Chapter 5

importance of drawing

The generation of drawings is a vital component of the design process in SolidWorks, as it serves as a central element in efficiently conveying the design purpose and fabrication specifications to many stakeholders, including manufacturers, customers, and project team members.

Detailed 2D Representation: SolidWorks drawings provide detailed, fully dimensioned 2D representations of 3D models, which are essential for communicating design intent and fabrication requirements to various stakeholders, such as manufacturers, customers, and project team members.

Bill of Materials (BOM) Generation: SolidWorks drawings enable the automatic generation of bill of materials (BOM), which are critical for inventory management, procurement, and cost estimation, streamlining the process of tracking and ordering the necessary components.

Collaboration and Communication: SolidWorks drawings facilitate collaboration and communication among the design team, stakeholders, and manufacturing partners by providing a standardized format for design documentation, ensuring a common understanding of the design specifications and requirements.

Manufacturing Instructions: SolidWorks drawings can be used to generate detailed manufacturing instructions, such as cutting lists, bend tables, and assembly sequences, helping to ensure that the final product is fabricated and assembled correctly, reducing the likelihood of costly errors or rework.

Design Iteration and Verification: SolidWorks drawings play a crucial role in the design iteration and verification process by allowing designers to create multiple drawing views, including section views, detail views, and isometric views, to better visualize and analyse their designs, identify potential issues, and make necessary modifications before the final product is produced.

setting sheets standard

Once the part is created, it’s time to manufacture it. For Manufacturing we need the dimensions, annotations and other details in our drawing. We can add all these details in the drafting environment. Now let’s follow along these steps:

Step 1: Open the part file in SolidWorks
Step 2: Go to the “New” drop down menu and select “Make Drawing from Part/Assembly”
Step 3: This will take you to the sheet format size, select the one based on your requirements. You can also use your own custom sheet format and size. In this case, the chosen format is (ANSI) Landscape.
Step 4: By default, SolidWorks will be using the ISO drafting standard. To customize this option, you can click the gear icon and go to document properties. If you change the drafting standard, it will change other properties such as annotation, dimension and every other property in this list
Step 5: Right-click on the sheet and choose properties. In this property window, we can change a few properties such as type of projection and the sheet scale.

Now that all the standard for the sheet is set, we are ready to add views in our sheet.

Adding standard views

Now to start adding the views, follow along these steps:

Step 1: To show all the views of your current part, click on the “View Palette” tab.
Step 2: Select the main view of your part (usually either front or top view) by dragging it into the sheet. Be careful when selecting the main view as all the other view will be linked to it.
Step 3: Now you can add other view by hovering your cursor on the sheet and click to confirm it.

standard 3 view

In SolidWorks, the standard 3-view refers to the three orthographic views that are commonly used to represent a 3D model in a 2D drawing. These three views are front view, top view and right-side view. To make a simple three standard view, follow along these steps:

Step 1: On the Drawing CommandManager, click on “standard 3 view”.
Step 2: It will automatically show the open document, you can also browse for other documents. Click “OK”.
Step 3: To change the properties of the drawing, click on the primary view.
Step 4: As we can see the scale is a bit too small, we can change that by changing into “Use sheet scale”. You can also change the configuration, orientation and display style on the drawing properties.

auxiliary views

In SolidWorks, an auxiliary view is a supplementary view of a 3D model that is created to provide additional information or a different perspective that is not adequately represented in the standard orthographic views (front, top, and right-side views). Follow along these steps to create an auxiliary view:

Step 1: On the Drawing CommandManager, click on “Auxiliary View”.
Step 2: Select the edge that you want the auxiliary view to be on.
Step 3: Place the auxiliary view on the sheet. You can edit and change the auxiliary view property on the PropertiesManager

Detail view

In SolidWorks, a Detail View is a type of auxiliary view that provides a magnified or zoomed-in representation of a specific area or feature of the 3D model within a drawing. Follow along these steps to create a Detail view:

Step 1: On the Drawing CommandManager, click on “Detail View”.
Step 2: Draw the circle with the preferred size and place it where you want the detail view to be.
Step 3: Place the detail view on the sheet. You can edit and change the detail view property on the PropertiesManager.

section view

In SolidWorks, a Section View is a type of auxiliary view that shows a cross-sectional representation of a 3D model, revealing its internal structure and hidden features. Follow along these steps to create a Section view:

Step 1: On the Drawing CommandManager, click on “Section View”
Step 2: Select the preferred cutting line.
Step 3: Place the cutting line on the part that needed the section view.
Step 4: Place the section view on the sheet. You can edit and change the section view property on the PropertiesManager.

adding annotation

Dimension and annotation

Dimensions and annotations are integral components of engineering drawings that collaborate to convey the design intention and furnish crucial information to diverse stakeholders engaged in the manufacturing and assembly procedures.

Dimensions are numerical values that precisely define the magnitude, position, and other measurable characteristics of a component or assembly. These include linear dimensions for length, width, or height, radial dimensions for radius or diameter, angular dimensions for intersecting surfaces, and coordinate dimensions for determining the location of a feature. The dimensions play a crucial role in guaranteeing the precise production and assembly of the product by supplying the essential size and positioning details.

