Modeling Text in SOLIDWORKS

Article by TriMech Solutions, LLC updated September 20, 2022

Article

The need often arises to model text on parts. Whether we need to mark it with a part number, product serial number, or other identification marks, markings are essential to design requirements. SOLIDWORKS provides us with several methods to get the job done. But not all approaches are equal. So let’s examine the types of text features we can create and learn the pros, cons, and best uses of each to begin modeling text in SOLIDWORKS.

A con common to all methods of modeling text is a significant increase in a model’s geometric complexity because of all the extra faces each character adds to a part. Modeling text is always expensive in terms of rebuild time compared to most other features. Some users choose not to model text on their parts at all, indicating required markings with annotations on the drawing instead. But when we do need to add text to our models, understanding our options and their potential impact on rebuild times can help us make better choices.

SOLIDWORKS Sketch Text

Regardless of the feature type you intend to create, first you need a sketch containing the text you want to model. If the text will be on a flat surface you can create a sketch directly on it, but that’s not always necessary. The sketch can be projected from a plane to a surface the text is being applied to, flat or not.

The Text tool on the Sketch tab of the command manager creates a sketch text object. By default, the object’s position is controlled from the lower-left corner of the first character.

SOLIDWORKS text tool

SOLIDWORKS Sketch Text tool

While you can just eyeball the text into the position you want, there’s a better way. The text property manager includes a Curves field where you can select an arc, circle, line, spline, or edge to control position. (In this context, think of a line as a ‘curve’ with an infinite radius.) Create, restrain, and dimension construction geometry to control the exact text position you need.

text appearance options

Text appearance options

More options are available for text appearance if you uncheck the ‘Use document font’ option. The example above contains two text objects, both using the same font options. The only difference between the two is the selected control curves. The upper text is tied to an arc, while the lower text is tied to a line.

SOLIDWORKS Text Features

The features we’ll be looking at include the following:

  • Extruded Boss
  • Extruded Cut
  • Split Line
  • Wrap (3 types)

Using these tools we can add raised text to a part, etch text into a part, or split faces of a part to represent text without adding or removing any material. All four can be used on either flat or curved surfaces, but each is best suited to different situations.

The example part shown below has 6 text features created from six identical sketches, three applied to flat faces, and three applied to curved faces. From left to right the flat faces are an Extruded Boss, an Extruded Cut, and a Split Line feature. The three on curved surfaces are all Wrap features, using the Emboss, Deboss, and Scribe options respectively.

SOLIDWORKS Text Examples

SOLIDWORKS Text Examples

SOLIDWORKS Extruded Boss & Extruded Cut Features

Extruded Boss and Cut features work best on flat surfaces. They can be added to curved surfaces, and the ‘Offset From Surface’ end condition is helpful in such cases. But this only effects the top or bottom faces of the text, with the sides remaining perpendicular to the sketch instead of the face the text is being applied to.

The example below demonstrates this problem. It’s an end-view of two lines of text created by an extruded boss projected from a sketch plane at the center of a cylinder. The ‘Offset From Surface’ option correctly positions the faces of the text, but the sides of the text are vertical instead of perpendicular to the faces.

Extruded text

Extruded text

The primary advantage of Extruded Boss and Extruded Cut features is they add much less rebuild time to a model than Wrap or Split Line features. So, whenever a simple extrude can be used, it’s usually the best option.

SOLIDWORKS Split Line Features

The Split Line feature divides a face into multiple faces using one of three methods: Silhouette, Projection, and Intersection. The Projection option is useful for modeling text. It allows us to project text in a sketch onto a selected face.

SOLIDWORKS Split Line Properties

SOLIDWORKS Split Line Properties

The selected face is split up creating 1 to 5 new faces per character. For example, a “2” would create a single new face, while a “%” would create 5 new faces. The resulting surfaces have no depth, so no extra side faces are added to the model. For example, a capital “I” would result in 1 new face using the Split Line tool. It would result in a minimum of 5 new faces using an extruded feature, and many more for some fonts.

It would be natural to assume this would mean 2D surface text would add less rebuild time to your model than 3D extruded text, but that’s not the case.  Split Line features are less geometrically and graphically complex but are still more costly features than simple extrudes. So, they’re probably best used on curved or irregular surfaces where extrudes will not do, and 3D text is not required.

Keep in mind the 2D text created with the Split Line tool does not have any ‘true edges’ like 3D text does. SOLIDWORKS recognizes where the character’s surfaces meet the surrounding surface as tangent edges. A drawing view with tangent edges visible will therefore show Split Line text, but a view with tangent edges removed will not.

SOLIDWORKS Wrap Features

The Wrap property manager has many options available. Wrap features can do everything Extruded Boss, Extruded Cut, and Split Line features can do, and then some. By selecting the Emboss, Deboss, and Scribe wrap types they can create raised, engraved, or 2D text by splitting a face into multiple faces like a Split Line feature. The Analytical and Spline Surface wrap methods allow sketch text to be projected onto flat, curved, or irregular surfaces with ease.

SOLIDWORKS Wrap Feature

SOLIDWORKS Wrap Feature

This makes Wrap the clear winner as the most versatile of our four features and might tempt some users to rely on it for all their text modeling needs. This would be a mistake, because that power and versatility comes at a heavy cost in rebuild time. Wraps are the most expensive option for modeling text.

Wrap features are best used on curved surfaces where raised or engraved text is required, and the sides of the text need to be perpendicular to the curved face rather than the sketch plane. So on flat surfaces I’d stick to extrudes for 3D text. If you want to create 2D surface text, the Split Line tool is somewhat more efficient than the Wrap-Scribe.

Text Performance Evaluation

Returning to our example part with its six different text features, we can use the Performance Evaluation tool to see exactly how much rebuild time each feature costs. Remember we have an Extruded Boss, an Extruded Cut, and a Split Line on the flat surfaces, and one of each type of Wrap feature on the curved surfaces.

Performance evaluation for modeling in SOLIDWORKS

Performance evaluation for modeling in SOLIDWORKS

The rebuild time for the entire part is 3.7 seconds, almost all accounted for by the 6 text features. Not surprisingly the Wrap features are the most expensive, with Scribe slightly outperforming the Emboss and Deboss options. The Split Line outperforms the Wrap-Scribe. Surprisingly, the simple Boss-Extrude and Cut-Extrude features are about three times more efficient than the Split Line, and about four times more efficient than the Wraps!

Modeling Text in SOLIDWORKS Conclusion

Should you add text to your part models, or just add marking notes to your drawings? That’s up to you and your design requirements. When choosing which method to use rebuild time is not always the deciding factor for modeling text in SOLIDWORKS. The unique geometry of your part, your project requirements, and company standards will guide your choice. But all other things being equal, you might as well build the most efficient model you can.

Related Links

Certified SOLIDWORKS Services available from Javelin

Javelin can help you to:

TriMech Solutions, LLC

TriMech provides thousands of engineering teams with 3D design and rapid prototyping solutions that work hand-in-hand, from sketch to manufacturing. Javelin became a subsidiary of TriMech Solutions LLC in 2021.