Pierce Relation
The Pierce relation holds a sketch point at the place where an edge of the part, or a reference axis, passes through the sketch plane. Use it to start a profile exactly on a path or an axis that runs across the sketch.
When to Use It
- Start a sweep profile on the edge it will follow
- Center a circle on a reference axis that crosses the sketch plane
- Put a point where an edge of the part meets the face you are sketching on
Step by Step
- Open a sketch on a plane or face that an edge of the part, or a reference axis, passes through (see Reference Geometry for axes). Sketching is part of modeling, which comes with the Pro plans.
- Click Select on the Sketch tab (or press S). This relation is not in the relation menus until you click Edit on the Sketch tab and tick Offer Pierce, Merge and Coradial when making relations.
- Move the pointer over the piece until its dots show, and click one point (an end, a corner or a center).
- Keep the pointer still for about half a second. In the bar that opens, click Pierce. You can also click it under Add a relation in the Properties panel.
- The point moves to the nearest place where an edge or axis passes through the plane, and a message says Pierce added: ... now sits where an edge of the part passes through the sketch plane. (or names the reference axis).
Options
| Setting | What it does |
|---|---|
| Edges | Every edge of the shown bodies is looked at. An edge lying in the sketch plane does not pass through it and is left out. An edge that ends on the plane counts. |
| Reference axes | Every shown reference axis that is not along the plane. |
| Which place | The one nearest to where the point is now. |
| Afterward | The point stays at that place; the rest of its piece can still move. |
Tips
- To choose between several places, drag the point near the one you want first.
- Hide a body or an axis to leave its places out.
- The place is worked out when you add the relation. If the part or the plane changes later, delete the relation and add it again so it finds the new place.
- One Ctrl+Z takes the relation back.
If Something Goes Wrong
- "No shown part edge or reference axis passes through this sketch plane, so there is nowhere for Pierce to put the point." Show the part, or add a reference axis that crosses the plane. Pierce is not offered at all until something passes through.
- "Pierce cannot hold together with the relations already there. Nothing changed." The point is held somewhere else, for example Fixed. Unfix it or delete the relation in the way.
- "Pierce works on a point of your own sketch." A point of a part edge or the origin cannot be moved.