Differentiating Between the Sweep and Loft Commands on Solidworks 2020

This instructable is designed to help differentiate the uses and methods of creating a sweep or a loft in Solidworks 2020, 2019, or 2018. I write this for people who have some introductory modeling experience in Solidworks.

For the purposes of TDE 331 (disregard this bit if you are not my teacher or classmates), this instructable is designed to apply to Standards for Technological Literacy Standard 19, Benchmark H. Standard 19 covers manufacturing technologies, and Benchmark H states "the manufacturing process includes the designing, development, making, and servicing of products and systems".

Supplies

Solidworks 2018 or newer

Step 1: Step 1: Model the Mug

Note: The dimensions in the model are up to you. I would recommend using the same dimensions for ease of comparison between my model and yours. I added the dimensions for the purpose of adequately defining my model.

Start by opening a new part file and choosing the front plane to create your first sketch.

Using the line tool, create half of the cross-section of the mug and the centerline.

Under the Features tab, select the Revolved Boss/Base tool. Select the vertical centerline as the Axis of Rotation and set the Direction 1 to 360 degrees.

Also under the features tab, select the Fillet tool. Select all of the face intersections except the intersection between the outer wall and the bottom of the lip and set the fillet radius to .1

Using the same method, fillet the underside of the lip and outer wall using a radius of .5

Congratulations, you have most of a mug.

Step 2: Step 2: the Sweep Command

Now to create a handle for the mug using the sweep command.

Before you can make the sweep, you will need to create the path that the handle follows and the cross-sectional profile of the handle.

To create the handle shape, I used three circles. The top circle has a coincident relation to the upper left corner of Sketch2. The middle circle is has tangential relations to the other two circles and to the inner wall of the mug. The lower circle is also set tangential to the inner wall of the mug. To show the original sketch, click the dropdown arrow beside revolve2, click sketch2, and then click on the eye logo to show/hide that sketch. Draw a line from the direct bottom of the top circle vertically down to where it is tangential to the bottom circle.

Under the Sketch tab, use the Trim Entities tool to remove the outer profiles of the upper and lower circles and the inner profile of the middle circle. Delete the line you made previously to create and open path.

Click exit sketch. You now have the handle shape.

To create the handle cross-section, find the reference geometry tool under the Features tab and select Plane from the dropdown menu. Select the Right plane from the file tree as your first reference and the inner wall of the mug as the second reference.

Make a new sketch on the plane you made. I used a circle for the sake of demonstration. You can use any shape. Make sure that the end of the handle shape is within the shape.

Under the Features tab, select the Swept Boss/Base tool. Select the shape you just made as the first option ad select the handle shape as the second.

Click the green check mark and now you have a mug with a handle that has a circular cross-section throughout the length.

Step 3: Step 3: the Loft Command

To start the with the loft, you will need to remove the handle you have just created, or you can quickly make a new part with the same mug. I would recommend the latter, but otherwise, use ctrl+z to back up the the point where you have the handle shape and the circular cross-section.

The loft tool is designed to follow a path that has differently shaped cross-sections throughout, unlike the sweep which can only handle one cross-section.

For this handle, you are going to make an elliptical cross-section for the side part of the handle to create a nice, flatter surface for the mug to rest around your hand. To do this, you will make a second circle for the bottom end of the handle and two ellipses for the middle of the handle.

To create the circle at the bottom of the handle, create a plane using the bottom face of the mug as the first reference and the point at the bottom end of the handle path as the second reference. Sketch a circle on this new plane with the center set coincident to the point selected above. Exit this sketch.

To create the ellipses, create a plane using the Right Plane as the first reference and the tangent point on the handle shape as the second reference. Draw an ellipse centered on that point. draw a second, preferably identical, ellipse where the handle shape passes through the plane and use the Pierce relation to constrain the ellipse. Exit the sketch.

Under the Features tab in the same place you found the Swept Boss/Base, select the Lofted Boss/Base. For the first reference, select the original circle from the cross-section and then select the two ellipses in order, and then select the bottom circle, making sure to click the green check box whenever it appears. This will give you a shape that doesn't match the handle shape you want.

Within the Loft options box on the left, click the dropdown arrow on the Centerline Parameters option and the select the handle profile you made earlier. This will cause the shape to remain yellow, but match the desired shape. Click the Green check, hide all the sketches and planes using the eye icon, and ta-da, you have a handle with multiple cross-sections.