Modeling a Connecting Rod in SolidWorks: A Comprehensive Guide

Welcome back to the Multibody Dynamics using SolidWorks blog series! In this blog series, we will walk through the detailed process of creating the geometry for a connecting rod—an essential component in a slider-crank mechanism. This part is crucial for converting translational motion into rotational motion, a mechanism commonly used in internal combustion engines, radial engines, and reciprocating compressors. The connecting rod is responsible for linking the piston to the crankshaft, making it a vital part in many mechanical systems. 

Let’s dive into the steps involved in creating this key component using SolidWorks. 

Step 1: Starting a New Part in SolidWorks 

Begin by opening a new part in SolidWorks. Navigate to File > New > Part, and ensure that your unit system is set to millimeters (mm). SolidWorks offers flexibility with units, and using millimeters for this project will help maintain accuracy and compatibility. Once the units are set, select the front plane to begin sketching the outline of the connecting rod. 

Step 2: Creating Concentric Circles 

For the connecting rod, the next step involves drawing two sets of concentric circles, representing the piston and crankshaft connection points. Use the circle tool to sketch the following: 

Piston connection: 

• Inner circle diameter: 25.4 mm 
• Outer circle offset: 10 mm 

Crankshaft connection: 

• Inner circle diameter: 43.75 mm 
• Outer circle offset: 20 mm 

The centers of these two sets of circles should be spaced 212.5 mm apart to ensure proper alignment and functionality in the final design. 

Step 3: Aligning and Constraining the Circles 

Once the circles are created, ensure that they are aligned horizontally. Select the center points of both sets of circles and apply the make horizontal constraint. This aligns them perfectly on the same horizontal axis and fully defines the position of the circles. 

After the circles are aligned, begin adding connecting lines between them to form the basic shape of the rod. Start by drawing two lines—one for the left side and one for the right side. Apply the following dimensions: 

Left-side line: 

• Distance from the circle’s center to the start of the line: 14.1 mm 

Right-side line: 

• Distance from the center to the start of the line: 21.4 mm 

To maintain symmetry, use the mirror entities tool to mirror the left line across the top plane. This method ensures that both sides of the rod are identical, which is critical for balance and performance in real-world applications. 

Step 4: Adding Fillets for a Smoother Design 

With the general shape of the connecting rod in place, the next step is to refine the design by adding fillets. Fillets help smooth out sharp edges, making the part more streamlined and reducing stress concentrations. Select the four corners of the connecting lines and apply a fillet radius of 20 mm. This not only improves the aesthetic appeal of the rod but also enhances its structural integrity. 

Step 5: Extruding the Sketch to 3D 

After finalizing the sketch, it’s time to extrude it into a 3D model. Select the mid-plane option when extruding, which ensures symmetry on both sides of the rod. Set the extrusion distance to 30 mm. This creates the top half of the connecting rod, providing the necessary thickness for strength and durability. 

Step 6: Creating Grooves for the Piston Cap 

The next task is to add grooves to the connecting rod to accommodate the piston cap. Select the front face of the rod and start a new sketch. Use the circle tool to draw a circle with a diameter of 20 mm. This circle will serve as the location for the grooves that will later hold the bolts connecting the piston cap. 

Apply the make vertical constraint to align the circle correctly, then use the mirror entities tool to mirror the circle onto the opposite side of the rod. Once the circles are mirrored, apply an extruded cut with a depth of 30 mm to create the necessary grooves. 

Step 7: Creating Bolt Holes 

Next, you’ll need to create holes for the bolts that will secure the piston cap. To do this, sketch another circle on the same face where the grooves were created. The diameter of the circle should be 11.25 mm. After drawing the circle, mirror it using the mirror entities tool as you did for the grooves. Once mirrored, apply an extruded cut with a depth of 30 mm to complete the bolt holes. 

Step 8: Finalizing the Connecting Rod 

With the bolt holes and grooves completed, the main body of the connecting rod is now finished. At this point, you can hide any unnecessary sketches by selecting them and clicking hide to clean up the workspace. This makes the model easier to work with as you move on to the next steps in the process. 

Conclusion: What’s Next? 

In this video, we’ve successfully modeled the primary structure of the connecting rod in SolidWorks, an essential component for multibody dynamics simulation. This detailed modeling process gives you a solid foundation for creating other mechanical components in SolidWorks and integrating them into larger assemblies. In the next part of this series, we will focus on creating the end cap geometry, finalizing the connecting rod, and preparing it for multibody dynamics analysis. 

Stay tuned for the next blog in the SolidWorks tutorial series, where we will explore more advanced modeling techniques and set up simulations to test the dynamic behavior of the rod in different scenarios. 

This blog is part of our ongoing series on Multibody Dynamics. 

If you missed the previous posts, check them out here.   

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