Modify Dimension Box
The modify dimension box, that appears when adding or editing a dimension, can be used in a number of useful ways to speed up the design process.
When adding a dimension, the default unit system is used to add the dimension, let’s assume this is millimetres. To quickly add in a dimension using a different unit system, such as inches, simply type in the required value and then choose from the unit drop down. The value will then be converted back into the default units.
As well as picking from the unit drop down list, unit symbols can also be typed, so for example, millimetre is ‘mm’, and inches could be input as either the inch symbol ‘quotation mark’ or ‘in’.
Lock Projection
Linear dimensions can be added in a variety of different ways, such as selecting a single line, selecting a line and an endpoint or selecting two endpoints.
When selecting a single line or two endpoints, the projection of the dimension can be placed, horizontally, vertically or parallel to the selection. It’s important to understand this as if the dimension is added incorrectly, the length will not be as required. This is obvious when working across angles such as 45 degrees, but becomes less obvious when working with lower value angles.
To help with this, the dimension projection can actually be locked before the dimension is placed, and this done by clicking the right mouse button, indicated by the padlock icon. Once this has been locked, the dimension can then be positioned anywhere within 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 centre 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 making a selection, and click to the side in which the dimension should be anchored from.
Shift should be held down for each selection, unless the centre 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.
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.
Radial and Diametric Dimensions
When creating sketch geometry for revolved parts, a dimension can be added either as a radius or a diameter value.
Selecting the sketch geometry and then a centreline, allows the dimension to be placed as a radial value, or if the dimension is toggled across the centreline, the dimension changes to a diameter. When this type of dimension is added, no radius or diameter symbols exist initially, so if this is required, with the dimension selected, click the diameter button within the dimension properties.
Once a dimension has been added in this way, if a diameter needs to be changed to a radius or vice versa, this can be toggled from the leaders tab. It’s common to need more than one dimension of this type too so once the first dimension has been added, the centreline selection is maintained, allowing more dimensions to quickly be added, without the centreline being selected each time.
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.
Virtual Sharp
When dimensions need to be added to a corner that no longer exists, a virtual sharp can be added to dimension to. This can be achieved in a few different ways.
To add a virtual sharp in manually, control select two entities and then click the point tool. This adds in a virtual sharp to the sketch that can then be dimensioned to.
Virtual sharps can also be added as part of the dimensioning process. With the smart dimension tool already active, right click on the first sketch line and choose ‘find intersection’, then click on the second sketch line. The virtual sharp is added and the dimension attached to it, ready for the dimensions second selection.
Mouse Gestures
We’ve mentioned mouse gestures in a number of previous blogs and videos as they are such an efficient way to access commands within SolidWorks, and the same goes for dimensioning.
Using the default settings, holding down the right mouse button and dragging up will prompt the smart dimension tool in both the sketch, and the 2D drawing environment.
Check out our blog and video on customising SolidWorks to improve performance for more information on how to maximise what can be done with mouse gestures.
