Uncommonly known types of related angles, and their SOLIDWORKS support. Some may surprise!
Geometry establishes a lot of imaginary objects and relationships between them in order to define models and the real world. Angles are an important set of those relationships. But, we often skip or forget types of relationships between angles. Let’s look at related angles. Related angles are pairs of angles that have some sort of relationship to each other. Several types of related angles are established by Geometry. Some may surprise, as they aren’t commonly known.
Types of related angles
Complementary angles – a pair of angles with a common vertex and a sum of a right angle (90°).
Supplementary angles – a pair of angles with a common vertex and a sum of a straight angle (180°).
Explementary angles – a pair of angles with a common vertex and a sum of a full circle (360°).
Vertically opposite angles – a pair of angles that equal to each other and are vertical-and-opposite of each other with a common vertex. These angles are formed by two intersecting lines.
Of course, a single complementary angle is one of the pair of complementary angles. A single supplementary angle is one of the pair of supplementary angles. A single explementary angle is one of a pair of explementary angles. And, a single vertically opposite angle is one of a pair of vertically opposite angles.
The term conjugate angles is sometimes used as a synonym for explementary angles. Technically, conjugate angles is a set of angles with a sum of 360°. Despite the word conjugate meaning coupled/related/connected, it seems that the term conjugate angles is a set that need not be made up of only two angles, and so the angles within the set are not necessarily related angles, though they are connected by a common vertex. Additionally, the term conjugate angles does not apply directly to any angles within the set, but only to the set itself, so there’s no singular form of this term.
SOLIDWORKS support for angle dimensions
Though explementary and vertically opposite angles are not as common as supplementary and complementary angles, they are important from time to time when designing and defining mechanical components and assemblies. As such, SOLIDWORKS has supported both explementary and vertically opposite angles since release 2015. See Year of the Angle Dimension – Part 2 – Flipping out (and over) and Flipped Angle Dimension in SOLIDWORKS for information on how to use these types of angles in your dimension scheme.
Other types of angle dimensions in SOLIDWORKS
Another type of angle supported in SOLIDWORKS since release 2015 is the straight angle (180°). You can dimension two lines that form a straight angle.
Also, angle dimensions can be created from one line and one vertex instead of always from two lines.
What do you do when you need to create an angle dimension at 180 degrees? Maybe you need a 180 degree angle driving dimension between two sketch lines for sketch mechanisms. Maybe you just want to show the relationship between two parts of an assembly at a particularly point in their motion relative to each other, expressed as configurations. Or, maybe you just want to create a 180 degree angle, just because. Previously, you were blocked from creating such a dimension directly. In order to create a 180 degree dimension, you had to move some geometry (sketch line, components, features) slightly off 180 degrees, create your dimension, then edit whatever was necessary in order to restore the 180 degree angle.
SOLIDWORKS 2015 Smart Dimension tool now supports the creation 180 degree dimensions directly. No longer is it necessary to use the workaround. For sketches, the two lines that form the rays of the 180 degree angle must either share a vertex, or be separated where a vertex is inferred from their intersection. Just start the Smart Dimesnion tool and select two colinear non-overlapping entities, and a 180 degree angle will be generated for you.
Previous releases of SOLIDWORKS introduced linear dimensions in sketches that can be applied symmetrically when created across a centerline. Further enhancements saw smarter behavior, where the selected centerline is remembered for multiple dimensions created in sequence. For SOLIDWORKS 2015, you can create multiple half and full symmetric angular dimensions without selecting the centerline each time.
To create a symmetrical angle dimension:
- In a sketch with a centerline and lines or points, click Smart Dimension at Tools>Dimensions>Smart.
- Select the centerline and another line which is at an angle to that centerline.
- To create a half angle dimension, move the mouse cursor to the desired location and click to place, as previously. However, to create a full angle dimension (across the centerline), hold down the SHIFT key.
- Drag the mouse cursor (along with the previewed dimension) to the opposite side of the centerline. As you do so, a preview of the angle dimension will appear symmetrically about the centerline.
- Click to place dimension as desired.
- Keep holding down the SHIFT key and select other lines at angles to the centerline. Angle dimensions to the centerline will automatically generate and will allow you make more symmetric angle dimensions successively.
When you use angles that are set to deg/min and deg/min/sec, there are often times when you’ll have zero (0) for one of the levels of units. For example, an angle may be 43 degrees, 0 minutes and 20 seconds. This is displayed as 43° 0′ 20″. For many people, the 0 minutes is redundent and unnecessary. SOLIDWORKS 2015 now has an option that allows you to show only the unit levels that have a non-zero value. For this example, the display is 43° 20″. This new setting can found at Tools>Options>Document Properties>Dimensions/Angle, and named “Remove units with 0 value for deg/min and deg/min/sec”.
With all the new functionality with view labels in SolidWorks 2014, some ancillary enhancements have also come about as a result from customer feedback during Beta Testing. One of these enhancements has been the new capability to display any view’s angle within an annotation note. Why would anyone need something like this?
Well, there are four default options for the display of the angle symbol auxiliary views.
- Show rotation symbol with rotation angle
- Show rotation angle
- Show the text “ROTATION” followed by the rotation angle and direction
- Show just the angle
If your company chooses to display just the rotation angle (as is common for GOST drawings), it is still sometimes necessary to display the rotation angle. Because the view label is a global setting within the drawing, there’s no way to accomodate this deviation from the standard settings without having some hugely complicated user interface to track individual labels here and there. So, instead, one additional annotation tag has been added. The advantage is that this new tag is available for any drawing view (not just auxiliary and section views). The new tag is <VIEWANGLE>. Type this into any annotation note. As long as that note is a attached to a view, that view’s angle will be shown. As an example, this new tag can be added to the auxiliary view label after the <VLANGLE> tag (or anywhere else in the note).
The settings and the result of using the new tag: