In this tutorial, I will walk through how to model a 10-inch cast-iron skillet using SOLIDWORKS. The skillet happens to be the item that I most often use in my kitchen. After I design the model, I will use SOLIDWORKS Simulation to test the design. 

First, let us start with a blank document and make sure to set the units of measurement correctly. Every piece of geometry that we do in SOLIDWORKS starts with a two-dimensional sketch. In this case, we will create a simple circle to start us off. We use sketch relations and dimensions to fully define the geometry before applying three-dimensional features like a drafted extrude. Make sure to draft this outward at a 20-degree angle. This is a good starting point for our design. Next, we are going to add a three-quarter inch and fillet to the bottom edge to represent the rounded portion at the bottom of the pan.Next, we need to hollow out this volume. We are going to do this with a revolve sketch, and instead of making it from scratch, we will use the offset tool to create new geometry from the already existing geometry from previous features. To do this, we will move it to the inside by using the reverse option, and we automatically get the new radius calculated for us. Next, we add a centerline and close off the contour the way we want it making sure to revolve this around the correct axis.

Creating and adding the handle to the design 

Next, it is time to make the handle, and we are going to make this as simple as possibly starting with a circle and two tangent lines. Again, sketch relations and dimensions are used to fully define this geometry. Finally, the trim tool can be used to slice out the line segment in the middle to create a single, closed contour. We can extrude this down 0.4 inches into the middle of our skillet. Now we are left with a little wedge of material in the middle that really does not belong. It would have made more sense to add that feature before adding the cut. No worries, we can simply reorder our features so that the cut happens after the handle has been added.

Next, we are going to add some more fillets. We want some large fillets set at a one-and-a-half-inch radius where the handle meets the pan. Then we will use a full-round fillet to round off the outside edge of the handle. We do this by simply picking on faces of all sides, and SOLIDWORKS calculates the radius for us.

Now we can see that it rolls in a little bit, but we need to create a rim anyway. To make this easier, we change to a wireframe view and add a simple sketch that we are going to revolve around. We do not need any dimensions in this sketch. We are going to reference the height of the one blue line (shown below) to be co-linear with the bottom of the other handle. Then we can simply add another center line and we will be able to revolve this. 

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Adding the helper handle to the skillet

Next, we are going to add another sketch to create the helper handle and for this one, since we have a symmetric shape to create, we are going to add a centerline and activate dynamic mirror entities. Now, when we create our lines, they will be reproduced on the other side of the mirror line. We will also copy the inner diameter to close off that shape and trim away the excess geometry.

We will use the offset tool once again to create the hole in the middle and a constant offset from the existing shape. We will then extrude this down and round it out with the fillet tool. And there is no need to pick every single one of the edges necessary because SOLIDWORKS is going to offer us quick groups of edges that might be the ones that we want to pick.

Finally, we need to create the hole at the end of the handle, but we want to make our sketch halfway in the middle of that handle. So, we are going to create a new sketch plane that sits at the mid-plane of the two existing surfaces and create a sketch there. We wake up the center point and make another simple teardrop shape. Only a few quick dimensions and sketch relations later and we will have a fully defined shape.

Next, we will use the trim tool to trim it down to have a single closed contour. Then we are going to use an extruded cut in both directions from the mid-plane and we will add a 45-degree draft angle going outward to create the unique shape of the hole in the handle. Lastly, adding some small fillets to those edges will smooth that geometry out and make it look just like the real thing.

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Testing your design with SOLIDWORKS Simulation

Our last step is to define the material by telling SOLIDWORKS that this part is made of cast iron, which will then allow us to get accurate properties either for simulation or just to take the mass properties.

We will now look at simulation, it is quick and easy to set up a simple, linear, static study to test the strength of the handle or simply add a fixture on the bottom of the pan as if we’re clamping it in place.

When Simulation is run, it is going to break this geometry down into many small tetrahedral elements and brute force solve the equations necessary to get a solution. We can see an exaggerated displacement, giving us an intuitive idea of how the handle bends and where the maximum stresses are. This will help determine if these areas need more material to make the pan stronger.

The final simulation test we will do is a drop test. We can test if the pan was dropped from a height of 1000 millimeters right down on the tip of the helper handle. Below we see an animation of how the stresses propagate through the material as it is dropped.

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