How do I use SolidWorks Draft & Wrap?

Solidworks has easy tools for applying draft to existing features. But when it comes to embossed wrap features it’s not quite as easy, so we’re going to need to get clever. Thus, I would like to introduce you to my 5 Step Method.


Step One: Create an embossed wrap

Create a simple Solidworks wrap sketch, then launch the Solidworks wrap command. Lastly, choose emboss method, and specify a thickness.

Solidworks wrap command, using emboss wrap type

Step Two: Create a scribe wrap

This step is a bit trickier, mostly because it requires some math. Don’t worry though it’s just a little trigonometry. Using scribe in a wrap projects the sketch onto the selected surface and creates a new face. I need to create a new sketch for this feature, and that is where the math comes in. If I break down my existing wrap into a 2D image I basically have one leg of a triangle. In this step, I want to add the other leg of the triangle. To determine the length of that leg, I’ll use my existing leg length (emboss thickness), and my desired draft angle. Then will a little help from trigonometry, I can calculate my leg length.


So now to apply that back to Solidworks. That “leg length” I just calculated will represent my offset distance. I will create a new sketch on the same plane as the first wrap. Then create offset entities of the original sketch towards the outside. The final step for this sketch is to convert the inside edge of my first sketch. Finally, I will scribe this sketch on the same surface as the first wrap.

Solidworks wrap command, using wrap type scribe

Step Three: Delete faces

I need to remove some faces to make room for a lofted surface. To do this use the Delete Face command, with the Delete option selected. This will give me edges that can be used to loft between.

Delete face command in Solidworks

Step Four: Create a lofted surface

A surface loft is basically the same as a solid loft, with the difference being it creates a surface not a solid. To create a lofted surface I need a minimum of two profiles to loft between. In this case, I want to connect the two “legs” of my triangle to create the hypotenuse. Or in other words loft between the outside each of the scribed wrap, to the outside edge of the embossed wrap. For selecting multiple edges, the SelectionManager is needed. This can be accessed from a right-click menu. The last trick is just to make sure both profiles were originally selected in a similar location.

Solidworks lofted surface command

Step Five: Knit surfaces

The previous steps left me with three separate surface bodies. To convert these back to a solid I need to knit them all together. The knit surfaces command lets me knit all three together and create a solid at the same time.

Solidworks Knit surfaces command. Create a solid.

And there it is. Five simple steps to apply a consistent Solidworks draft angle around an embossed Solidworks wrap feature.