Projected Curve

With two non-parallel sketch curves in the graphic area:

1. Click .

   

2. Select the Two sketches option.
3. With focus in the First sketch field, select the First sketch (on the model or in the Feature list).
4. With focus in the Second sketch field, select the Second sketch (on the model or in the Feature list).

5. Complex curves can be reapproximated to create simpler curves. Check Approximate to open options to reapproximate the curve. The original curve is displayed in orange, and the new approximated curve is displayed in magenta.

   • Target degree - Enter the target curve degree for the selected curve.
   • Maximum control points - Enter the maximum number of control points allowed for the selected curve.
   • Tolerance - Tolerance of the selected curve, as a length measurement. Enter the tolerance value.
   • Keep start derivative - Check to keep tangency at the beginning of the selected curve.
   • Keep end derivative - Check to keep tangency at the ending of the selected curve.
   • Show deviation - Check to view the maximum deviation between the original curve and the reapproximated curve.

   

6. Click to accept.

You can not show/hide the feature associated with a Curve; use the show/hide functionality in the Curves list instead.

Example

The first sketch is selected:

The second sketch is selected and the resulting curve appears:

The curve is listed in the Parts list under Curves:

With a curve and a face in the graphic area:

1. Click .

   

2. Select the Curve to face option.
3. With focus in the Edges field, select the edge/curve (you can select multiple) to project onto a face.
4. Select the perspective of the projection:
   1. Normal to target - Project the curve or curves onto the target face normal to the target.

      

   2. Direction - Select a curve or edge illustrating the direction in which to project the curve or curves.

      

5. With focus in the Targets field, select the face (or faces) onto which to project the selected curves.

6. Complex curves can be reapproximated to create simpler curves. Check Approximate to open options to reapproximate the curve. The original curve is displayed in orange, and the new approximated curve is displayed in magenta.

   • Target degree - Enter the target curve degree for the selected curve.
   • Maximum control points - Enter the maximum number of control points allowed for the selected curve.
   • Tolerance - Tolerance of the selected curve, as a length measurement. Enter the tolerance value.
   • Keep start derivative - Check to keep tangency at the beginning of the selected curve.
   • Keep end derivative - Check to keep tangency at the ending of the selected curve.
   • Show deviation - Check to view the maximum deviation between the original curve and the reapproximated curve.

   

7. Click to accept.

You can not show/hide the feature associated with a Curve; use the show/hide functionality in the Parts list instead.

In addition to the surfacing tools, curves are used to create the basic building blocks of surfaces.

This lists the collection of curve feature tools. This is not an exhaustive list. Additional Feature tools may be used when manipulating curves.

• Sketch tools - Tools in the Sketch toolbar such as Line, Corner rectangle, Center point rectangle, Center point circle, 3 point circle, Tangent arc, 3 point arc, Spline, Point, and Construction used to create a sketch in a Part Studio.
• Helix - Create a helix using a conical or cylindrical face, single axis or z-axis of a mate connector, or circular edge.
• 3D fit spline - Create a 3D fit spline through a series of vertices. Creates a curve which is listed in the Parts list under Curves.
• Projected curve - Create a curve from the projection of two sketches (Two sketches option) or from the projection of a curve on a face (Curve to face option).
• Bridging curve - Create a Curve connecting any two points, vertices, or Mate connectors. The resulting Curve is listed in the Feature list and the Parts list.
• Composite curve - Represent multiple edges as one Curve. Select multiple adjacent edges, sketch entities, and other curves. Selecting non-contiguous edges may result in multiple Curves created. Selections for each Curve must meet at their vertices. (Curves are listed in the Parts > Curves list.)
• Intersection curve - Create a curve at the intersection of two or more surfaces or faces. The selections must intersect.
• Trim curve - Trim or extend a curve by a distance or to a bounding entity.
• Isocline - Create an isocline on a sloped face. An isocline runs on a face at positions where the face has a certain slope compared to its reference definition. The resulting isocline is listed in the Feature list and Parts list.
• Offset curve - Create and extend and/or split a new curve by offsetting edges on surrounding faces.
• Isoparametric curve - Create smooth curves that run along a face or surface in the U or V direction.
• Edit curve - Edit an existing curve by selecting sketch entities or curves to apply a simplified approximation, elevate the degree, reposition control curve vertices and/or planarize into any 2D plane.

With two non-parallel sketch curves in the graphic area:

1. Tap the Projected curve tool.

   

   

2. Select the Two sketches option.
3. Select the First sketch.

   

4. Select the Second sketch.

   

5. Tap the checkmark.

With a curve and a face in the graphic area:

1. Click .

   

2. Select the Curve to face option.
3. With focus in the Edges field, select the edge/curve (you can select multiple) to project onto a face.
4. Select the perspective of the projection:
   1. Normal to target - Project the curve or curves onto the target face normal to the target.

      

   2. Direction - Select a curve or edge illustrating the direction in which to project the curve or curves.

      

5. With focus in the Targets field, select the face (or faces) onto which to project the selected curves.
6. Tap the checkmark to accept.

You can not show/hide the feature associated with a Curve; use the show/hide functionality in the Parts list instead.

With two non-parallel sketch curves in the graphic area:

1. Tap the Projected curve tool.

   

   

2. Select the First sketch.

   

3. Select the Second sketch.

   

4. Tap the checkmark.

You can not show/hide the feature associated with a Curve; use the show/hide functionality in the Parts list instead.

With a curve and a face in the graphic area:

1. Click .

   

2. Select the Curve to face option.
3. With focus in the Edges field, select the edge/curve (you can select multiple) to project onto a face.
4. Select the perspective of the projection:
   1. Normal to target - Project the curve or curves onto the target face normal to the target.

      

   2. Direction - Select a curve or edge illustrating the direction in which to project the curve or curves.

      

5. With focus in the Targets field, select the face (or faces) onto which to project the selected curves.
6. Tap the checkmark to accept.

You can not show/hide the feature associated with a Curve; use the show/hide functionality in the Parts list instead.