Modeling Thin Walled Parts | TriMech Training Tidbits

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I’ll guide you through the process of modeling a thin walled part that includes a revolved feature. Specifically, something most of us need during our workday, a ceramic coffee cup! The tools and techniques shown here are from the part modeling lessons in the SOLIDWORKS Essentials class. The coffee cup is loosely based on one of my favorite glass mugs, which is entirely unsuitable for hot drinks.

Key Takeaways for Modeling Thin Walled Parts

In the process of modeling this part, we’ll cover:

• Open Profile Sketches
• Doubled Dimensions
• Convert Entities in a Sketch
• Revolved Features
• Swept Features
• Thin Features
• Full Round Fillets
• Materials & Appearances

Open Profile Sketches and Doubled Dimensions

The sketch shown below, created on the Front Plane, is what we’ll use to create the main body of the coffee cup. The 3 dashed construction lines will not extrude to create a 3D model. Only the three solid lines and the two sketch fillets connecting them will extrude. Notice the area is not shaded because the construction lines don’t count as part of the sketch contour. So, this is an open profile sketch.

Open profile sketch for revolved thin feature

The two diameters are doubled dimensions. The trick to creating them is having a center line (aka construction line) to dimension to. Using the Smart Dimension tool, select the centerline and another entity (such as a line, point, etc.). Before you place the dimension, move your cursor to the opposite side of the center line from the other entity. The dimension will automatically be doubled.

Modeling Revolved Features and Thin Features

Now we can launch the Revolved Boss/Base command. A pop-up will appear to warn us that the sketch profile is open. It will ask us if we want the sketch to be automatically closed. If we select Yes, it will alter the sketch to make it a closed profile. If we select No, the Thin Feature section of the Property Manager will be activated.

First, let’s deal with the requirements of any Revolved Feature. The Direction defaults to Blind and 360°, so the contour will be revolved all the way around a central axis. If only one center line exists in a sketch, it will automatically be selected as the Axis of Revolution. If there are multiple center/construction lines in the sketch, as is the case here, we’ll have to select which one we want to use.

Creating the revolved feature for a thin walled part

Second, let’s look at the additional controls for a Thin Feature. Extruded Bosses and Cuts can use the Thin Feature functionality, whether the sketch is an open or closed profile. When the Thin Feature section of the Property Manager is activated, sketch entities will be given a specified thickness as they extrude. We can choose to add this thickness to either side of the entities, or a different amount to each side, or select the Mid-Plane option as shown below.

Using Convert Entities for the Model Base

Now that we have the cup shape with a wall thickness of 1/4 inch, it’s time to add the base. We’ll make it nice and wide because nobody wants spilled coffee.

We’ll start a new sketch on the Top Plane. What we want is a circle that exactly matches the upper edge of the Revolved Feature. Select the edge and then click Convert Entities on the Sketch tab of the Command Manager.

Using the Convert Entities command to make the base

A new circle entity will be created, projected into the sketch from the model edge. An On Edge sketch relation will make sure it remains the same as the edge it was created from. (If you select a face to convert, all its edges will be projected into the sketch.) This ensures that if we change the outer diameter in the future, the base will change to match.

Now we can create an Extruded Boss. We’ll give it the same 1/4 inch thickness as the Revolved Boss. Use the Mid Plane end condition so that we’ll get 1/8 inch extruded above and below the sketch plane. That will make sure we don’t get any unexpected gaps in geometry due to the angled side of the cup.

Creating a Path Sketch for a Swept Feature

We need a sketch to define the cup’s handle. Since the handle needs to be attached to the wall of the cup, we can select Sketch1 in the Feature Tree and click Show in the Context Toolbar. To make Sketch1 stand out better, right-click it in the Tree and select Sketch Color from the Context Menu. Pick a color, such as magenta, which will stand out better.

The path sketch for a sweep shown in magenta

Now we can create a new sketch on the Front Plane. As shown above, it will consist of a horizontal line, an arc, another line, and another arc. This is another open profile sketch with the upper and lower endpoints attached to lines in Sketch1 with Coincident relations. Dimensions and geometric relations can then be added to fully define the handle shape.

Extruding a Swept Feature with a Circular Profile

The new sketch will be the path of a Swept Boss. When creating this type of feature, we take a cross-section profile and sweep it along the path.

There are two Profile options in the Sweep Property Manager: Sketch Profile and Circular Profile. In either case, we need to specify our path sketch in the appropriate field.

Using a circular profile for a Swept Feature

If we want a simple circular cross-section, we can just give it the diameter value and hit OK. If we want any other cross-section, we have to create a profile sketch first. Here we just want 1/2″ diameter for the circle, so we only need one sketch.

Creating Constant Size Fillets

Our sketch-based features are done, but we need fillets to round off sharp edges. We need two Constant Size Fillet features, as shown in the Section View below.

Quarter and half-inch fillets on the model

Half-inch radius fillets are added between the two edges where the Revolved and Extruded Bosses meet. Quarter-inch fillets are added to the two edges where the Swept and Revolved Bosses meet.

Using Full Round Fillets for Automatic Dimensions

There are four different types of fillets, with many options available. Constant Size fillets are the most common. The others are Variable Size, Face, and Full Round Fillets, the latter of which we’ll use to round off the lip and base of the coffee cup.

A Full Round Fillet replaces a flat face with a curved one without needing to input dimensions. The Property Manager has different selection fields for the center face we’re replacing and the faces to either side of it. We can’t create multiple fillets as part of the same feature due to the nature of the tool. So, after rounding off the lip of the cup, we can add another fillet to round off the base.

Using Full Round Fillets to round off a flat face

TIP: If you tap the right button immediately after selecting a face, the active selection field will be advanced to the next one to save you some mouse travel. After the last selection, tap the right button again to finish the command.

Apply Material Properties to the Cup

Geometrically, the cup is done. But we can still assign material properties to the model, along with a more realistic appearance. Right-click Materials in the tree, and the Material dialog box will appear. Browse the database to find an appropriate one, such as Ceramic Porcelain. The new material and appearance will be assigned to the model when we hit the Apply button.

Applying a material to the model

Edit Appearance to Fine-Tune Looks

There are many ways to add and customize the appearance of a model. All we need to do in this case is give our cup a more interesting color. Click Edit Appearance on the Heads-Up Toolbar, then pick a color from the palette and hit OK.

The coffee cup colored in SOLIDWORKS red

I went with SOLIDWORKS red for my coffee cup. To turn off the display of the black edges, select the Shaded Display Style from the Heads-Up Toolbar. 

Gaining Valuable SOLIDWORKS Skills

SOLIDWORKS is capable of modeling nearly any part you can dream of. The SOLIDWORKS Essentials class provides you with the tools and techniques you need for many part models. More advanced tools, features, and options are covered in the SOLIDWORKS Advanced Part Modeling class, and the SOLIDWORKS Surface Modeling class builds from there.

Take all three classes and you’ll be able to create everything from simple hardware to complex, organic-looking designs. One of the ways we help is with our SOLIDWORKS Training Passport, which enables you to take a range of classes on your own schedule at a lower cost than registering for the classes individually.

Learn more about the SOLIDWORKS Training Passport »