SOLIDWORKS 2014 introduced the All Uppercase option for Note Annotations. Forgetting to use CAPS LOCK is no longer something to fear.
There was a dark time when one had to remember to turn on CAPS LOCK keyboard toggle while they created engineering drawing notes. This was problematic because if you forgot, you’d have to retype everything. If you were creating your general notes, that was a lot of retyping. Even if you remembered to use CAPS LOCK, you’d still have to find workarounds for file properties and certain custom properties that displayed the raw system value, where capitalization wasn’t possible. A light shined upon the world in 2013. That year, SOLIDWORKS 2014 introduced the All Uppercase option for Note Annotations.
However, unlike word processor applications, SOLIDWORKS is smart about how it capitalizes text.
Original text is preserved, so if you turn the setting off, your text returns to its original state.
The setting recognizes the value of file and custom properties and capitalizes these as well.
Where you would want the “mm” in the word “dimmer” to capitalize as “DIMMER”, you wouldn’t want the “mm” in “10 mm” to capitalize. So, along with the new functionality, SOLIDWORKS is smart enough to know the difference by using its Exclusion list.
There is the ability to use the capitalization setting as a Document Property, meaning that any note you create will automatically use the All Uppercase setting. You still have local control for each note, of course.
SOLIDWORKS 2018 introduced this functionality for Tables in SOLIDWORKS. You can change the setting for an entire table, a range of cells or individual cells.
Finally, SOLIDWORKS 2020 introduced this functionality for Dimensions (including Hole Callouts).
You have the ability to set All Uppercase document defaults differently for Notes, Tables and Dimensions, so if you want to automatically capitalize your notes, but not your dimensions or tables, you have that choice.
One more point; a tip:
Select a note.
Hold down SHIFT and press F3.
While holding SHIFT, each time you press F3, you will toggle All Uppercase on and off for the selected note.
This is the same keystroke as MS Word for switching between casing options.
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”.
There was a heavy focus on expanding functionality of angle dimensions using the Smart Dimension tool in SOLIDWORKS 2015. These enhancements streamline drawing detailing and sketch creation tasks. Here’s the first of such enhancements.
There is a long standing request for the ability to apply angle dimensions where one ray is aligned to geometry (model edge or sketch line) and the other ray is along an imaginary vertical or horizontal direction. In SOLIDWORKS 2015, there is a new capability with Smart Dimension tool that enables you to create this type of angle dimension.
Start the Smart Dimension tool.
In a drawing view, select a model edge.
Select a collinear and adjacent point (vertex or sketch point).
A crosshair appears over the selected point. Select one of the crosshair’s segments.
For drafters that need more control over how dimensions are displayed on their drawings, SolidWorks 2014 has introduced a couple of new controls. First, styles for extension lines and dimension lines can now be assigned independently from each other on dimensions. The default line styles can be set in Document Properties for each dimension type, and within the Dimension PropertyManager.
In the PropertyManager, a new group box has been added, called “Extension Line Style”. Within this group box, there is an option to keep the line style that same as the leader/dimension style with the option “Same as leader style”. If you wish to use the document defaults, selected “Use document display”.
If both of these settings are unchecked, you can set the extension line for the selected dimensions separately from the dimension line style. The example here shows the line thickness as different.
Second, you can now set individual extension lines to display as centerlines. This allow you to identify extension lines that emanate from holes, per ASME practices. To make this change, right-click on the extension line and select “Set Extension Line as Centerline”.
To change it back to normal style, right-click on the extension line again and select “Reset Extension Line Style”.