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

In SOLIDWORKS, almost every sketch-based feature still starts from a 2D sketch on a plane or planar face. You cannot make a standard 2D sketch directly on a cylindrical or freeform surface, so you need a few different workflows to get geometry to follow a curved face.
At the same time, tools like Spline On Surface, Split Line, and the Wrap feature give you far more control than simply guessing depths with basic extrudes.

This guide explains practical ways to add bosses, cuts, text, and images to curved surfaces using:

  • Extrude / Extruded Cut from planes aligned to the curvature
  • Sweep / Swept Cut along paths that hug a curved face
  • Wrap for embossed / debossed / scribed text or profiles
  • Decals for cosmetic logos and artwork
  • Additional tools like Split Line, Projected Curve and Spline On Surface for more advanced work

As a quick rule of thumb:

  • Use Extrude / Sweep / Wrap when you need real geometry for machining, 3D printing, or manufacturing.
  • Use Decals when you only need visual detail such as logos or labels.

Extrude

Contents

The goal with extrudes is to control both the “span” of the feature on the curved surface and the depth of material being added or removed. You can combine a planar layout sketch, a reference plane, and modern end conditions like Up to Surface and Offset from Surface to avoid trial-and-error.

1. Create a planar layout sketch

To create an extrude that protrudes from a curved surface (for example on a cylinder), start with a 2D layout:

  1. Create a sketch on a convenient planar face
    On the Top (or another planar) face, start a 2D sketch and draw a line representing the length of the feature measured along the curved surface.
    Fully define this line with dimensions and relations so its endpoints mark where the feature should start and stop on the cylinder.
  2. Create a reference plane through one endpoint
    Go to Insert > Reference Geometry > Plane:

    • First reference: one of the main planes (Front/Right) or another datum plane.
    • Second reference: the endpoint of the layout line.

    Define the plane so it is parallel to your chosen reference plane but passes directly through the endpoint. This plane will be used for the actual profile sketch, positioned correctly relative to the curved face.

  3. Sketch the feature profile on the new plane
    On this new plane, start another sketch. Use Convert Entities to bring in the layout line and mark it as construction geometry.
    Create the feature profile (for example, a rectangle) so that its width is bounded by the converted line. Geometry between the endpoints of that line will correspond to the area of the curved surface you planned in the first sketch.

At this point you have:

  • A layout sketch on a planar face that defines the footprint of the feature on the curved surface.
  • A profile sketch on a reference plane aligned with that footprint.

2. Use end conditions instead of guessing depths

Working from a plane that is offset from the curved surface can make it difficult to guess how far to extrude to meet or pass through the face. Instead of manually trial-and-error depths, you can use more intelligent end conditions:

  • Up to Surface – ends the extrusion exactly when it contacts a selected face or surface (for example, the cylinder).
  • Offset from Surface – ends the extrusion at a user-defined distance away from the target face (useful for setting consistent wall thickness or clearance).

A robust workflow for an extruded boss interacting with a curved surface is:

  1. Start Extruded Boss/Base from your profile sketch.
  2. Set the End Condition to Up to Surface and select the curved face.
  3. If you need a gap or embedment, switch to Offset from Surface and enter the required offset value.

If you want the feature to start directly on the curved face and extend outward, use the From option in the Extrude PropertyManager:

  • Set From to Surface/Face/Plane.
  • Select the curved face as the starting surface.
  • Then choose your desired end condition and depth for the extrusion.

3. Extruded cuts on curved surfaces

An extruded cut on a curved face uses the same fundamental approach:

  • Sketch the cut profile on a tangent or offset plane.
  • Use Up to Surface, Through All, or Offset from Surface as the end condition.

This lets you:

  • Cut precisely to the curved surface (for pockets or recesses).
  • Cut through the entire body (for slots, windows, or holes).
  • Leave a controlled wall thickness behind the curved surface by using Offset from Surface.

You can still adjust the length of the original layout line in the planar sketch if you need to change how far the cut spans around the curve, while the end condition handles how deep the feature goes.

Sweep

Sweeps are ideal when you want ribs, grooves, wires, or slots to follow a curved surface along a controlled path instead of pushing straight in like a traditional extrude. In a sweep, a 2D profile follows a path that can lie on or near the curved face.

