag the line itself but you can drag its endpoints to increase or decrease the length of the line.

At the bottom of the SolidWorks window, you can find the status of your sketch while you are editing it. If any of your sketch entities are in red or yellow color, the status bar will instead state the No Solution Found warning. You can access SketchXpert by clicking on the warning which you can use to fix the sketch.

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You can click on any relation in the graphics area and the entities will get highlighted between which the relation is present. For example in the below image, when we clicked on the tangent relation it highlighted the two arcs between which it has been applied.

If sketch relations are not visible, click on the down arrow present alongside the Hide/Show icon in the heads-up toolbar and then click on the View Sketch Relations icon. Alternatively, you can go to View -> Hide/Show and select Hide Relations. However, making sketch relations visible is not recommended most of the time as they do tend to make the sketch look clumsy and complex. Also, if there are a lot of visible sketch relations in your open sketch it may affect the performance of the software.

Tip: If the sketch relations are still not visible make sure that the Hide/Show icon in the heads-up toolbar is not selected or the Hide all types option is not selected under View -> Hide/Show.

How To Delete A Sketch Relation in SolidWorks?

To delete a relation, if the sketch relations are visible, you can click on the relation’s icon (green in color) in the graphics area that you want to delete and press the Delete key on your keyboard.

Or, you can click on the entity between which the relation was added and you can then delete the relation from the Existing Relations table.

You can also use the Display/Delete Relations tool to list all the relations that are present in your sketch then select the ones that you want to delete from the table and then click on the Delete button or use the Delete All button to delete all the relations that are listed in the table. You can also filter the relations according to your needs by expanding the All in this sketch option. Use the Replace button provided below to replace the entities between which the relation was added.

List of Sketch Relations in SolidWorks

Below is the list of relations that can be used in SolidWorks. Note that you need to select the stated entities, only after that you will see the option to add these relations.

1. Horizontal: Select either one or more lines or two or more points (a point can be any point let it be a midpoint, endpoint, or just a standalone point). The lines will become horizontal (not colinear); in the case of points, they will be aligned horizontally like they are on a single line.

2. Vertical: Select either one or more lines or two or more points. The lines will become vertical (not colinear); in the case of points, they will be aligned vertically like they are on a single line.

3. Collinear: Select two or more lines. The lines will become colinear like they are on the same line. In the image below, all three lines are made collinear.

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4. Coincident: Select a point and a line/arc/ellipse. The point will lie on the selected entity.

5. Perpendicular: Select two lines. The lines will become perpendicular to each other.

6. Parallel: Select two or more lines. The lines will become parallel to each other.

7. Midpoint: Select a point and a line. The point will lie at the midpoint of the line.

8. Tangent: Select an arc/ellipse/spline and a line/arc. You can also select a point where two entities are merging. The selected entities will become tangent to one another.

9. Concentric: Select two or more arcs/circles, or a point and an arc/circle. The selected entities will now have the same center point.

10. Coradial: Select two or more arcs or circles. The arcs will have the same center point and also the same radius.

11. Equal: Select two or more lines or two or more arcs/circles. The length of the line will become equal. In the case of arcs, radii will become equal.

12. Equal Curvature: Select two splines. The radius of curvature and the direction vector of the splines will become the same.

13. Intersection: Select two lines and one point. The point will lie at the intersection of the lines.

14. Symmetric: Select a centerline and two points/lines/arcs/ellipses. The items will lie equidistant from the centerline, on an imaginary line that is perpendicular to the centerline. This relation is also added automatically when you use the Mirror Entities tool to create symmetric sketch entities.

15. Fix: Select any entity. The entity’s size and location will be fixed. However, the endpoints of a fixed line, arc, or elliptical segment are free to move. If you want to fix the endpoints, select them and apply the Fix relation to them separately.

16. Fix Slot: Select a slot. The slot’s size and location will be fixed.

17. Pierce: Select a point and an axis/edge/line/spline. The sketch point will become coincident with where the axis, edge, or curve pierces the sketch plane. The pierce relation is heavily used in guide curves. Notice in the image below, the endpoint of the spline has a coincident relation with the circle but it is still not on the circle. Adding a pierce relation will make it lie on the circle.

18. Merge Points: Select two sketch points or endpoints. The two points will be merged into a single point.

19. Doubled Distance: Using the Smart Dimension, select a centerline and any sketch entity. When you move the cursor to the other side of the centerline, the sketch entity will be dimensioned at twice the distance from the centerline. Useful when creating sketches for the  Revolve feature.

20. Equal Slots: Select two or more slot sketch entities. The slots will now have equal lengths and radii.

21. Tangent to Face: Select a sketch entity and a solid face. The sketch entity and face will become tangent to one another.

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23. Torsion Continuity: Select two splines, a spline and an arc, or a spline and model edges that are linear, circular, conic, parabolic, elliptical, or spline-based. The selected entities must share a common endpoint for this relation to be accessible. The sketch entities will obtain a smooth continuity relation with equal curvature and equal rate of curvature at the shared endpoint. A black-colored zig-zag arrow is also placed at the shared endpoint to help identify that the point now has a torsion continuity.

Below are some relations that are automatically added when you use different sketch tools:

Note that the entities created by the sketch tools are fully defined and if you want to edit them you have to delete the existing relation.

24. On Edge: This relation is added automatically when the edges of the solid are projected to the sketch plane using the Convert Entities tool.

25. Silhouette on Edge: This relation is added when the edges of the solid are projected to the sketch plane using the Silhouette Entities tool.

26. At intersection of two faces: This relation is added when the Intersection Curve tool is used to obtain a curve at different types of intersections.

27. Geo-offset Entities: This relation is added when you use the Geodesic Offset type of Offset on Surface tool to create a 3D sketch entity that is at an offset distance from the boundary of the surface.

28. Offset: This relation is added automatically when the Offset Entities tool is used to create an offset of sketch entities or edges of the solid.

29. Patterened: This relation is added when you use the Linear/Circular Sketch Pattern tool to create a linear or circular pattern of sketch entities.

Below are some relations that are only available in a 3D sketch:

1. ParallelYZ: Select a line and a plane (or a planar face) in a 3D sketch. The line will become parallel to the YZ plane with respect to the selected plane.

2. ParallelZX: Select a line and a plane (or a planar face) in a 3D sketch. The line will become parallel to the ZX plane with respect to the selected plane.

3. AlongZ: Select a line in a 3D sketch. The line will become parallel to the Z-axis of your part.

4. AlongX: Select a line in a 3D sketch. The line will become parallel to the X-axis of your part.

5. AlongY: Select a line in a 3D sketch. The line will become parallel to the Y-axis of your part.

6. On Plane: Select sketch entities and a plane/planar face. The sketch entities will now lie on the plane.

7. On Surface: Select sketch entities and a surface/non-planer face. The sketch entities will now lie on the surface.

And that is it. We hope that this article helped you learn how to use the relations in SolidWorks. If you have any questions or suggestions, feel free to leave a comment down below.