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4.2.2: How to create an engineering drawing

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    Why are engineering drawings important?

    Engineering drawings are essential tools for effective communication between machinists, engineers, and other teams. These detailed illustrations ensure that designs can be accurately interpreted and manufactured. Additionally, they provide a reliable way to document your work, which is critical for troubleshooting failures, implementing revisions, or maintaining records for future use (1).

    Key components of engineering drawings include:

    • Bill of Materials (BOM): This section lists all components required for the assembly of your design, ensuring proper identification and sourcing of parts.

    • Title Block: Found within the drawing template, this block includes essential details such as your name, the part name, and tracking information like dates or revision numbers.

    Many organizations, including NC State, have standardized templates for engineering drawings, ensuring consistency and adherence to specific guidelines. Using these templates ensures your work meets professional and institutional standards.

    References 

    (1) Inodvance. The Importance of Technical Drawings in Engineering. https://blog.indovance.com/importanc...ical-drawings/ (accessed 2024-11-19).

    Step 0 - Save your part and familiarize yourself with your workspace

    To be able to put your part into an engineering drawing, you will need to have it saved.  If you can't insert the views into Solidworks, navigate to the other menu and save it there.  

    DrawingMenuUpdated.JPG
    SketchMenuDrawing.JPG

     

    Step 1 - Create a New Drawing

    1. Hover over the SolidWorks logo in the top-left corner.

    2. Select File, then click New.

    3. From the menu that appears (see Figure 1), choose Drawing.

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    Fig 1.) Menu for selecting the type of document to create, including parts, assemblies, and drawings.

    Step 2 - Select the Template

    1. SolidWorks provides preloaded templates that serve as the foundation for your drawings.

    2. From the menu shown (see Figure 2), choose A2 (ANSI) Landscape—a standard template in SolidWorks.

    3. If you prefer to use a custom template, click Browse and select your desired template from your computer.

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    Fig 2.) Menu for selecting a template to create an engineering drawing in SolidWorks.

    Step 3 - Drag Your Part onto the Template

    1. After selecting your template, begin by placing the primary view of your part onto the drawing.

    2. In SolidWorks, click Model View and choose the part you want to create a drawing for.

    3. Hover over the template. A preview of the space your view will occupy will appear (see Figure 3).

    4. Click on the template to place your view.

    Warning:  You may encounter issues if you have not recently saved AND opened the file.  If you cannot select a part, press browse in the menu to the left, and select your part.

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    Fig 3.)  Preview of the Model View tool in SolidWorks, showing the side view placement before it is added to the drawing.

    Step 4 - Place Your Views

    1. Once the Model View tool is active, begin placing additional views of your part.

    2. Start by placing the principal view (front view) on the drawing.

    3. Add at least two additional views:

      • Place a view above or beside the principal view to display the top or side view, respectively.

      • Place a view diagonally from the principal view to create an isometric view.

    4. Ensure you have the top view, side view, and isometric view positioned as shown in Figure 4.

    Note:There may be some overlap between drawings in this step, they will be repositioned in the next step.

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    Fig 4.)  All four views—principal, top, side, and isometric—are placed on the drawing template.

    Step 5 - Move Your Views

    1. To move the isometric view, hover over it and click on the dashed outline. When your cursor turns into 4 blue arrows, drag the view to a new position.

    2. You can also move the top, side, and front views, but keep in mind that these views are linked—moving one will move the others.

    3. Move the isometric view away from the top view as shown in Figure 5.

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    Fig 5.)  The isometric view after being moved away from the top view.

    Step 6 - Show Your Hidden Lines

    1. Click on any of your views.

    2. In the menu on the left, under Display Style, check the box labeled Visible Hidden Lines (see Figure 6).

    3. This will make the dimensioning process in Step 7 much easier.

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    Fig 6.)  The menu through which parts and views are selected in SolidWorks, with the option to display hidden lines highlighted.

    Step 7 - Dimension Your Views

    1. Dimensioning is a crucial step in creating an engineering drawing. The goal is to provide enough information so that anyone reading the drawing can understand all the views of the part.

    2. If you specify a dimension in one view, there’s no need to repeat it in other views.

    3. You can dimension to hidden lines, center points, radii, and construction lines.

    4. To start dimensioning, navigate to the Sketch menu and select Smart Dimension.

    5. This tool works similarly to how it was used for dimensioning sketches, but keep in mind that in this context, the dimensions cannot be edited.

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    Fig 7.)  A properly dimensioned engineering drawing

    Step 8 - Fill Out Your Title Block

    1. The title block is the most important part of your engineering drawing. It attributes the design to you and provides tracking information, as well as essential part specifications.

    2. To edit the title block in SolidWorks, navigate to the timeline and right-click on the Sheet Format (see Figure 8).

    3. From the menu, select Edit Sheet Format.

    4. In this mode, you can click to add text and edit the sheet format.

    5. Fill in all applicable fields, making sure to include your name and any other required information.

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    Fig 8.)  The menu where you can find the options to edit and fill out the title block in SolidWorks.

    Step 9 - Save Your Document as a PDF

    1. Hover over the SolidWorks logo, then select File and click Save As.

    2. In the File Manager, under Save as Type, select PDF.

    3. Choose your save location and click Save.

    4.2.2: How to create an engineering drawing is shared under a not declared license and was authored, remixed, and/or curated by LibreTexts.

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