Home » How to sketch on a curved surface in SolidWorks?

Sketching directly onto a curved surface is not possible in SolidWorks. The method used to create a sketch will depend on the feature to be used.



To create an extrude that protrudes from the curved surface, begin by creating a sketch on the top surface. Create and constrain a line representing the length of the extrude that is required and exit the sketch. Use the “Reference Geometry” option to offset the front plane through one of the points on the sketched line.  Create a sketch on this new plane and use “Convert Entities” to use the line from sketch2 as a reference in sketch5, set is as a construction line.  Proceed to create any sketch, geometry up to the ends of the line will have full contact with the curved surface.  Consider the rectangle in the following example.

Working from a plane that is offset from the surface makes it difficult to gauge the extruded length required to penetrate the surface. Adjust the length of the line in Sketch2 to suit the width of the extrusion desired, if Plane2 has been properly defined its position will adjust accordingly.

Use the same method for a extruded cut, adjust the extrude length to suit.


This process is similar to that of extrude, use the right plane when creating the reference plane. This time use convert entities to include the end point of the line and the circular edge for reference. The left corner of the rectangle can be set to coincident with the endpoint or vertically aligned to it. This will depend on the desired position of the sweep.  Use the reference line created by selecting the circular edge to set the position of the right side of the rectangle. Once the sketch is complete sweep to the length of the line in sketc2.

Follow the same process for a swept cut, adjust the width of the width of the rectangle to suit the cut requirement.


Use this method to project the desired sketch onto the surface of the curve. Create a plane offset to tangent or passed the curved surface. Use this plane to create the desired sketch, in the example that follows the sketch contains text and a slot.  Select the “Wrap” feature from the CommandManager to begin the command.  The first step of this command is to select the sketch to be projected and the surface to project onto.  There are three options to choose from:

  • Emboss – Adds material to the specified thickness, similar to extrude.
  • Deboss – Removes material to the specified thickness (depth) similar to engraving.
  • Scribe – Creates an imprint of the sketch contours onto the curved surface.

The final product, using the emboss option, is shown in the image below.


Images can be placed on a curved surface using the decal option via the DisplayManger. Decals are flat and do not have any geometry, therefore they are purely for cosmetic purposes. Select the DisplayManager tab located just above the design tree and click the decal icon.  From here the decal library can be opened to select an image stored in the library folder. Alternatively select an image by right clicking and selecting “Add decal”, then browse to the desired image location.

To apply a decal from the library drag the image onto the curved surface.  Use the add decal option to insert a custom image, after selecting the image click on the curved surface to apply the decal.  Click the green arrow to complete the command in both instances.  The final result is shown below.

To delete a decal, expand the “Decals” drop down from the DisplayManager tab, select the decal to delete and press the delete button on the keyboard.