How to Use Pierce Relation in SOLIDWORKS

The Pierce relation makes a sketch point intersect a curve, edge, or sketch entity that passes through the sketch plane. It is often used for sweep profiles, guide curves, tubing paths, weldments, and any feature where a profile must start exactly on a path.

What the Pierce relation does

A Pierce relation is different from Coincident. Coincident works when two items lie in the same sketch plane. Pierce is used when a curve or edge passes through the active sketch plane and you need a sketch point to sit exactly where that crossing occurs.

This is why Pierce is so common in sweeps. The sweep profile must be tied to the path at the correct start point, even though the path may be a 3D sketch or an edge from another feature.

Add a Pierce relation

1. Edit the sketch that contains the profile or point you want to control.
2. Select the sketch point, endpoint, or profile point.
3. Hold Ctrl and select the curve, 3D sketch segment, model edge, or path that passes through the sketch plane.
4. In the relations box, choose Pierce.
5. Rebuild the model and confirm the point stays attached to the path.

If Pierce is not available, the selected path may not actually pass through the sketch plane. Rotate the model and inspect the geometry before adding more relations.

Use Pierce with sweep profiles

For a swept boss or swept cut, place the profile sketch on a plane at the start of the path. Then use Pierce to attach the profile center, corner, or endpoint to the path. This keeps the profile from drifting away from the sweep path when the model changes.

A fully defined sweep profile is easier to edit later. Add the Pierce relation first, then dimension the profile size and add any orientation relations needed for the design.

Common problems

If the relation over-defines the sketch, remove duplicate Coincident, Horizontal, Vertical, or midpoint relations that are fighting the Pierce relation. If the profile flips or rotates unexpectedly, add a construction line or reference relation to control orientation.

If the path changes and the feature fails, check whether the path still crosses the profile sketch plane. A small path edit can move the crossing point away from the plane and break the Pierce relation.

When to use another relation

Use Coincident when both entities are in the same sketch plane. Use Pierce when the selected curve or edge passes through the sketch plane. Use Convert Entities when you need to copy an edge into the sketch itself rather than simply attach a point to where it crosses the plane.

Choosing the right relation keeps the sketch easier to repair and makes sweep features more predictable.