How to Create Technical Drawings in Onshape: BOMs, Exploded Views & More

Rıdvan Polat

5 February 2026 12 mins to read

In this training series, we will use the Air Engine assembly created on the tablet in the previous episode. You will learn how to create a Bill of Material table, Explode the assembly, generate Drawings, add Callouts, create regional sections using Broken-out section view tools, insert Sheet metal Flat patterns, and finally Export the drawing as a PDF.

To begin, we will transition from using Onshape on the mobile app to the web browser to access more advanced features. Since I’ve covered every detail in the videos, I’ve focused only on the key points in the text descriptions.

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

If you haven’t yet tried Onshape, PTC’s cloud-native CAD and PDM platform, 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.

BOM & Generate Part Number

The Bill of Material (BOM) is essential for manufacturing. The Part Number is an integral part of the BOM table. It acts as the part’s identity, which is crucial for manufacturing, purchasing, and inventory tracking.

BOM Strategy & Naming Logic

Pro Tip: In many CAD programs, you must create a drawing to view the BOM table. In Onshape, however, you can customize the BOM table directly within the assembly environment.

Pro Tip: We mentioned the Part Studio naming logic in the previous blog post. When we add the Name column to the BOM table, the names of the bodies inside are displayed, not the Part Studio name. Therefore, we need to rename the bodies.

Generating Part Numbers

Pro Tip: Entering Part Numbers manually is often undesirable and time-consuming. In Onshape, you can generate unique part numbers with custom prefixes using the Sequential Part Number Generation feature via Company settings.

Pro Tip: There are two ways to generate a Part Number. First, by right-clicking a cell under the Part Number column in the BOM table and selecting Generate next part number. Second, by returning to the Part Studio, right-clicking the Part Studio tab, and generating it from the Properties window.

Exporting BOM Data

Pro Tip: You can export the BOM table in CSV format. When opened, all data may appear in a single column, separated by commas. In Microsoft Excel, go to the Data tab, select Text to Columns, and choose Comma as the delimiter to split the data into separate columns.

Explode

Explode holds a significant place among the sought-after features in many CAD programs, in my opinion. In the various CAD trainings I have delivered, I have observed that users prioritize this command to demonstrate assembly steps.

Pro Tip: If you want to see the assembly alignment lines of connected parts, you should use the Explode lines option. We selected all parts except the Plate and moved them, creating a distance between the Bracket and the Base Plate. We can use the Explode lines option when we want to show that the Bracket holes align with the holes on the Base Plate.

There are two points to consider with this option:

When you check the option, it automatically generates an axis line. This axis line might not always be correct. In such cases, you should select the face/edge/point you want the center to pass through.
When making a selection, you need to select the holes/slots of the moving part. If you select the holes of the Base Plate instead of the Bracket, you will not be able to see the lines.

Drawing

Although we model everything in 3D, a 2D drawing containing dimensions, a BOM table, and an Exploded view is indispensable for manufacturing. In the industry, this is known as a Technical Drawing.

BOM, Exploded and Callout

Understanding Sheet vs. Component Scales

Pro Tip: There are important points to consider when using Sheet Scale and Part Scale. If you set the sheet scale and insert a part/assembly, the components are scaled according to the sheet. When you double-click on a component, you will see “(Sheet)” in parentheses next to the scale value in the View Properties window. This indicates that the component is using the sheet scale. You need to be careful if you change the scale value from this screen, since it affects only that part, not the sheet. If you need such a change, checking the Scale Label checkbox would be helpful for the person reviewing the drawing to avoid the perception of a size difference between parts.

Pro Tip: Scale is used to fit the part onto the sheet. The most confusing part for new CAD users is thinking that the part’s dimensions change according to the scale. Multiplying/dividing the part’s dimensions based on the scale is the wrong method. Meaning, no matter what the scale is, the dimensions of the part do not change.

Projection Angle Standards

Pro Tip: The Projection Angle varies according to the selected technical drawing standard. For example, in the ISO standard, this angle is First angle. In the ANSI standard, it is Third angle. We can explain these two terms as follows:

1. First Angle Projection: Imagine you have a flashlight and you are shining light on the part from the right. The shadow of the part, i.e., its projection, falls on the wall behind it, meaning to the left. We draw the detail we see from the right on the left side of the paper.

We draw what we see from the top at the bottom. In other words, the view falls opposite to the direction of view. The technical drawing symbol is as follows.

2. Third Angle Projection: Imagine there is a transparent glass between you and the part. When you look at the part from the right, you draw the image on the glass right in front of you, meaning to the right.

The view seen from the right is drawn on the right, and the view seen from the top is drawn on the top. You draw what you see where it is. The technical drawing symbol is as follows.

Exploded Views & Callouts

Pro Tip: By double-clicking the Air Engine we added to the technical drawing, we can bring the Explode 2 created in the assembly environment to the drawing environment via the opened View Properties window.

