Wrap and Circular Pattern tools: Model a Beer Mug with SolidWorks

This tutorial aims at, among other things, getting familiar with the Wrap tool through the modelization of a beer mug in SolidWorks.

As you can see on the cover picture, the mug consists in a revolved profile that is somewhat more curved than a mere cylinder. It makes the wrapping process not trivial.

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Open a new part by going to File > New… > Part.
Start a new sketch on the front plane:

Add these lines first. The vertical one in a construction line (you can access it by expanding the Line icon). It won’t matter in the final profile. It simply helps constructing the sketch, hence its name.

Go ahead and add a Spline:

In order to properly define this Spline, we need to dimension the two blue handles by specifying their direction and magnitude. To do so, add these Construction Lines and their respective angular dimensions:

Click on one handle and on the oblique line associated while Shift is pressed to add a Parallel relation.
Add the rest of the sketch. The second Spline has its handles parallel to the construction lines too. Define the magnitude by clicking on the handles with the Dimension tool enabled.

The sketch is now ready to be revolved. Find the Revolved Boss/Base tool in the Features tab:

Let’s refine the shape a little. Add a special kind of Fillet ( Features tab) to the upper surface, by selecting the Full round fillet option. The upper surface needs to be added in the purple box, and the two adjacent surfaces in the other boxes.

Now, on the top plane, add a circle whose center is the origin and diameter is 40 mm. After exiting the sketch, use the Extruded Cut tool to remove 5 mm of matter:

Find the Draft tool in the Features tab and apply a 30° draft to the cylindrical surface you just created. Select the base of the mug as support:

The global shape is done. It is time to carve the motives in the glass.

The Wrap tool literally allows us to “wrap” a planar sketch around a curved surface, a cylindrical shape in most of the cases. Unlike a regular cylinder, the mug as not a constant radius. We thereby need an idea of the space we have to draw our sketch so that it can be wrapped and repeated 10 times around the mug.
I drew a simple figure to explain what will follow. The grey surface is the mug, a black sketch is drawn on a blue plane and is wrapped around the mug to give the yellow profile. What the figure illustrates is that the sketch is drawn with the projection of the grey curve on the right-hand side. However, once wrapped around the mug, the yellow profile doesn’t reach this grey curve. It is not hard to visualize, since the wrapping distance is greater than a simple projection. We will use this distance between the grey curve and the wrapped content as a little space between the motives.

One motif is repeated 10 times around the mug. Each motif is symmetrical, that is, we only need to draw one half. As a matter of fact, we need to draw the profile within 360 / (2 * 10) = 18°.
Draw these perpendicular lines over the top plane:

Go to Insert > Surface > Extrude… and extrude this pair of lines through the entire model.
Start a new 3D Sketch:

Find the Intersection Curve tool:

Select the outer surface as well as the two previously extruded surfaces.

Go to Insert > Features > Delete Body… to delete the pair of extruded surfaces since we do not need them any longer.
On the right plane:

Draw some lines over the construction lines, and convert the entities of the 3D Sketch by finding the Convert Entities tool:

Use the Trim tool to get rid of the unwanted parts of that sketch.

Exit the sketch. Find the Wrap tool.

Use the Deboss option to remove volume.

Use the Mirror tool on the last feature:

Add a 3 mm Fillet to the motif central face:

Add extra Fillets here as well:

We will repeat a similar process on the front plane.

The last profile was on the right plane. The number of occurrences allows us to draw the new motif on the front plane so that it starts at half the length of the previous profile.

Repeat the previous steps:

We now need to add the third layer of motives. The process is always the same. On the right plane:

Find the Circular Pattern under the Linear Pattern icon.
Fill the panel just like I did with the first two layers.

We do not repeat the third layer because we need to get rid of one of its occurrences separately.

Enter the Circular Pattern tool a second time. Add the relevant features but this time skip the instance facing the right plane (the orange dot on the picture below):

The next step is to model the handle. To do so, we are going to sweep a profile along a path.

On the front plane, start a new sketch on the skipped occurrence side:

Note that both handles have a horizontal relation. This profile is the path.
Now, on the right plane, add a new sketch. Add a rectangle by placing its center where the path starts.

Then add 2.5 mm Sketch Fillets to the corners:
Find the Swept Boss/Base tool in the Features tab. You want to select Twist Along Path to get a nice handle without separation and uncheck Merge result:

Finally go to Insert > Features > Split… in order to split the handle and remove to unwanted parts.
Select the outer surface and the surface of the motif directly in front of you while looking from the right as trim tools. Let the computer perform the calculation and cut the parts:

Combine both bodies by going to Insert > Features > Combine….
Add some Fillets and the mug is finished!

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Get this tutorial as a PDF file and download the SolidWorks source files.
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