Introduction

Welcome to the world of SolidWorks. As of 2022 SolidWorks was the 2nd most used CAE/CAD (Computer Aided Engingeering/Computer Aided Design) software used in the proffesional sector. SolidWorks allows the user to design and model a system of parts as well as test them in various simulations. You are able to run tests for adding stress/force to parts, fluid dynamics, and other situations. After completing this training manual you will understand how to use various tools in SolidWorks to design simple parts and assemblies both from scratch and premade templates. You will also gain an understanding of general constraint conventions and good practices.

Downloading SolidWorks

If you have a CAE account the first thing you will need to do is install SolidWorks on your computer or use one of the computers in the engineering computer labs in or der to follow along with the learning activity and practice SolidWorks in general. You should be able to find SolidWorks at https://software.wisc.edu/cgi-bin/ssl/csl.cgi under the productivity section.

After clicking on SolidWorks you will be redirected to a new page where you will have to enter your email and then proceed by downloading and following the installation wizard. I am currently working on finding out if we can get temporary access to CAE computer labs for trainers to learn the software in those labs. (Or some kind of solution that gives none engineering major trainers access to the software.)

You will need a CAE account to download SolidWork.

Outcomes and Objectives

In this manual you will learn how to create simple sketches, turn sketches into parts, and then turn those parts into an assembly

• Sketch - A sketch is a two dimensional representation of the part you are trying to model.
• Part - A part is just a sketch that has been given three dimensional constraints and is represented and manipulated in 3D.
• Assembly - An assembly is a combination of parts into one model.

Setting Up Your Workspace

An important part of using SolidWorks, and most computer programs, is having an organised virtual workspace. In SolidWorks this mostly just means that you know where all your files are and where to find them, however you decide to do that is up to you.

Dimensions

The last piece of housekeeping information before we get into the guts of SolidWorks is dimensions. When you open SolidWorks and start a new project you will see the letters “IPS” with a little arrow pointing upwards in the bottom right corner. You can change the dimensions by clicking on the small arrow. (Instead of "IPS" you might see "MMGS", "CGS", or "MKS"). The most common two that you will use are IPS and MMGS. “IPS” stands for inches, pounds, and seconds while "MMGS" stands for millimeters, grams, and seconds.

Getting Started

SolidWorks Workspace and Vocabulary

We will begin by getting oriented with the SolidWorks UI. As soon as you open SolidWorks you will be prompted to create a new part, assembly, or drawing as shown in Figure 1.

In this workshop we will be focusing on parts and assemblies only. Within those two we keep it pretty basic, looking at the most important tools for getting started on designing your own parts. Once you start a new part you will be presented with the standard SolidWorks workspace

At the center of the screen you can see a three dimensional axis which is the origin of your workspace. On the top right of your screen you can find the ribbon. This is where you will find your tools and other useful options. Below the ribbon you will see various tabs that read “Features”, “Sketch”, “Markup”, etc. These tabs will give you access to different ribbons for different stages of developing your part. On the left side of the screen, below the tabs, you will see the FeatureManager design tree. This will mostly be used for selecting and editing sketches and other components of your part. When you create a new sketch or component it will appear in this window.

Tools

Sketch Tools
All these tools are located in the sketch ribbon.

Sketch tool - Furthest left button in sketch ribbon. Used for starting a new sketch.
Smart Dimension tool - Located on the right of the Sketch tool. Used for defining dimensions of shapes and distances.
Shaped sketch tools - Circle, ellipse, line, square, and other shape options are available for creating your sketch. Located to the right of the Sketch and Smart Dimension tools.

3D Tools
All of these tools are located in the Features ribbon.

Extruded Boss Base - This tool is located on the far right of the Features ribbon and is used for giving your sketches a third dimension.
Extruded Cut - This tool is located to the right of the Extruded Boss Base tool and is used for making cuts through your part. The cut shape is dependent on the sketch shape you outlined for the cut. (For example, if you were modeling a DVD you would need to first create a 3D disc and then add a second circular sketch in the center as the basis for your cut.)

Assembly Tools
All these tools are located in the Assembly ribbon.

Insert Components - This tool is located in the top left of the Assembly ribbon, and will be used to import parts into your assembly workspace.
Mate - This tool is located to the right of the Insert Component tool and will allow you to create relationships between different parts you have imported.

Understanding Sketches, Parts, and Assemblies in SolidWorks

Sketches

Sketches are always the beginning of your SolidWorks part development. The sketch represents the 2D silhouette of your part. You can create pretty much any shape you wish with all sorts of cutouts. Unlike assemblies, you are able to create and manipulate sketches and parts in the same SolidWorks file. An important note is that you can also create a sketch on any surface, including the surface of a part or an extra plane you have created.

Parts

Parts always start their life as 2D sketches which are then turned three-dimensional by adding thickness to said sketch. As previously stated, you can start a new sketch on the face of a part, this helps to create cuts in your parts or a material projection. There are many tools that help you edit your part such as the “Fillet” tool which creates softened edges to your part. We won’t be going into detail on these tools but you can obtain a basic understanding of them by experimenting on your own. Another interesting functionality of parts is that you are able to change what your part is made from so it has the material properties of whatever material you choose.

Assemblies

Assemblies are a great way to test the geometric constraints, performance under stress, and other properties of your product before it is physically produced. Because of this most prototyping starts as an assembly where tests can be ran on them. Assemblies are combinations of various parts you have designed and connected in a way that mimics their real world functionality. The workspace interface of an assembly is laid out the same as it is for a part but some of the ribbons and tools are different. For example, the Feature ribbon is gone but you have the Assembly ribbon now. The main tool you’ll be using for connecting parts is called the “Mate” tool. The “Mate” tool allows you to connect parts together by their surfaces or their edges.