Annotations, however, refer to written or graphical features that are included in a drawing to offer supplementary information, directions, or clarifications. This encompasses annotations for material specifications or instructions for manufacture, indicators and labels to highlight characteristics, standardized symbols for welding, surface finishes, or geometric dimensioning and tolerancing, and tolerances that define the permissible range of variation.

Dimensions and annotations are essential components in the creation of engineering drawings that effectively convey the 3D design and aid in the successful realization of a physical product.

Adding Dimensions with DimXpert

In SolidWorks, you can use the DimXpert feature to automatically add dimensions to your drawing views. The DimXpert feature in SolidWorks simplifies the dimensioning process and helps ensure consistency and compliance with industry standards. By using DimXpert, you can quickly add the necessary dimensions to your engineering drawings, freeing up time for other design and documentation tasks.

Step 1: Create a new drawing document or open an existing one.
Step 2: Go to the "Annotation" tab, click on “Smart Dimension” and click on the "DimXpert" dropdown.
Step 3: Click on the entities that you want to give the dimension and choose the part of the circle. This will represent the place where the dimension will be located.
Step 4: Now repeat the steps until all the dimensions of your part have been placed. You can customize the dimensions on the PropertiesManager.
Step 5: Carefully review the drawing to ensure that all the dimensions are accurately placed as the design intent.
Step 4: Now repeat the steps until all the dimensions of your part have been placed. You can customize the dimensions on the PropertiesManager.
Step 5: Carefully review the drawing to ensure that all the dimensions are accurately placed as the design intent.

Adding Dimensions with Autodimension

In SolidWorks, you can use the “Autodimension” feature to automatically add dimensions to your drawing views. The “Autodimension” feature in SolidWorks provides a quick and efficient way to add dimensions to your engineering drawings. By using this tool, you can save time and ensure consistency in your dimensioning practices. However, keep in mind that you may need to further customize the dimensions and annotations to meet specific requirements or design intent.

Step 1: Create a new drawing document or open an existing one.
Step 2: Go to the "Annotation" tab, click on “Smart Dimension” and click on the "Autodimension" dropdown
Step 3: Select the view that you want to add the dimension and click “OK”.
Step 4: Let’s fix the dimension to make it more presentable. Select all the dimensions on the right and click the pop up
Step 5: Click on the “Auto Arrange Dimension” and “Space Evenly Linear/Radial” features.
Step 6: Repeat for all the dimensions on the bottom of the view.
Step 7: Repeat for all other view in the drawing.
Step 8: Carefully review the drawing to ensure that all the dimensions are accurately placed as the design intent.

Basic of note

Let’s start adding text in the drawing. To add text, we can use the “Note” feature from the annotation tab. When you click the “Note” feature, it will show you several panels but for now let’s focus on the Leader panel. By default, it will select “Auto Leader”.

To use this feature, follow along these steps:
Step 1: Click on the feature in your drawing. Now the leader line will be connected to the feature.
Step 2: Click again to place the end of the leader line. Now a text option will appear.
Step 3: Add your note and adjust it as you want and click “OK”. You will end up something like this. Now, try to use different type of leader in your drawing.

assembly drawing

alternate position view

In an assembly drawing, an alternate position view is a drawing view that shows a component or part in a different position or orientation compared to its primary position within the assembly.
The purpose of an alternate position view is to provide additional visual information about a specific component or subassembly that cannot be clearly conveyed from the standard orthographic views (front, top, right side) of the overall assembly. To use the

alternate position view simply follow along these steps:
Step 1: Open the assembly part that contains more than one configuration.
Step 2: Make a drawing from the assembly.
Step 3: Insert the assembly into the drawing sheet and change the display style to shaded.
Step 4: Now let’s go to Drawing > Alternate Position View.
Step 5: On the PropertyManager, choose the “Existing configuration” and select the configuration that you want to be displayed.

The assembly should display the alternate configuration on the drawing.

Exploded View and Bill of Materials

By including both the exploded view and the bill of materials in the engineering drawings, you provide a comprehensive set of information that supports the entire product lifecycle, from manufacturing and assembly to maintenance and service. This level of detail and visual communication is essential for ensuring the successful realization of the product design. To add the exploded view of the assembly in drawing,

follow along these steps:
Step 1: Insert the assembly into the drawing sheet and change the display style to shaded.
Step 2: Make sure the assembly is in default configuration. On the PropertyManager, tick on show in exploded view.

The assembly should display the exploded view on the drawing. Now to add the Bill of Materials for the assembly simply follow all the steps below:
Step 1: Go to Annotation > Tables > Bill of Materials.
Step 2: Select the drawing view and click “OK”.
Step 3: Place the Bill of Materials on the drawing sheet.

adding balloons

Adding balloons to engineering drawings is a common practice to provide clear identification and reference of the individual components within an assembly.

To add the balloons to your drawing simply follow along these steps:
Step 1: Go to Annotation > Balloon.
Step 2: Click once on the part and then click one more time to place the balloons. You can change the property of the balloon on the PropertyManager.
Step 3: Repeat the steps for each part that needed the ballon. Carefully review the drawing to ensure the balloons are properly positioned, the numbering is sequential, and the leader lines are clear and unobstructed.

Drawing and documentation

Basics of drawing