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.
The people (i.e., SolidWorks users) have spoken and SolidWorks Corp listened. The infamous Dimension Palette now functions differently. The controversy surrounding the Dimension Palette started almost immediately after SolidWorks 2010 SP0 was released. People started posting heated complaints in the SolidWorks forums. I addressed many of those complaints in a previous article.
How has Dimension Palette changed? It no longer comes up automatically when the user accesses a dimension on a drawing. Instead, when one or more dimensions are selected, a Dimension Palette button appears above and to the right of the mouse pointer’s location. This is similar to other pop up toolbars, such as the Shortcut Menu.
To active the Dimension Palette, simply move the mouse cursor over the Dimension Palette button. This will pop up the Dimension Palette. From there, use of the Dimension Palette is the same as before.
Some minor visual tweaks were also added to improve the look and control of the Dimension Palette. The corners are now rounded. There is also the addition of a Move tab that allows the Dimension Palette to be moved around the view pane by the user.
New behavioral improvements allow the Dimension Palette to be more predictable. If the user interacts with the Dimension Palette, it will remain on screen for as long as the dimension selection is active and the mouse cursor remains in the view pane. If the Dimension Palette is brought up by the user but the user does not interact with it, the Dimension Palette will disappear when the mouse pointer moves away from it. If this happens, simply press the CTRL key to bring the Dimension Palette button back, if desired. Also, if the Dimension Palette pops up and it is not wanted, it may be banished by pressing the ESC key.
I’ve had a chance to use this new functionality already. The changes to Dimension Palette represent serious improvement! I’m not going to say the solution is complete. I believe development of the Dimension Palette needs to mature before it becomes a classic like the Shortcut Bar. These improvements do make it more user friendly. If there are no other reasons to upgrade to SolidWorks 2010 SP3, the improvements to the Dimension Palette are reason enough.
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.
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.
Foreshortened linear diameter dimensions are not specifically supported by ASME Y14.5M-1994. I don’t know if “ASME Y14.5M-2009” will have such support added. Even if not, there is a common practice of showing foreshortened diameters. SolidWorks supports the two most common delineations for these.
To have a foreshortened diameter dimension, the diameter being dimensioned will have to be cut off in the view. This means effective use of these is pretty much limited to detail views, since this is likely to be the only place one would normally use such dimensions. I may try to experiment in the future to see just how far I can stretch SolidWorks functionality in this area, but for this article, I’m going to stick to the basics. Please note that these instructions are SolidWorks 2009 based. Steps will be similar in older versions, but may not be exactly the same. They will be close enough to make this a good guide, though.
To employ a foreshortened diameter dimension, there is some preparation needed within the model. You cannot just insert your model into a drawing and add a non imported dimension onto a circular feature. Because of the way Hole Wizard functions, foreshortening will also not work for holes created with it. Why? I’m not sure as to the reasoning. I just know SolidWorks only enables this function for imported dimensions (dimensions inserted from model).
Start a sketch in your model. This sketch will become your feature.
Draw a circle.
Dimension that circle as a linear diameter dimension. This will not work if the dimension is radial.
Make sure this dimension is set as mark for drawing.
Create a feature from the sketch.
On the drawing
Insert the model onto a drawing. Create a detail view which cuts across a circular feature.
Once the drawing is set up, here are the steps.
If the center of the circle appears in the detail, select the detail view by LMB clicking it. If the center does not appear in the detail, then select the parent view instead.
Insert model items. This can be done by Insert pulldown>Model Items. One of the dimensions to appear will be the diameter of the circular feature.
Click OK in the PropertiesManager Pane to accept and close Model Items panel. If already in the detail view, you are done. The dimension will appear as a foreshortened linear diameter dimension. However, if working in the parent view, a few more steps are required to get the desired effect.
Hold down the SHIFT key. Select the diameter dimension by clicking and hold the LMB over it.
Drag the dimension in the detail view. Let go of the LMB and SHIFT key. This will copy your dimension into the detail view. The dimension will appear as a foreshortened linear diameter dimension.
Delete the dimension from the parent view.
SolidWorks is very particular about how it allows foreshortened linear diameter dimensions. These steps must be followed exactly in the manner described here. I wish SolidWorks made it easy to implement foreshortened diameter dimensions, including allowing them for non inserted dimensions.
Future articles on this topic will discuss styles of foreshortened delineation (how to get double arrows instead of the zigzag dimension line).Â It will also discuss one work around so foreshortening can be applied to other types of linear dimensions, producing a result sometimes called clipped dimensions.