## Angles and their relationships

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.

### Conjugate?

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.

## Sneak Peek of SolidWorks 2013: Auto-Dimension While Sketching

From the SolidWorks Blog:

While SolidWorks has had the ability to add dimensions while sketching for some time, SolidWorks 2013 makes it a whole lot more intuitive. Now, when you enter dimension values while sketching, SolidWorks will automatically add it to the geometry.

## How to dimension feature patterns on drawings

A couple of days ago, I briefly covered the mythical specification “non-accumulative tolerance” (or “non-cumulative”) as it is often applied to direct dimensions on feature patterns.  See the example in Figure 1 where the dimensional callout attempts to simply dimension a pattern without considering tolerance stack-up.  However, this attempt fails since any two non-adjecent holes cannot avoid accumulation of tolerance due to the dimensioning scheme.  The problem gets worse if three or more positions within the patten are compared to each other.

#### ASME repetitive feature dimensioning scheme

ASME Y14.5-2009 actually provides a linear method to detail feature patterns, called repetitive features and dimensions.  See Figure 2. Unfortunately, the standard does not provide any tolerance rules for its prescribed scheme. Presumably, this leads us to interpret a repetitive feature dimension as though it is shorthand for chain dimensioning.  Chain dimensioning accumulates tolerance as the pattern departs from the dimensioned start position.  Sometimes this is OK, but often this is unacceptable since the accumulation of tolerance can quickly lead to features that do not align to mating features on other components.

#### Disorganized direct dimensions

Another dimensioning scheme that I’ve seen involves a complete disregard for the fact that a pattern exists.  See Figure 3.  Directly dimensioning each of the positions within the pattern to each other may be acceptable in some scenarios, but likely isn’t a very clear choice for larger feature patterns.  The problem with this scheme is that it can be very difficult to determine the true accumulation of the tolerance stack-up.  It may also be difficult to determine design intent.

#### Baseline dimension scheme

To avoid the issues associated with other direct dimensioning schemes, one may choose to use baseline dimensioning, which may also be called rectangular coordinate dimensioning in some scenarios.  The advantage of a baseline dimension scheme is that it limits the accumulation of tolerances to the stake-up from just two dimensions.  This is because the total stack-up between any two positions within the feature pattern are related through a common baseline.  The problem with baseline dimensioning is obvious in Figure 4; its take up a lot of space on the drawing.

#### Ordinate dimensioning

A common alternative to baseline dimensioning is ordinate dimensioning, also known as rectangular coordinate dimensioning without dimension lines.  This scheme also relies on a baseline, referred to as zero (0), from which all of the features are dimensioned.  The advantage of ordinate dimensioning is that it takes up far less space on a drawing, as shown in Figure 5.  Tolerance stack-up is limited to just two dimensions between any two positions within the pattern.

#### Using GD&T for best results

The best way to avoid accumulation of tolerances is to use a methodology that does not rely on any form of direct dimensions.  ASME Y14.5 actually suggests that GD&T should be used instead of direct dimensions to locate features.  I have discovered the hard way that many individuals in the engineering field have an irrational fear of GD&T.  Even still, GD&T provides a far superior method for the location of positions within a feature pattern. The example in Figure 6 shows a less cluttered drawing.  With the addition of MMC to the feature control frame, this method could provide even better results since it would make use of bonus tolerance.  The position of each feature within the pattern has an optimal tolerance zone that more closely matches design intent.  One more added benefit is that all features controlled by a single feature control frame are automatically considered as a pattern.

Since the tolerance zone is optimized, using GD&T may help reduce costs by allowing the manufacturing process to vary in a way that is more in line with design intent.  In turn, this can reduce the number of unnecessary part rejections.

#### Conclusion

When detailing feature patterns, one may wish to avoid the use of direct dimensioning methods or shortcuts like the mythical “non-accumulative tolerance”.  The best choice to detail a feature pattern is GD&T.  However, if GD&T is not desired, the next best method is prolly an ordinate dimension scheme.  It should be noted that for each of the dimensioning and tolerancing schemes shown within this article, there are a variety of ways to implement them.  This article is meant to present general examples.  Actual tolerancing requirements are guided by design intent and other considerations per individual cases.

