SOLIDWORKS uses Smart Dimensions, in addition to relations, to help fully define sketches. inWhether it’s the length of a line, a hole distance from an edge, or any other measurements that need to be established, adding dimensions to a sketch is always good practice to ensure the user’s design intent is captured correctly. What users may not know is that where you click and what you click on can result in different dimension placement. Here are a few tricks when inserting dimensions:

Lock dimension position

SOLIDWORKS lets users control the position of dimensions after entities have been selected and the dimension is displayed as a preview. Once the dimension is locked in place, a user can only drag it in the direction it is locked in.

To lock a dimension:

1. Select Smart Dimension.
2. Click the line(s) or point(s) to dimension.
3. Move the pointer until the preview indicates the dimension position desired. Notice the icon next to the pointer.
4. Right-click to lock the dimension’s position. The lock on the mouse icon should change.
5. Pull dimension to desired location, click to place.

Doubled distance from centerline

A doubled distance is a value that is two times the distance of the sketch entity to the centerline. Doubled distance relations help to determine the equal distance to the other side of the centerline and are helpful when creating profile sketches for revolved features.

To insert a doubled distance:

1. Select Smart Dimension.
2. Click either the solid line or the centerline.
3. Select the other line.
4. Drag pointer to opposite side of the centerline.

Dimension to edge of an arc or circle

By default, when dimensioning to an arc or circle SOLIDWORKS will place the dimension to the center point of the arc/circle as seen in the first pair of circles below (27.36mm). Users are also able to dimension to the edges of the arc/circle if preferred.

To dimension to the edge of an arc/circle:

1. Select Smart Dimension.
2. Hold Shift when selecting edge(s) of an arc/circle to be dimensioned to.

Arc length

Instead of dimensioning an arc and getting a radius, SOLIDWORKS easily allows for the arc length to be found. This works for sketch fillets as well.

To insert an arc length:

1. Select Smart Dimension.
2. In any order, select the arc and both end points.

Arc angle dimension

Finding the angle of an arc is quick to do with SOLIDWORKS. With just three clicks of the mouse the dimension is already shown.

To insert arc angle:

1. Select Smart Dimension .
2. In any order, select both end points and the center point of the arc.

Angular dimension using imaginary lines

Angular dimensions from imaginary horizontal and vertical lines makes it easy to apply an angle to a line. This saves time by avoiding additional construction geometry needed for referencing. The dimension can be locked in position by right clicking after selecting the line and end point.

To insert an angular dimension using an imaginary line

1. Select Smart Dimension.
2. In any order, select the line and an end point.
3. Choose one of the imaginary line arrows to dimension from.

Virtual sharps

A virtual sharp is a point where the virtual intersection of two lines would meet. Dimensions and relations can be applied to virtual sharps.

To insert a virtual sharp:

1. Select Smart Dimension .                                     1.  Begin in edit sketch or in a drawing view
2. Right click on one of the lines                OR         2. CTRL select both lines
3. Select “Find Intersection”                                     3. Choose Sketch Point command
4. Click on other line

Copy/Move dimensions in drawing views

Dimensions in a drawing can be copied or moved into another view. The orientation of the drawing view must be appropriate for the dimension.

1. Hold Shift to move or Control to copy dimension.
2. While holding Shift or Control, click and drag dimension to another view.