How to Assembly an Air Engine in Onshape?

Rıdvan Polat

2 February 2026 9 mins to read

In this training series, we will use a tablet to assemble the 12 parts we previously designed also on a tablet. Since I covered all the details in the videos, I only touched upon the important points in the descriptions.

In the next blog post, you will also learn how to create a Bill of Material table, Explode the assembly, create a Drawing, add callouts, create regional section views with broken-out sections, add sheet metal flat patterns, and finally export the drawing as a PDF.

Before starting the assembly steps, make sure you have access to Onshape so you can follow the workflow directly on your own device.

If you haven’t tried Onshape, PTC’s cloud-native CAD and PDM platform, yet, you can click on the link below to create a free Onshape account or try Onshape Professional—which includes tools such as Simulation and Render Studio—free for 6 months.

6 Months Free Access to Onshape Professional

If you are ready, let’s begin.

Things to Know About Assemblies

Understanding Part Studio vs Part

The first step of the assembly is adding the parts you have designed. If you are using the Insert command in Onshape for the first time, it is helpful to understand the part naming logic in the menu. This can be confusing at first, especially if you have experience with other CAD programs.

In Onshape, a Part Studio represents the workspace where parts are created; it is not a part itself, but a design environment. Each solid body created within it is defined as a Part.

Therefore:

A Part Studio name is the name of the design environment.
A Part name is the name of the actual manufacturable part added to the assembly.

Even if you have designed only a single part in a Part Studio, you will see the following structure when adding parts:

Part Studio name (e.g., Base Plate)
Part name (default: Part 1)

So, What is the Benefit of this System?

If you are creating multi-part designs (often called multi-body in other traditional CAD systems), it allows you to insert each part into the assembly environment separately.
Since each part acts as a separate entity, it can be displayed as a distinct item in the BOM table.

What Should You Watch Out For?

Onshape offers two different options when inserting a part or parts designed in a Part Studio into the assembly:

You can select each part in the Part Studio individually and add it to the assembly.
If you want all parts in the Part Studio to behave as a single component, you can use the Insert entire Part Studio as rigid command.

When you select the Insert entire Part Studio as rigid command, the part or parts designed in the Part Studio environment appear passive (grayed out), and the Part Studio (Base Plate in our example) is added to the Instance list. When you select the arrow next to the Base Plate in the Instance list, you can see the bodies from the Part Studio.

We used this command while creating this assembly, since all of our designs consist of a single component and to see the Part Studio naming in the assembly environment.

Pro Tip: If you are creating multi-part designs and each part requires a separate mate in the assembly, it makes more sense to select each part individually.

Assembly Methodology

Onshape’s assembly methodology differs from traditional methods. In traditional systems, inserting a cylindrical pin into a hole requires at least two constraints: First, making the cylindrical surfaces concentric, and, second, making the flat surfaces coincident. While this positions the pin within the hole, it can still rotate. Preventing this rotation requires a third constraint. This method is called Low-Level Constraints.

In Onshape, it is different. With the Mate Connector feature, this multi-step process is completed in a single step.

How to Use Mate Connectors?

When a Mate command is active in the assembly environment, hovering your cursor over a part reveals multiple points (Mate Connectors) on that face. Each of these points is effectively a local coordinate system. Once you select the appropriate connector on both parts, the system positions and aligns them simultaneously according to the chosen Mate. This approach is called High-Level Constraints. In short, you perform a multi-step operation in one go, significantly reducing assembly time.

Pro Tip: Since there is no cursor in the mobile app on the tablet, you must first tap the part’s face and then select the connector.

Step-by-Step Air Engine Assembly

Now that you have the necessary information, we can proceed to the Air Engine assembly step-by-step. Since the videos show the necessary steps, I focused on important tips related to those steps rather than explaining each one.

Assembly Strategy & Logic

Pro Tip: Mate commands constrain the degrees of freedom of parts relative to each other or to space. This allows us to simulate the movement of a real-world mechanism’s components in the CAD environment.

Pro Tip: The mobility of a rigid body free in space is defined by 6 Degrees of Freedom (6 DOF). These movements are grouped into two main categories:

Translation: Linear movements along the X, Y, and Z axes (3 DOF).
Rotation: Angular movements around the X, Y, and Z axes (3 DOF).