Guided Activity

Starting a New Part

1. To begin, open SolidWorks and select "Part" in the "New" section of the pop up window or use File --> New --> Part.
2. To orient the camera first, find the "Front Plane" on the left side panel. Right click on "Front Plane" and click the "Normal Too" button.

   

Beginning a Sketch

1. Click on the "Sketch" tab above the workspace window. You should see a section of the "Sketch" ribbon that has a line, circle, square, etc. These are the main tools used for sketching.

   

2. Select the "Straight slot tool" in the bottom left corner of the tools, this is for creating rounded rectangles.
3. Click on the origin which is at the center of the front plane and has an arrow for the x,y, and z axis (a small circle should appear)
4. Drag your cursor directly left or right of the origin, a straight line should appear.
5. Click again to create a line of any distance, we will define the lengths later.
6. Click one more time to define an arbitrary height and radius for the rounded rectangle as shown in Figure 5.

   

Defining Your Dimensions

1. To define our new dimensions we will use the "Smart Dimension tool"
2. Select the "Smart Dimensions" tool that is located directly left of the sketch tools previously mentioned.
3. Click the dimension defining the length of our rounded rectangle and set a new distance of 7 inches.
4. Click the height dimension and set a new height of 1 inch.
5. Click the "Smart Dimension" tool again to deselect it or use the Escape Key.

Editing Your Sketch

1. Select the "circle" sketch tool now.
2. Click on either end of the horizontal centerline of the rounded rectangle.
3. Drag your cursor out and click to define a circle with any radius.
4. Repeat steps b and c for the other end of the line.
5. Select the "Smart dimension" tool to dimension the circles.
6. Click on the outer rim of either circle (this will allow you to dimension the diameter).
7. Change the diameter to 0.5 inch for both circles.

Making Your Sketch a Part

1. Select the "Features" tab directly left of the "Sketch" tab.

   

2. Click the "Extruded Boss/Base" tool on the ribbon directly above the "Features" tab. You should see a yellow shell pop out from the sketch and give thickness to our rounded rectangle.

   

   Notice that the left panel has changed to give us options for the "Boss-Extrude"
3. In the "Direction 1" section find the D1 entry box and enter a dimension of 0.25 inches.
4. Click on the green checkmark on the top of the left panel or use the enter key to complete the extrusion. We now have the template for all of the parts that will make up our assembly.

Saving our new part

1. Click "File" on the top left of the screen.
2. Find and select the "Save as" button.
3. Name the part "link_template" as this will be used as the template for the rest of our links.
4. Save to your desired location.
5. Repeat steps 1-4 to create a file named "link_1". Now we have the template and the first link for our assembly.

   

Altering Parts

1. We need to create three more links at different lengths of 6, 5, and 3 inches so we will re-dimension our template and save it as a new file three times.
2. On the left panel find "Boss-Extrude1" and click the drop down arrow directly to its left.
3. Right click the "Sketch1" which just appeared.
4. Select the "Edit Sketch" button above the right right click menu.

   

5. Select the length dimension and change it to 6 inches.

   

6. Save this new part as "link_2" (SolidWorks may prompt you to rebuild the part, if so, rebuild it).
7. Repeat steps 2 through 6 to create link 3 at a length of 5 inches and link 4 at a length of 3 inches.

   

   Above is link 3 which should be 5 inches long.

   

   Above is link 4 which should be 3 inches long.

Creating an Assembly

At this point you should have files for a template and 4 links at 7, 6, 5, and 3 inches long. Now we will create an assembly so we can set relationships between all of our parts.

1. Click File --> New --> Assembly.
2. The left hand panel will give you the option to import and parts that are currently open, beneath the window of available parts there is a "Browse" button, click that.

   

3. Find and select "Link_1".
4. Click anywhere on the workspace to place our first link.
5. To keep yourself oriented you can right click on the face of our link and use the same "Normal too" option.
6. Find and click the assembly tab underneath the ribbon.
7. Above that and to the right you will see the "Insert Components" button, click this.

   

8. This brings back a familiar panel, repeat steps 4 through 6 to import and place the last three links.

Adding Relationships/Mates Between Parts

Now this is a long one so buckle in. For refrence throughout this step, SolidWorks calls relationships between parts, "Mates".

1. With all of the links oriented the same, use the "Normal Too" tool to align your view with the side of the links.

   

   From now on, I will refer to this as the front side. Which side you chose doesn't actually matter but we need to differentiate the two sides.
2. In order to add relationships between our parts we will use the "Mate" tool located directly right of the "Insert Components" tool.

   
   

   Theoretically, the holes we made in our links would be bolt holes to hold our linkage together, for this reason our mates will be centered around the holes.
3. Without anything selected, click the "Mate" tool.
4. On link one, click on the rim of the right circle on the front side,

   
   

   then click on the rim of the right circle on the back side of link two.

   
   

5. Click enter or the green check mark and click the red check mark on the left panel to exit the "Mate" tool.
6. You can now freely rotate link 2 about the right bolt hole on the first link.

   

7. Select the "Mate" tool again, click the rim of the free bolt hole on the front side then click the rim of the right hole on the back side of the link 3. Click the green checkmark.
   

   

8. The "Mate" tool should still be active, click the rim of the left hole on the back side of link 3 then click the rim of the right hole on the back side of link 4. Click the green checkmark.

   

9. Click the rim on the left side of the back side of link 4 then click the rim on the left side on the front side of link 1. Click the green checkmark.

   

   Now all of the links will behave as if they were bolted together through the holes we have aligned.
10. Click File --> Save As, name your assembly whatever your heart desires.

    

Thank you for walking through my guided SolidWorks tutorial! For more information or clarification you can visit the SolidWorks Tips and Tutorials website here or go to Youtube!