The modify dimension box in SolidWorks, which appears when adding or editing a dimension, offers several useful features to expedite the design process.
By default, dimensions are added using the system's default unit, typically millimeters.
However, you can quickly input a dimension in a different unit, such as inches, by typing the value and selecting the desired unit from the drop-down menu. The value will then be converted back to the default units.
Additionally, you can type unit symbols directly. For instance, you can use 'mm' for millimeters and either the inch symbol (") or 'in' for inches. This flexibility can significantly streamline your workflow.
Lock Projection
Linear dimensions in SolidWorks can be added in several ways, such as by selecting a single line, a line and an endpoint, or two endpoints.
When you select a single line or two endpoints, you can place the dimension projection horizontally, vertically, or parallel to the selection. It's crucial to get this right because an incorrect dimension can lead to inaccurate lengths, especially at angles like 45 degrees, and even more so at smaller angles.
To assist with this, you can lock the dimension projection before placing the dimension. This is done by right-clicking and selecting the padlock icon. Once locked, you can position the dimension anywhere on the screen.
Dimension to min max of arc or circle
When dimensioning between two circles or arcs, the default dimension that is added goes to the center of each selection.
To add the dimension so that it’s anchored to either the minimum or maximum or the arc or circle, hold down shift before selecting, and click to the side in which the dimension should be anchored from
Shift should be held down for each selection, unless the center point is required.
Once placed, should the anchoring of the dimensions need to be modified, this can be controlled from the leaders tab within the dimension properties.
Dimensioning the arc length
Adding dimensions to an arc to capture its radius value is really straightforward, but how about dimensioning the length of an arc.
Well, to add the length of an arc, both endpoints and the arc itself need to be selected.
The resultant dimension will then follow the curvature of the arc, as well as showing the arc symbol above the dimension.
Angular Dimensions Using an Imaginary Line
Angle dimensions can easily be added by selecting two non-parallel lines. But angles can also be added between a line and an imaginary horizontal or vertical line too.
When in the smart dimension tool, select the line or edge that the angle dimension needs to reference, and then select an endpoint.
A crosshair appears and a segment can be selected to define where the angle is defined from.
Radial and Diametric Dimensions
When creating sketch geometry for revolved parts, you can add dimensions as either radius or diameter values.
By selecting the sketch geometry and then a centerline, the dimension can be placed as a radius, or if the dimension is toggled across the centerline, it switches to a diameter.
Initially, no symbols for radius or diameter are shown.
To include them, select the dimension and click the diameter button in the dimension properties.
If you need to change a diameter to a radius or vice versa after the dimension is added, you can toggle this option from the Leaders tab.
It’s often necessary to add multiple dimensions of this type, and once the first dimension is placed, the centerline selection remains active, making it easier to add additional dimensions without having to select the centerline each time.