Pro Tip: You should proceed by assembling parts just as you would connect them in real life. The most preferred option is to first insert the main component that will hold all other parts, fix it using the Fix command, and build upon it.

Fastened Mate

Pro Tip: We use the Fastened Mate constraint for parts that should remain static relative to each other. We use the Fastened Mate constraint between the Bracket part, which sits on the Base Plate aligned via bolt holes, and the Motor Block parts, which sit on the Bracket aligned via bolt holes. The assembly uses the Fastened Mate constraint between the Crank, Crankshaft, and Crank Pin parts.

Revolute Mate

Pro Tip: The Crankshaft and its attached parts must rotate around their own axis within the cylindrical housing inside the Motor Block part. To ensure this constraint, we use the Revolute Mate command. The two connector points required for the Revolute Mate are the center point of the surface inside the Motor Block‘s cylindrical housing that will contact the Crank, and the center point of the protruding cylindrical surface of the Crank part that will contact the motor block. With this constraint, the Crankshaft can rotate around its own axis but cannot perform any translation movement (1 DOF).

Visibility & Isolation

Pro Tip: Overlapping parts might obstruct your view. In such cases, make only the parts you are assembling visible, and hide the others, will help your view.

Pro Tip: You might want to see the details inside a part in the assembly environment. In such cases, you can adjust the transparency of the part via the Appearance option by going to the Part Studio environment of the relevant part, selecting it, and then tapping the three dots on the mobile app or right-clicking with a mouse on PC. We change the transparency of the Motor Block to see the Piston‘s movement inside it.

Pro Tip: A part you add to the assembly might remain under other parts. When you have many parts, hiding/showing each one via the instance list can be time-consuming. To see only the Piston after adding it to the assembly environment, we select the Piston and choose the Hide other instances option via the three dots/right-click. This option hides other components collectively. After moving the Piston to a visible location, you can view all hidden components by selecting a hidden component and using the Show all instances option via the three dots/right-click.

Slider Mate

Pro Tip: The movement of the Piston inside the cylinder located in the Motor Block is linear and should only be up-and-down. To ensure this constraint, we use the Slider Mate command. The Slider Mate command prevents the Piston from rotating around its own axis. It allows it to perform translation movement in only one direction (1 DOF).

Custom Mate Connectors

Pro Tip: In some parts, the suggested Mate Connectors might not be in the desired locations. The Piston Pin must sit centrally in the cylindrical slot within the Piston, equidistant from the left and right. To achieve this, we will use the Mate Connector command found in the Part’s environment. We can either return to the Piston‘s Part Studio or, while in the Assembly, select the Piston and use the Edit in Context option to view part environment options. While in the part environment, we Show the sketch forming the cylindrical slot and select the circular sketch using the Mate Connector command. This places a Mate Connector at the center of the circle.

Crucial Detail: If you confirm the command like this, the Mate Connector will not be visible in the assembly environment. To change this, while inside the Mate Connector command, select Owner Entity, remove the Part of Sketch option, select the part itself instead, and then confirm. Now, in the assembly environment, we can complete the Revolute Mate constraint by selecting the center connector of the Piston Pin and the Mate Connector located on the Piston.

Cylindrical Mate

Pro Tip: The Rod part must be able to move left and right while rotating around its own axis when seated on the Piston Pin. The constraint command that provides this movement is the Cylindrical Mate. This command is basically a combination of the Slider and Revolute commands (2 DOF).

Reorienting Parts

Pro Tip: When mating two parts, the part might not be in the exact position you want due to its initial orientation. In such cases, you can rotate the part in 90-degree increments to bring it to the appropriate position using the Reorient secondary axis option within the open Mate dialog window.

Don’t forget to subscribe to our blog to stay informed about our next blog, which will delve into the details of technical drawings.

Author
Recent Posts

Rıdvan Polat

Co-Founder at ChampionXperience

Ridvan Polat is a SOLIDWORKS Elite Application Engineer, Founder of ChampionXperience, and a recognized SOLIDWORKS, ENOVIA, and 3DEXPERIENCE Champion. He specializes in CATIA & ENOVIA technical support and 3DEXPERIENCE early engagement adaptation, helping organizations optimize PLM workflows.