How to Extrude Text in SOLIDWORKS

There is no need to worry—SOLIDWORKS does not require that each character is sketched out by hand. Instead, you can use the built-in Sketch Text tool and turn that text into real geometry.

In SOLIDWORKS, “extruding text” usually means one of the following:

• Raised (embossed) text that adds material
• Engraved (debossed) text that removes material
• Scribed text that imprints/splits faces with no depth (useful for appearances, decals, or marks without removing material)

Step 1: Create a sketch that contains text (required for every method)

Both methods in this tutorial start with a sketch that contains Sketch Text. Sketch Text can be placed on straight lines, arcs, circles, splines, edges, or sketch segments—so you can position and orient the text without drawing each letter.

Before inserting text, it helps to create a simple “guide” entity (for example, a construction line, arc, or spline). You can then select that entity in Sketch Text so the letters follow the direction/curve you want. If you place text on a full circle, keep in mind that circles don’t have a start/end point—so justification options can be limited unless you split the circle into an arc.

The common requirement for both is a sketch that contains text. Begin by creating a new sketch with the text as shown in the screenshot.

Select a curve/edge/sketch segment in the Curves selection box to control where the text sits and how it flows. Type your text in the Text box.

You can link text to file properties (for example, Part Number, Description, configuration properties, etc.) using the Link to Property button indicated in green. This is handy for automatically stamping part numbers or revision text that updates when properties change.

Untick Use document font so you can control the font settings for this specific sketch text. For the example shown, set the font to Arial 8pt. If your text looks cramped on tight curves, use Width Factor and Spacing (when available) to reduce overlap and improve readability.

Use the rotate button, indicated in orange, to rotate either selected characters or the full word. You can also rotate using text syntax. The format for rotation is <r30> text here </r>. The number value indicates the rotation angle of the letter(s). Positive angles rotate counterclockwise; negative angles rotate clockwise (for example, <r-10>).

The alignment options are only available for text along a curve, edge, or sketch segment.

Extrude (Boss/Base or Cut)

The simplest way to create 3D text on a planar face is with an extrude feature.

Raised text (adds material)

Use Extruded Boss/Base to create raised lettering (an emboss effect) on flat faces. Exit the sketch, select the sketch that contains the text, then choose Extruded Boss/Base from the CommandManager and set the depth.

Engraved text (removes material)

Use Extruded Cut to engrave/etch lettering (a deboss effect). The workflow is the same: select the text sketch, start Extruded Cut, and set the cut depth.

If you run into errors such as intersecting contours (common when letters bunch up on the inside of a tight curve), first try increasing letter spacing, using a simpler font, or changing the curve. If the sketch still won’t behave, you can convert Sketch Text into standard sketch entities using Dissolve Sketch Text. This often makes trimming/repairing the profiles easier, but it also removes the “editable text” behavior—so treat it as a step you do after you’re satisfied with the font/size.

Also note: if you choose a single-line or open-contour style font, your sketch may behave like an open contour. In those cases, you may need to use Thin Feature in the extrude, or switch to a wrap/scribe-style workflow depending on your goal.

Wrap (Emboss, Deboss, or Scribe)

The Wrap feature is the most reliable approach for text on curved faces because it projects the sketch onto the target face. Wrap can:

• Emboss (adds material)
• Deboss (removes material)
• Scribe (imprints/splits faces with no thickness)

Wrap includes two methods—commonly Analytical and Spline Surface. Analytical is typically best for planar/cylindrical/conical faces and can wrap around those shapes. Spline Surface can handle more complex faces, but it may not be able to wrap fully around a model and can require higher accuracy settings for clean results.

To emboss text, click Wrap on the CommandManager to start the command and use these options:

1. Wrap Type – Emboss.  Emboss extrudes text, deboss cuts text and scribe creates an imprint of the sketch contours on the face.
2. Wrap method – Analytical.
3. Thickness – 3mm.