1. Create or capture the sweep path

For a sweep around a cylindrical surface, use this process:

  1. Create the path
    You can:

    • Sketch the path on a planar face and then Wrap or Project it onto the curved face, or
    • Use Convert Entities on an existing edge that already lies on the curved surface, such as the intersection between a plane and the cylinder.
  2. Create a reference plane for the profile
    Use Reference Geometry > Plane with:

    • The path plus one endpoint, or
    • An endpoint and an axis

    so that the plane is normal to the path at its starting point. This will ensure the profile is oriented correctly.

  3. Sketch the sweep profile
    On this new plane, sketch the profile to sweep (for example, a rectangle for a groove or rib).
    Make the profile’s corner coincident with or vertically aligned to the path endpoint so the sweep has a clean starting condition.

2. Create the swept feature

To create the feature:

  1. Choose Swept Boss/Base or Swept Cut.
  2. Select your profile sketch as the Profile.
  3. Select the path sketch as the Path.
  4. Keep the Orientation / Twist Type set to Follow Path in most cases so the profile stays normal to the curve.

For features that require especially robust results around cylinders (such as helical grooves or knurls), you can model a small solid “cutter” as the profile and then use a solid sweep (tool-body sweep). This often produces cleaner geometry for complex paths.

To create a swept cut, follow exactly the same steps but choose Swept Cut and make the rectangle (or other profile) represent the cross-section of material to remove.

Wrap

The Wrap feature directly projects a sketch onto a curved face and can add material, remove material, or simply imprint the sketch. It is usually the cleanest option for adding text, logos, and detailed contours to cylindrical and conical faces, and in newer versions it can handle a wide range of other surface types.

1. Prepare the wrap sketch

  1. Create an offset or tangent plane
    Make a plane that is tangent to or slightly offset from the curved face where you want your design.
  2. Sketch the design
    On this plane, sketch the desired geometry: text, slots, logos, or any combination of closed contours.
    For analytical wraps, keep the sketch composed of closed contours; open contours are not supported in that mode.

In the example below, the sketch contains text and a slot that will be wrapped onto the cylindrical surface.

2. Apply the Wrap feature

To use the feature:

  1. On the Features tab, click Wrap.
  2. Select the sketch in the graphics area or FeatureManager tree.
  3. Select the curved face as the target surface.
  4. Choose a Wrap Type:
    • Emboss – adds material to a specified thickness, similar to an extruded boss following the surface.
    • Deboss – removes material to a specified depth, similar to an engraved recess.
    • Scribe – imprints the sketch contours into the face without adding or removing volume (creates visible edges only).
  5. Choose a Wrap Method:
    • Analytical – best for cylinders, cones, and other analytic surfaces. It can handle wrapping text around the full circumference of a cylinder.
    • Spline Surface – better for more organic or irregular faces, often limited to local areas rather than full 360° wraps.

The final model below shows the result of using the Emboss option: raised text and a slot that follow the curvature of the cylinder.

Compared with building equivalent geometry using extrudes or sweeps, Wrap is often more stable and easier to edit when you are working with text or graphic-style sketches on cylindrical faces.

Decal

Where Wrap creates real geometry, Decal creates a visual image mapped onto faces. Decals are perfect for labels, logos, screen graphics, and printed markings that don’t need to be machined or 3D printed.

Decals show up in:

  • Shaded model views in SOLIDWORKS
  • Renderings (PhotoView 360 and SOLIDWORKS Visualize)
  • eDrawings and shaded drawing views, if configured

They do not add edges or volume to the model, so they are purely cosmetic.

1. Adding a decal to a curved surface

  1. Open the DisplayManager and Decals pane
    Click the DisplayManager tab (just above the FeatureManager design tree) and then click the Decals icon to show existing decals.
  2. Choose or load an image
    You can:

    • Drag a decal from the built-in decal library onto the model, or
    • Right-click in the Decals area and choose Add Decal, then browse to an image file (PNG, JPG, BMP, etc.).
  3. Apply the decal
    After the decal is selected, click on the curved surface where it should appear.
    SOLIDWORKS creates a mapping from the image onto that face. You can drag the handles to scale and position it.

2. Control mapping, size, and appearance

When editing a decal, three tabs are especially important:

  • Image
    Select the bitmap file, define background transparency, and control brightness or hue. If your logo image includes an alpha channel (transparent background), enable that option to cleanly remove the background.
  • Mapping
    Choose how the decal is wrapped:

    • Label – places the decal on a single face, like a sticker.
    • Projection – projects the decal from a direction, such as from the current view.
    • Cylindrical – wraps an image around a cylindrical face, ideal for bottles, cans, and pipes.
    • Spherical – wraps decals over spherical or dome-like shapes.
  • Illumination
    Controls how the decal reacts to lights, reflections, and shadows. Often you can simply enable the option to use the underlying appearance, so the decal inherits the material’s lighting behavior.