## SolidWorks 2010 Rapid Dimension

Adding dimensions to parts on drawings is now quicker in SolidWorks 2010 with the addition of Rapid Dimension.  Once the user enters the Dimension command, Rapid Dimension allows the them to quickly position dimensions (almost automatically) as they are added.  Not only will dimensions automatically space out correctly as they are inserted, they will be inserted at the correct location, even without that location in view.

Now, each time a dimension is added to a drawing, SolidWorks will pop up with a pie, divided into two pieces for linear dimensions or four pieces for radial dimensions.  (Technically, these pies are called the rapid dimension manipulators.)

Each piece of the pie represents the direction (which side of the part) that the user can choose to place their new dimension.  When the user selects the half or quarter, the dimension is placed in the correct location on that side of the part within the drawing view.

Two methods can be used to select the dimension location using the pie.  The user can simply LMB click on the portion of the pie in the desired direction.  The user can also use a mouseless method, by pressing tab to toggle between the pieces of the pie; then press the spacebar to select.  Additionally, the user can choose the ignore the choices offered by the pie to manually place the dimension, just as they would in previous versions of SolidWorks.

The auto-spacing between dimensions is determined by the user’s settings in Tools>Options…>Document Properties>Dimensions within the Offset distances field.  The ability to set default dimension line offsets has been in SolidWorks for quite some time, but it’s never been quite so useful as it is in Solidworks 2010.

Within a few minutes of using Rapid Dimensions, many users will likely become instantly addicted to the new function, as it promises to be a major time saver when detailing drawings in SolidWorks 2010 and beyond.

### Deleting Dimensions

One additional item about dimension placement is SolidWorks behavior when a dimension is deleted.  If the user deletes a dimension or even just removes text from a dimension, SolidWorks has the ability to automatically realign the spacing of the neighboring dimensions to get rid of gaps caused by that deletion.  The user has the option to turn this ability on by going to Tools>Options…>Document Properties>Dimensions to select the Adjust spacing when dimensions are deleted or text is removed checkbox.

## Dimensioning of Slots in SOLIDWORKS for ASME Y14.5

Ever since the additions of the slot sketch tool for 2009 and the Hole Wizard Slot for 2014, SOLIDWORKS almost seems like a whole new software for the those who design machined parts.  Adding these tools were long overdue.  Additionally, SOLIDWORKS supports the standard methods for dimensioning slots when they are created by using these tools.

ASME Y14.5M-1994 paragraph 1.8.10 and figure 1-35 provide three methods for the dimensioning of slots, with no stipulation regarding which is preferred for particular scenarios.   (Note: all three methods require the insertion of a non-dimensioned “2X R” note pointing at one of the slot’s end radii.)

In one fashion or another, SOLIDWORKS supports all three methods, though it does have a default for both simple slots and arc slots.  For brevity, this article will only cover simple slots.

The first slot dimensioning method (a) provides the width and the distance between the end radii center points.

`Method (a)`

The second method (b) is the easiest and simplest to dimension.  Simply state width and overall length, and use an arrow to point to the slot’s object line.  Though originally reserved for punching operations, ASME Y14.5M-1994 (and later versions) allows for the use of this method on any simple slot.  When using Hole Callout to dimension a slot in SOLIDWORKS 2009 or later, this is the type of dimension that is inserted.

`Method (b)`

The third method (c)  provides the width and overall length of the slot in linear dimensions.  This method is preferred if the slot has positional tolerances that use the boundary method (see ASME Y14.5M-1994 figure 5-47).

`Method (c)`

For all of the above methods, add the “2X R” separately by using Smart Dimension tool.

Side note: of the three choices, the ASME board almost left out (a) and (b).  The original release draft of ASME Y14.5M-(1994) only shows method (c) in figure 1-35.