In this post, we will dive into the next crucial step in SolidWorks sketching: adding dimensions. Dimensions not only define the size of a sketch but also control its scale and ensure its accuracy. Understanding how to properly apply dimensions is key to creating a robust and modifiable design.
Why Dimensions Matter in SolidWorks
When creating sketches in SolidWorks , the software does not initially assign any fixed sizes to the sketch entities. Instead, it allows users to define dimensions manually, giving full control over the design. Dimensions serve two main purposes:
- Defining Size – Without dimensions, a sketch is just a shape without scale. Adding dimensions ensures that the features have the correct real-world proportions.
- Maintaining Design Intent – Dimensions allow you to modify and refine the sketch without breaking its structure. By defining relations and dimensions together, you ensure the model behaves predictably when changes are made.
The key tool for adding dimensions is the Smart Dimension Tool, which can be found in the Sketch menu. This tool allows you to quickly define the size and positioning of sketch entities.
Scaling the Sketch with the First Dimension
One of the most important concepts to understand when adding dimensions in SolidWorks is that the first dimension you apply scales the entire sketch. Imagine that the sketch’s proportions are locked in place, and the first dimension acts as a reference, adjusting everything else in relation to it.
For example, if you create a simple rectangle without specifying dimensions, it exists only as a shape. The moment you apply a dimension to one of its lines, all other entities scale accordingly. This ensures that the sketch retains its original shape while acquiring a specific size.
Applying Different Types of Dimensions
The Smart Dimension Tool is versatile, allowing you to add multiple types of dimensions depending on your needs. Here’s how you can apply various dimensioning techniques:
Linear Dimensions
To dimension a straight line, select the line, then click to place the dimension. The dimension value can then be manually entered in the Modify Dimension box.
As a useful feature, the Modify Dimension box acts as a built-in calculator. You can perform operations such as addition, multiplication, and even unit conversions directly within the input field. For example, if you’re working in millimetres but need to enter a value in inches, you can type the value in inches, select the unit from the dropdown, and SolidWorks will automatically convert it to millimetres.
Angular Dimensions
When defining angles between two lines, select both lines, and SolidWorks will display a preview of the angle measurement. Be mindful of where you position the cursor when applying an angular dimension, as the value may shift depending on placement. Ensure the correct angle is displayed before making your final selection.
Between Two Entities
You can also apply dimensions between two separate entities, such as two lines or points. Initially, the dimension will appear to represent only the first selection, but after clicking the second entity, SolidWorks updates the dimension to reflect the distance between the two.
Aligned, Horizontal, and Vertical Dimensions
When dimensioning a line at an angle, there are three possible placements: aligned, horizontal, or vertical. The dimension type you choose significantly impacts how the sketch behaves when modified. At shallow angles, the difference between aligned and horizontal or vertical dimensions may not be immediately apparent. To lock the correct alignment in place, use a right-click before moving the cursor elsewhere.
Diameter and Radius Dimensions
So far, we have focused on straight-line dimensions, but SolidWorks also allows dimensioning of circles and arcs. To demonstrate this, let’s add a circle to the sketch using the Center Circle Tool. The first click places the centre, while the second defines the size.
By default, when you add a dimension to a circle, SolidWorks assumes you are specifying the diameter. If you are working with an arc instead, the radius is the default. However, you can easily toggle between diameter and radius by right-clicking on the dimension and selecting the desired option.
Another useful technique for dimensioning circles is controlling their position relative to the rest of the sketch. By default, dimensions reference the centre point of a circle, but you can also measure to the minimum or maximum arc point by holding Shift while selecting the circle. This technique is particularly useful for maintaining specific clearances or ensuring precise hole placement in a part.
Finalizing and Editing Dimensions
Once dimensions are applied, they can always be modified. Simply double-click a dimension to bring up the Modify Dimension box, where you can enter a new value. Because SolidWorks sketches are parametric, changing one dimension updates the entire sketch while maintaining its design intent.
A great way to check if all dimensions are correctly applied is to try dragging different sketch entities. If the sketch moves in unintended ways, there may be missing dimensions or incorrect constraints. Adjusting dimensions ensures the sketch is fully defined and behaves as expected when modifications are made.
Bringing It All Together
With the Smart Dimension Tool, you can precisely define the size and positioning of your sketches, ensuring they are accurate and modifiable. In this post, we explored how dimensions scale a sketch, how to add linear and angular dimensions, and how to dimension circles and arcs effectively.
By mastering dimensions, you gain full control over your sketches, making it easier to create complex parts that adapt well to design changes.
In the next post, we will take things further by looking at fully defining a sketch and understanding constraints, ensuring that your designs are stable, predictable, and ready for 3D modelling. Stay tuned!
