How To Use Projected and Wrap Features in SOLIDWORKS

Problem

SOLIDWORKS offers multiple ways to map a 2D Sketch onto a 3D surface or face. Each method can produce a different result, and it is important to decide which one is best for your design. 

This article will go over both Projected and Wrap Features. The Projected Features include information about the "Projected Curve", "Split Line", and "Convert Entities" features, while "Wrap" is a standalone feature.

Solution 1: Projected Curve

A projection is used to map a set of entities to a 3D face or surface perpendicular (or normal) to the sketch plane.

If the projection is viewed normal to the sketch, it will appear to follow the same path, despite each point having different heights in relation to the sketch plane.

To use the "Projected Curve" feature, follow the steps below:

1. Navigate to the "Features" tab.
2. Select the "Curves" button to open the Curve Commands drop-down menu.

3. Click "Project Curve" from the drop-down menu.

   

4. Select the appropriate Projection type from the "Projected Curve" property manager.

   

   Sketch on faces - Projects a sketch onto a face or surface. 

   Sketch on sketch - Produces a curve that represents the intersection of both sketches.

5. If "Sketch on faces" was selected, Select the intended sketch, surface/face, and (optional) projection direction as shown below.

   

6. If "Sketch on sketch" was selected, select the two intended sketches as shown below.

   

7. Click the green check to complete the feature.

Once the projected curve is complete, you are left with 3D curve geometry. These are most commonly used as sweep paths and guide curves for sweeps, lofts, and boundary features.

Solution 2: Split Line

The "Split Line" feature has three different types. However, this article will only cover the "Projection" type. This type requires a sketch and a face selection.

To use the "Split Line" feature, follow the steps below:

1. Navigate to the "Features" tab.
2. Select the "Curves" button to open the Curve Commands drop-down menu.

3. Click "Split Line" from the drop-down menu.

   

4. Select "Projection" as the type of split.

5. Select the intended sketch and surface/face as shown below.

   

6. Click the green check to complete the feature.

   

Once the split line is complete, you will have a result similar to the "Projected Curve" feature. However, this feature uses the projection to divide the selected face into multiple faces.

Solution 3: Convert Entities

Another type of projection in SOLIDWORKS is the "Convert Entities" tool. This is helpful when you need to project geometry onto a 2D sketch plane. This is a type of sketch relation that can be activated from the sketch toolbar.

To use the "Convert Entities" tool, follow the steps below:

1. Navigate to the "Sketch" tab.
2. Create a new sketch using the "Sketch" button in the upper-left corner.
3. Select the intended plane or planar face you would like to sketch on.

4. Click the "Convert Entities" button.

   

5. Choose the geometry you would like to project onto your sketch plane.

   

6. Click the green check to complete the command.

It will then create new sketch entities that project what you have selected. If your selection's geometry updates, this feature will also update. This tool is also available for 3D Sketches, but it does not project the geometry onto a specific plane.

Solution 4: Wrap

It is best to think about a Wrap feature as applying a sketch as a sticker or decal to a curved surface. The image below shows the difference between the seed sketch and its result, when viewed normal to the sketch plane.

The final shape does not match the original sketch. The distance between points is calculated across the surface instead.

The Wrap feature is best for applying text to a model. A "Projected Curve" or "Split Line" methods will produce the stretched-out result below on any curved surface.

To use the "Wrap" feature, follow the steps below:

1. Complete the sketch that you intend to wrap.
2. Navigate to the "Features" tab in the Command Manager.

3. Select the "Wrap" button.

   

4. Select the sketch you would like to wrap to activate the "Wrap" property manager.

   

5. Select "Scribe" as the Wrap Type.

   

   The Wrap feature can also "Emboss" or "Deboss" instead of "Scribe". An emboss will create a raised feature, while a deboss will create an indented feature.

6. Select the appropriate Wrap Method for your application.

   

   Analytical - This method is best for wrapping a sketch around a planar, cylindrical, or conical face. A limitation of this method is that the sketch plane must be tangent to the face.

   

   Spline Surface - This method will wrap the sketch on any face type. However, it cannot wrap around a model past 180 degrees. Therefore, it doesn't work well with cylinders and cones. This tool is best used when the analytical method produces an error or incorrect results.

   

7. When using the "Spline Surface" wrap method, additional options for "Accuracy" appear in the property manager.

   

   This can be used to increase the detail of the wrap feature, which is sometimes necessary for more complex geometry. Increasing this value can significantly impact performance. Therefore, it is recommended to keep it as low as possible.

8. Select the surface/face you would like to wrap your sketch onto.

   

9. Click the green check to complete the feature.

For further technical support, please contact Hawk Ridge Systems at 877.266.4469 for the U.S. or 866.587.6803 for Canada and support@hawkridgesys.com.