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# Coincident Vs. Pierce Sketch Relation in SOLIDWORKS

Understanding how your sketch relations affect your model will help you avoid errors and unwanted results. Without the proper sketch relations, some commands will fail, results will twist or deform, or break later on in the editing process. The two sketch relations that most commonly get misused or mixed up are Coincident and Pierce. It can be challenging to know when to use the coincident or pierce relationship because in some situations they do appear to behave the same way. In this article, we will take a look at what each relation does and how to use them.

## Coincident

When working within a single 2D sketch a coincident relation tells SOLIDWORKS to place a point so that it lies on another sketch entity, such as line arc or ellipse. This point can still move freely along the sketch entity. Applying a coincident relation in 3D space, or on 2 planes, is simpler than a pierce relation because these 2 planes do not need to intersect. A coincident relationship between a point and curve does not fully define the point. The sketch point is positioned so that it can lie anywhere along the projection of the curve or a plane that can pass through both entities. This flexibility leaves the sketch vulnerable to changing or moving. The example below shows what the results look like between a point and curve.

In this example, the endpoints are able to move freely along where the Top Plane intersects the Front Plane.

## Pierce

If you are working within a 2D sketch a pierce relationship is not an option. This relation is only an option when working with 2 intersecting planes. A pierce relationship is always between a sketch point and an external reference. You may use a point with a sketch entity, curve, feature, or model edge that intersects the active sketch plane. This relationship will place the point at the exact location where the curve pierces the active sketch plane while also fully defining the point. The example below is the same model set up as before but shows the results of a pierce relationship.

The pierce relationship is a more advanced sketch relation and is typically used for creating sweeps lofts and boundary boss/bases. Use this relationship anytime a path, profile, or guide curve needs to maintain a connection with its external reference.

SOLIDWORKS has become more forgiving and will allow the use of coincident sketch relations to create more advanced boss/bases like sweeps. Keep in mind that design changes, later on, may lead to a lost connection to the external reference and cause a feature to fail. Hopefully, this helps discern the difference between coincident and pierce relationships.

Sara Hollett
Application Engineer
Computer Aided Technology