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10 Steps to Creating Your First Product in SOLIDWORKS

CAD Simulation

10 Steps to Creating Your First Product in SOLIDWORKS

Understanding how to use design tools efficiently is critical to your career as an engineer. With this tutorial, we will create a simple part that is suitable for manufacturing using the least number of steps.

To get you up and running with your first part design, we’re going to be walk through a 10-step process of modeling a lightweight titanium camping mug from scratch. This model was chosen because of the relative ease with which it can be created. We’ll also touch base on some of the most critical SOLIDWORKS building blocks.

Once completed, the model will provide a perfect example of a product design that can either be rendered to communicate the design plan to others, 3D printed to create a physical prototype or used as a reference to create 2D drawings directly in the software, which can be sent off to a manufacturer for a production quote.

(1) Create a New Part

To get started, open up SOLIDWORKS and create a new part. In the Feature Tree to the left of your workspace, select Front Plane. In the icons above the working area, select View Orientation > Front. This ensures that you are looking directly at the front of the Front Plane, which is necessary to sketch with accuracy.

(2) Draw a Centerline

Now that you are looking directly at the Front Plane, head up into the Sketch Toolbar and select Line > Centerline. Once the Centerline tool is selected, place it in the very center of the Front Plane box over the directional red arrows. Follow your mouse directly straight up from the up arrow so that there is a blue dotted guideline, then click just above the Front Plane boundary box. To define the other end of the Centerline, drag your mouse back over the red arrow and click approximately just as far below the Front Plane boundary box as you clicked above it, then press Escape to drop the tool. This Centerline will be used as a point of reference as you move forward with sketching the camping mug profile.

 

(3) Sketch a Camping Mug Profile

With the newly created Centerline as your point of reference, select the Line tool again and being sketching the profile of your camping mug’s wall. The profile is the same as the cross-section of the wall if the mug were to be cut in half. Use this opportunity to be creative with the bottom edges and even the angle of the outer wall.

To quickly create a dimensionally accurate outer edge, sketch only one edge of the profile, make sure it is selected, and then use the Offset Entities command to duplicate your sketch. Note the properties of the command in the window to the left, including distance and which side of the original sketch you will be using to create the duplicate entity. Once you have two parallel lines that represent the inner and outer walls of your camping mug, close off each end of the lines using the line tool so there are no empty gaps between them.

When you are finished, confirm that you are done sketching by exiting the sketch in the upper right-hand corner.

(4) Revolve the Profile

Now that you have completed the profile of your camping mug, it’s time to revolve it 360 degrees to create a watertight vessel. Do this by selecting the outer edge of your profile sketch, then navigate up to the Features toolbar and select the Revolved Boss/Base command.

If your sketch was completed in Step 3, the software should have already fired off the Revolve, and you should be left with a yellow cup-like object that follows the outline of your original profile sketch.

If for any reason you encounter an error, simply go back to Step 3 and ensure that your profile is complete.

(5) Sketch the Handle Profile

Now that the main portion of your camping mug is complete, it’s time to add a handle. Similar to how you sketched the original profile of your mug, you’re going to select the Front Plane from the Feature Tree on the left side of the screen. To ensure that you are working flat on the Front Plane, head up to the View Orientation icon at the top of the workspace and select the Front view.

To make sure that your handle isn’t floating in space, you need to ensure that it pierces the outer edge of your mug. To do this, head up to the Display Style icon at the top of the workspace and select Hidden Lines Visible. This will allow you to see both the inner and outer edges of the mug. Using the Line tool found in the Sketch toolbar, create the first point of the handle profile on the inner edge of the mug, which will turn orange when you mouse over it.

Bring out your sketch and create a natural handle profile. Feel free to be creative here and explore other sketching tools such as the Sketch Fillet, which will add a rounded edge to any sharp corners.

Finish up by connecting the last point of your sketch on the same inner wall that you started from.

(6) Create a New Plane

To build the handle, you’re going to need to create a new point of reference to build from. To do this, you’re going to create a new plane.

In the Feature Tree, select Right Plane, then mouse over the SOLIDWORKS logo in the upper left-hand of the UI until the additional program options (File, Edit, View, etc.) become visible. Navigate over to the Insert menu and locate Reference Geometry > Plane. You now have an additional working plane that is parallel to the existing Right Plane.

To align this new plane to your handle profile, move your mouse cursor over to the first point you made when you sketched your handle until the point turns orange, then right-click and press the green check mark in the upper right-hand corner of the workspace. You’ve now created a new working plane on the edge of the camping mug from which to create the body profile of your handle. To make sure that you can distinguish it from the other planes, rename it as “MugEdge.”

(7) Sketch a Handle Body Profile

Now that you have created the “MugEdge” plane from which you can build your handle body profile, it’s time to make sure that you’re working on it accurately. To do this, head up to View Orientation icon and select Normal To. This will place your view directly over the MugEdge plane.

Now that you’re looking directly at the top of your mug, navigate up to the Sketch toolbar and select Straight Slot > Centerpoint Straight Slot. This will allow you to build a symmetrical slot from the midpoint.

With the Centerpoint Straight Slot tool active, hover your mouse over the first sketch point of your handle until the line turns orange, then click. Using the guidelines that appear, drag out to the width that you want for your handle––but keep in mind that it doesn’t need to be too wide. Once you have chosen the width you want, click again. Now drag your mouse up or down to repeat this process for the mug’s height. Again, remember to think like a designer and not go overboard with a design that requires too much material or that creates a mug that would be difficult to hold.

Once you are satisfied with your design, confirm that you are finished sketching by exiting the sketch in the upper right-hand area of the workspace.

(8) Sweep the Handle Body

Now that you have a profile and a path for creating your handle, you can run the Swept Boss/Base command to actually make the handle a physical part of your existing mug.

Do this by navigating to the Features toolbar and selecting Swept Boss/Base. In the profile dialog box (blue), select the profile of the handle body that you just created with the Centerpoint Straight Slot tool. Follow this by clicking on the handle profile sketch for the path dialog box (pink). If all of the sketches were completed accurately, the software will automatically create the handle based on this profile and path information, which will be highlighted in yellow.

To confirm this process, simply select the green check mark in the upper right-hand corner of the workspace.

(9) Adjust the Dimensions or Proportions

Now that you have completed the first iteration of your mug design, you have a better understanding of how your earlier design decisions led to the final proportions. If you need to make any changes, simply go back into the Feature Tree and edit a sketch.

(10) Add Fillets and Design Details

To add the finishing touches, it’s time to go around and refine the sharp edges with a fillet. Even if you don’t particularly care for a heavy rounded edge aesthetic, it’s important to consider that most objects in the real world that appear to have a straight edge actually have a small fillet on the corner as a natural side effect of the manufacturing process. Again, this is an opportunity to be creative and get your feet wet.

Now that you’ve designed a camping mug, it’s time to make a 3D-printed prototype to see how your design translates in the real world, create a rendering to communicate how the mug would look in a particular setting, or create a SOLIDWORKS drawing to send the mug off to a manufacturer and see what is involved with bringing the design into production.


About the Author

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Simon Martin is a writer and industrial designer in New York City.

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