The SOLIDWORKS 3D Sketch Golden Ticket

3D Sketch is a powerful, if challenging tool. Here's how to use it better, by making Willy Wonka's Everlasting Gobstopper.

I tried to re-create Willy Wonka’s Everlasting Gobstopper, and let me tell you that simple looking little piece of candy was not so simple to model. No wonder Mr. Slugworth was trying to steal the secret! I tried approaching it with several different techniques and, in the end, the results I desired required 3D sketches. I would like to hand you the SOLIDWORKS golden ticket to the secrets I learned and discoveries I made while working with 3D sketches to model this fictional candy.

Creating Geometry

In a 3D sketch, new geometry can be created in three dimensions by referencing bodies, planes, surfaces, or vertices which already exist. This can be as simple as converting edges or clicking on vertices for starting and ending points of the geometry. In my Everlasting Gobstopper model, I used the edges of a solid body to create construction geometry in three dimensions. I then used the midpoint of this construction geometry to sketch the centerline geometry for a loft to make the candy branches.  I found creating the centerline free hand, without anything to reference, the most challenging part about using a 3D sketch.

When creating free hand geometry in a 3D sketch, I think the most important thing to understand is that sketch geometry is inherently 2D. This means that even though three dimensions are potentially available, it will default to only using two when geometry is first created. After it is created, the geometry is then able to be dragged and positioned in three dimensions. I used my cursor feedback to take advantage of this.

When I created my 3D sketches for the candy branches, I paid particular attention to my cursor and space handles. The cursor identified the axes labels comprising the plane I was currently working on. The space handles displayed arrows mimicking the global coordinate system where I last clicked and highlighted in red the two axes creating the plane I as currently working on. If I needed to switch orientations, I used the tab key to rotate through the three plane options. These two items helped me to orientate the geometry when I was initially placing it in my sketch. Once placed, I repositioned the end of the geometry to make the branches look more organic.

Another available option to help you take advantage of the default two dimensional inclination of sketch geometry in a 3D sketch is a 3D sketch plane. A 3D sketch plane is a 2D plane that only exists inside the 3D sketch. When activated, sketching will happen exclusively on that plane and you will get behavior similar to when working in a 2D sketch. To add a 3D sketch plane go to Tools>Sketch Entities>Plane. To use an existing plane in a 3D sketch, select the plane and go to Insert> 3D Sketch On Plane or double click on the plane. I didn’t use this technique in my model, but I thought it was worth mentioning.


Automatic relationships are still indicated through the yellow flags next to your cursor in a 3D sketch. However, in a 3D sketch you will find there are fewer instances and types of relationships that can be added automatically. In my Everlasting Gobstopper 3D sketches, my use of an existing body and construction geometry did not require me to add any additional relationships. However, I found it helpful to review all the different types and necessary selections for relationships in a 3D sketch because they are different.

All the existing relationships that you can have in a 2D sketch are still available. However, some of these relationships will have additional options or requirements in a 3D sketch.

There are also additional relationships that only become available to you in a 3D sketch.


Once I had the centerline for my Everlasting Gobstopper candy branch in the correct position, my last step was to add dimensions, which would fully define the sketch. Fully defining a sketch is an import best practice that should always be followed, especially in 3D sketches.

When adding dimensions in a 3D sketch, by default you will start out with the absolute value. If you would like the dimensions to only be along one direction, you can use the tab key to switch to just along x, along y, or along z. By continuing to hit tab will cycle you back through the options starting at absolute again. The cursor will update to tell you which direction the dimension is along.

Working with a 3D Sketch can be challenging, however, it is a useful tool. Like my Everlasting Gobstopper, there may be times when a 3D sketch will be necessary and I hope now you will be more comfortable working in this sketch state with SOLIDWORKS. If you don’t believe me, just listen to the Oompa Loompas!

Oompa loompa doompety doo
I’ve got a model challenge for you
Oompa loompa doompety dee
If you are wise you’ll listen to me

What do you get when you try something new
Modeling as much as you engineers do
Why 3D sketches are not so hard now
Not when CADimensions showed you how
You will really like the look of it

Oompa loompa doompety da
If you 3D Sketch then you will go far
You will model in happiness too
Like the oompa loompa dompety doo!

Happy Modeling!