Intersection Curve
Makes sketch curves where the sketch plane cuts the part. Pick a face, a body or the whole part, and the lines, arcs and circles where the plane passes through it are laid into the sketch as pieces you can edit, trim, offset and dimension.
When to Use It
- Draw the outline of the part where a plane cuts through it, such as a section through the middle of a casting
- Start a rib, a pocket or a cut that must follow the shape of the part at a given height
- Find where a round or sloped face crosses the sketch plane, and draw from that line
- Check a wall thickness or a gap at a plane by dimensioning the curves it makes
Step by Step
- Open the model for modeling, then open a sketch on a plane that cuts through the part (see Planes and Faces). A plane of the part, or an Offset plane moved into it, works best. Sketching is part of modeling, which comes with the Pro plans.
- On the Sketch tab, click Advanced, then Intersect Curve. The panel opens.
- Choose Faces to pick single faces, or Bodies to pick whole bodies.
- Click the faces or bodies the sketch plane cuts. Each one lights up: orange for a face, purple for a body. Click one again to let it go.
- Press Make curves. Or press Whole part at any time to use every body of the part at once, with no picks.
- The curves are made in the sketch and a message says how many lines, arcs and circles there are.
Options
- Faces. A click picks the face under the pointer. Only the curve where the plane cuts that face is made, such as one line across a flat side or one circle around a hole.
- Bodies. A click picks the whole body under the pointer. The full outline where the plane cuts the body is made, holes included.
- Whole part. Every body of the part at once, without picking.
- Construction geometry. The curves are made as construction geometry, for reference only. They are not part of a profile to extrude or cut.
- Hold in place. Each curve is fixed where the part has it, as Convert Entities does. Off (the default), the curves are plain pieces tied end to end with Coincident where they meet, so the outline stays joined when you drag it.
What Each Cut Makes
- A flat face cut across makes a line.
- A hole, a shaft or a ball cut square to its axis makes a circle, or an arc when only part of it is cut.
- A round face cut at a slant, and any other curve, makes a run of short lines that lie on the true curve. The message counts them so you know.
- A face that lies on the sketch plane gives its own edges, as Convert Entities would.
Tips and What to Expect
- The curves are a copy taken now. If the part changes later, make them again.
- Making the same curves twice adds nothing, and a message says they are in the sketch already.
- A pick the plane does not reach is left out and counted in the message.
- One Undo takes back everything one press made.
- Press Esc to let go of the picks, and Esc again to end the tool.
- Nothing in the part or its History changes. Only the sketch gets new pieces.
Limits
- Only the sketch plane can do the cutting. A second plane or a second surface cannot be picked to cut the part, and curves between two surfaces in space (a 3D sketch) are not made.
- Curves other than lines and circles, such as the slanted cut of a round face, come in as short lines, not as one smooth curve.
- At most 50 picks at a time, 2000 curves and 400000 points in one press. A larger cut is refused with a message; pick fewer faces or bodies.
- The engine stops after 20 seconds and nothing is made. Pick fewer faces or bodies, or one face at a time.
Problems
- The sketch plane does not pass through the part. The plane lies outside the part. Sketch on a plane that cuts it, or move an Offset plane into the part.
- The sketch plane does not meet that face. The face is above or below the plane, or only touches it at a point. Pick a face the plane cuts through, or press Whole part.
- The curves cannot hold with the relations already in the sketch. A relation you added earlier fights the new curves. Nothing was changed; turn on Hold in place, or remove the relation first.