Pro Tip: You can establish a link between the BOM table and the component thanks to the Callout command, or the “ballooning” command as it is known in other CAD programs. From the Callout command window, you can specify the shape of the balloon and which values should be written inside, to the right and to the left of the balloon. We leave the Item number selected in the center and select the Part Number option for the area on the right side. Simply selecting the desired parts is enough to add the Callout.

Drawing Properties

Pro Tip: Changing the size of an Annotation arrow or a dimension arrow and the size of the dimension text significantly affects readability and prevents errors. You can change all these settings via the Drawing Properties located on the right side.

Property Linking

Pro Tip: Inside the drawing title block, there are many titles added specifically for the template and special properties linked to the document. For example, when we double-click on the dashed lines in the box labeled Title, a Note window welcomes us to add text. Via this window, we can make manual entries as well as add drawing property (information specific to the drawing document) or reference property (information specific to the associated model) values. We confirm the command by selecting the Insert Sheet Reference Property option and adding the Name property. This brings the name of the Assembly.

Broken-out section, Flat Pattern and PDF Export

Show/Hide Options

Pro Tip: You might want a part to appear colored instead of black-and-white, or you might want to change the visibility of thread lines or hidden lines on the part. You can make these adjustments via the Show/hide menu opened by right-clicking on the part.

Keyboard Shortcuts

Pro Tip: Some users prefer working using keyboard shortcut keys to speed up their work. When you hover your mouse cursor over the commands, you can see the shortcut key for the command. For example, the shortcut for the Dimension command is the D key.

Chamfer & Hole/Thread Callouts

Pro Tip: To be able to use the Chamfer command located within the Dimension commands, you can see the dimension of the chamfered edge after selecting a chamfered edge and another edge connected to that edge.

Pro Tip: When there are many holes of the same diameter on the model, you can show that they are all the same diameter and how many there are with the Hole/thread callout command. When we select the command and select a hole on the Bracket, an Annotation like “4X Ø4 THRU” appears. Here, while determining the number of holes, it counts by looking at the pattern command. Since we used two separate pattern commands to replicate the holes on the Bracket part, this option will not be correct for us. When we expand the menu by clicking the arrow next to “4X” then double-clicking on the text to choose to count based on the part instead of the Pattern, you can see that the number of holes is updated to 6.

Dimension Alignment & Arrowhead Style

Pro Tip: One of the most important things in a technical drawing is readability. It is important that dimension arrows and callouts are aligned with each other. You can get help from the dotted pink line that helps you align the horizontal arrows with horizontals and vertical arrows with verticals when you move the dimension arrows.

Pro Tip: In cases where the values on the dimension arrows cannot be read well, it may be desired for the arrowheads to be inward/outward to increase readability. In such cases, you can change the direction of the arrow by hovering over the dimension arrow and clicking on the dots on the dimension arrow.

Section Views & Hatching

Pro Tip: It might be necessary to show the detail of a hidden channel or hole located within a specific region on a part. Section view commands are used for this. There are M4 bolt holes on the Base Plate part. We want to show the detail of one of these holes in the side view. For this, Broken-out section view command for this. We create a closed area with a spline in the side view. This area corresponds to the location where the hole is found. Afterward, we confirm the command by selecting the center of the hole in the top view to specify the section depth. This gives us the opportunity to show how the hole looks inside the side view and the dimensions of the hole.

Pro Tip: The shape of the sectioned regions varies according to standards and the material of the part. To change this, you can change the hatch properties by right-clicking on the Part.

Tables & Property Linking

Pro Tip: There may be cases where you need to provide additional information by adding a note or table to the technical drawing. We want a table containing the Part Name and Part Number on every page for the parts. Therefore, we create a table with 2×2 rows and columns. We write Name and Part Number in the first row of the table. We link the Name and Part Number properties to the table using the reference property option shown earlier. The table pulls the data of the component on the Sheet where the table is located.

Sheet Metal Flat Patterns

Pro Tip: The indispensable part of sheet metal design for manufacturing is showing the flat pattern of the sheet in the technical drawing. Thanks to this flat pattern, it is made possible to know at what dimensions the sheet will be cut from before bending. Also, getting the DXF output of a flattened sheet metal part has great importance in manufacturing. When you bring the flat pattern of a sheet metal to the technical drawing in Onshape, the necessary angles and directions for bending are specified on the sheet.

Export as PDF

Pro Tip: To give a meaningful name to the technical drawing document, we right-click on the Drawing 1 tab and name it Air Engine. After creating all technical drawings for other parts, we export our document by right-clicking on the Air Engine tab and selecting the PDF file format via the Export menu.

With this tutorial, you have gained detailed information about Exploded parts, BOM tables, and creating technical drawings. In the next part, we will apply a force on the Piston and test its effect on the Connecting Rod with Onshape Simulation.

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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.