To delete a decal, expand the Decals folder in the DisplayManager, select the decal, and press the Delete key.

3. Using Surface Flatten for real-world stickers

If you plan to print and apply an actual label or vinyl to a complex shape, you can use the Surface Flatten tool (available in SOLIDWORKS Premium) to generate a 2D flattened pattern of that surface. You can include split lines or sketch edges in the flatten to define trim lines for physical decals or vinyl.

Other Useful Tools for Curved Surfaces

Beyond Extrude, Sweep, Wrap, and Decal, there are several additional tools that help you control geometry on curved faces more precisely.

Split Line – project a sketch to split a curved face

The Split Line tool projects sketch entities, edges, or curves onto faces to split those faces into multiple regions. This is a great way to:

  • Turn a 2D sketch into a boundary on a curved surface.
  • Create separate regions on a face for appearances or decals.
  • Generate new edges to use as paths or reference geometry.

To project a sketch onto a curved surface:

  1. Create the desired sketch on a plane (for example, a logo outline or headlight shape).
  2. Go to Insert > Curve > Split Line or use the Split Line icon on the Curves toolbar.
  3. Set Type of Split to Projection.
  4. Select the sketch under Sketch to Project and the curved faces under Faces to Split.

SOLIDWORKS creates new face boundaries on the curved surface that follow your sketch. These boundaries can be used to:

  • Apply appearances or decals to only part of a curved face.
  • Serve as a path for sweeps or guide curves for surface features.
  • Provide clearer edges in drawings and visualizations.

Projected Curve – create 3D curves from sketches

A Projected Curve lets you project a sketch onto surfaces or combine multiple sketches to create a 3D curve. This is particularly useful when you want a precise 3D path that conforms closely to a curved face.

  • Sketch on Faces mode projects a sketch directly onto one or more faces.
  • Sketch on Sketch mode intersects two sketches (often on perpendicular planes) to form a spatial curve.

These curves can then be used as sweep paths, guide curves for lofts and surfaces, or references for Split Line and Surface Flatten.

Spline On Surface & 3D Sketch – “drawing” directly on the face

In some workflows you want to draw freeform curves directly on a curved surface instead of working from planar projections. Two tools are especially helpful:

  • Spline On Surface
    Start a sketch and choose Spline On Surface. Each point you place lies on the selected face, and the resulting spline stays attached to that surface even if it spans multiple faces. This is very useful for styling, surfacing, and defining complex edges.
  • 3D Sketch
    When you need spatial curves that reference multiple faces and edges, a 3D sketch allows you to create lines, splines, and arcs in three dimensions. You can constrain points to lie on faces, edges, or planes and use these 3D curves as paths or guide geometry.

These tools behave like “sketching on the surface” even though they create curves rather than full 2D sketches. They are ideal when you need organic shapes or complex boundaries that follow a model’s curvature.

Which Method Should You Use?

  • Simple bosses or cuts intersecting a curved surface
    Use Extrude / Extruded Cut from a planar sketch with Up to Surface or Offset from Surface end conditions.
  • Slots, ribs, or grooves that follow a path around the curve
    Use a Sweep / Swept Cut. Create the path with Wrap, Split Line, or Projected Curve, then place the profile on a plane normal to the path.
  • Text or logos that need to be real geometry
    Use Wrap with Emboss or Deboss. Prefer the Analytical option for cylinders and cones, and Spline Surface for irregular faces.
  • Purely cosmetic artwork
    Use Decals with appropriate mapping (label, projection, cylindrical, or spherical). Combine with Surface Flatten if you need 2D templates for printing real stickers or vinyl.
  • Precise boundaries, colour breaks, or region control on curved faces
    Use Split Line, optionally combined with Spline On Surface or Projected Curve to define the boundary curves.

Although you cannot sketch directly on a curved surface in the same way you sketch on a plane, these tools give you full control over how your geometry and visuals follow the curvature of your parts. By combining layout sketches, reference planes, projection tools, and surface-aware features, you can build clean, editable models that behave predictably, even on complex 3D shapes.

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