Home » How to use SolidWorks Wrap Feature?

The wrap feature of Solidworks is a very useful and powerful tool that is used to create designs on the faces of solid bodies. You can either emboss entities or carve them on any type of surface with the help of this tool. Also, you can use it to project sketches on the surfaces or faces of the geometries.

In this article, we are going to show you how to use the Wrap tool in Solidworks, where you can use it, and what options you have if this tool fails. So let’s get started.

How to use the Wrap tool?


1. To use the Wrap tool you must have a Solid/Surface body on which you want to wrap and a sketch that you want to wrap on that surface.

2. Next, select the sketch you want to wrap from the FeatureManager Design Tree. You can always use an existing sketch or create a new one if required. However, there are a few requirements that must be fulfilled by the sketch to be used for the wrap feature:

  • The sketch should not have any open contours. It must only contain closed contours. Your sketch can have as many closed contours as you require.
  • If the sketch is to be used for the Spline Surface method, then the center of the sketch must project on the selected surfaces/faces that you want to wrap.
  • If the sketch is to be used for the Analytical method, the sketch plane needs to be parallel to a tangent plane on the face on which you want to wrap i.e. you don’t have to make a tangent plane just make sure that it is possible if an offset is made of the sketch plane.

3. Click Wrap on the Features toolbar, or click Insert > Features > Wrap.

5. Under Wrap Type select:

  • Emboss: This option will create a raised feature on the face. This adds material to the solid body.

  • Deboss: This option creates an indented/carved feature on the face. This removes material from the solid body.

  • Scribe: This option is used to imprint the sketch contours on the face. This option is similar to the Split Line tool and Project Curve tool.

5. Select any one of the following:

  • Analytical: Select this method, if you want to wrap a sketch onto a planar or non-planar face. You can create a planar face from cylindrical, conical, or extruded models. You can also select a planar profile to add multiple, closed spline sketches. Spherical or Toroidal faces are not supported.

In the Face For Wrap Sketch input box, select a planer or non-planar face in the graphics area on which you want to wrap. You can select multiple adjacent faces but it is not recommended because sometimes this method does not work well with multiple faces.

  • Spline Surface: This method is used to wrap a sketch on any type of surface/face.

Note: The Spline Surface method was introduced in 2017. So if you are using a previous version of SolidWorks you will not find this option. You can only use cylindrical and conical faces in previous versions.

Tip: If you are wondering so why would you ever need to use the Analytical method when the Spline Surface method can wrap on any type of face? Well, because the spline surface method has its limitation. You can’t use this method to fully wrap the sketch around a model. 

The Analytical method allows you to wrap your sketch multiple times around the model. Just make sure that the sketch is inclined so that the wrap doesn’t have to wrap on the wrap itself after it completes one revolution. Or if you want the wrap to revolve just one time, make sure that the length of the sketch is equal to or less than the circumference of the cylindrical face. You can’t do it with the Spline Surface method.

In the Face For Wrap Sketch input box, select as many faces as required to allow the wrap to successfully complete. The faces must be adjacent to one another. You can’t select discrete faces. And also make sure that the center of the sketch is projecting onto any of the surfaces you selected.

6. Set a value for Thickness for the emboss/deboss.

7. Select Reverse direction, if necessary. This will make the emboss/deboss use the opposite side of the face.

8. In the Pull Direction option, you can select a line, linear edge, or plane to set in which direction the wrap will pull to create the wrap. You can leave it empty if you want the pull direction to be normal to the surface. For a line or linear edge, the pull direction is the direction of the selected entity. For a plane, the pull direction is normal to the plane.

Note: Pull Direction option is only available if you select Emboss or Deboss in the Wrap type.

9. When using the Spline Surface method, you gain access to a new option in the Wrap feature, an accuracy bar. If you set the accuracy level to low, the wrap feature will be applied in the least time and you will get the fastest rebuild times but you may experience issues with the shape and placement of your geometry. If you set the accuracy level to high, the shape and placement of the geometry will be much better but it increases the time taken to create the wrap and will result in more rebuild time.

Notice how the circular entities of the sketch are deformed in Low Accuracy but they retained their shape when accuracy is set to High.

What are the limitations of the Wrap Feature and how to overcome them?

1. There is no inbuilt draft feature available within the wrap tool. So you may want to avoid the Wrap tool to create details that requires a draft. You may want to use the Split Line, Delete Face, and Loft/Boundary feature to apply the draft. Or you can also use the Draft tool present in the Features toolbar or go to Insert -> Features -> Draft.

2. Sometimes you may find that even with the Accuracy bar set to high, the shape of the wrap is different than your sketch or the placement position of the wrap is not what it should be ideally. There is only so much this feature can do, If you want more control you may want to use Power Surfacing tools such as Split Line, Offset Surface, Thicken/Thickened Cut, etc. to achieve a better result than the wrap.

3. Scribe type splits the surface into many faces. This option works similarly to the Split Line tool. Use the Project Curve tool to project a sketch onto a surface without splitting the surface. Read More…

What can I do if the Wrap fails or it is not giving me satisfactory results?

The only alternative to the Wrap feature is to use advanced Surface tools. One method to obtain similar results is to use Split Line to split the surface into multiple faces and then use the Offset Surface tool to offset that surface with an offset value of zero and then use Thicken or Thickened Cut tool to either emboss the design on the surface or deboss it up.

If you want an alternative to the Scribe tool of Wrap, you can use Split Line or Project Curve tool. All of them works pretty much the same but have their own use case and differences. Read More…