Revision clouds is a new annotation type in SolidWorks. The main purpose for revision clouds is to allow you to call attention areas where a revision was made on a drawing. Though revision clouds are not the same as comment clouds in eDrawings, you may also want to use it to highlight comments for redlines, if you wish. Revision clouds are likely the most entertaining annotation, as you can also get artsy and make actual cloud shapes just for the fun of it.
Making a revision cloud is easy. Open up a drawing in SolidWorks 2013, goto the annotations tab on the CommandManager. Nearby Revision Symbol, you’ll find Revision Cloud. The PropertyManager allows you choose cloud type, Rectangle, Ellipse, Irregular Polygon and Freehand. You can also control the maximum size of the cloud puff radius, line type, line thickness and layer. Color can also be controlled via the layer or by using the Line Color tool in the Line Format toolbar. Here’s some examples.
Elliptical cloud around a dimension
You can group the dimension and cloud together
Once grouped, the cloud and dimension will move together
Example of a rectangular cloud
Example of an irregular polygon cloud
Example of a freehand cloud with a different line style
SolidWorks provides the ability to support many different shapes for flag notes. In addition to shapes, there are several methods in SolidWorks to create flag notes on a drawing. Each method gives a slightly different result in how the flag note symbol looks and how it is attached to the leader line. Part 1 of this article will cover shapes and the flag note symbols.
Flag note symbol shapes
There are two general methods to add flag note symbols to an Annotation Note.
The first (and older) method is to use the symbol library. There are literally hundreds of symbols included within the library. The library supports triangle, square and circle symbols for numbers and letters, with or without the period. This method inserts a tag into the Annotation Note, which then generates the flag note symbol, based on existing data in the gtol.sym file.
Using the Flag note symbols from the symbol library
To use this method, create the Annotation Note with a leader.
While in the edit mode, click on the Add Symbol button in the PropertyManager.
This opens up the Symbol Library. Pick the appropriate flag note symbol and OK.This opens up the Symbol Library. Pick the appropriate flag note symbol and OK.
This will insert the symbol into the Annotation Note.
If the triangle is chosen, the resultant symbol is not an equilateral triangle. The square and circle symbols are truly squares and circles, respectively. Note the gap between the flag note and leader. This gap can get bigger or be completely removed with a different method, which I will go into in part 2 of this article.
I have to admit my original Balloon Note macro was quite quirky. It was the most complicated VBA project I’d done at the time, so I don’t feel too bad about it. I finally had a chance to try out the SolidWorks 2010 implementation – SO – I decided to rethink the whole thing. WOW – I really have to apologize, I’m surprised that old code worked at all. However, if you liked the general idea found in my original Balloon Note macro, I’m sure you’ll like this completely rebuilt version.
If you have no idea what I’m writing about:
Balloon Note is designed to add a Reference Note to an existing Item Balloon and Group them together automatically. It can add an automatically updating Quantity Text object. The result is similar to a function SolidWorks added in 2010, but, you can adjust the location of the text using the ALT + Select and drag method. The strange squiggle (QTY variable) in the text box represents the selected part quantity, until you apply the Reference Note location (Top, Right, Bottom or Left). Balloon Note uses your current document setting for the Note font height to create the Reference Note. The Links button uses a plain text file “BalloonNote_07.ini” located in the same directory as BalloonNote_07.swp to store your lists of links and symbols. The download includes two versions, BalloonNote_07.swp for SW 2007 (you could possibly change the Reference Libraries to your version) and BalloonNote.dll for SW 2010 x32.
SolidWorks move towards quality has affected many areas in SolidWorks 2010, including annotation functionality. One of particular note is the fact that borders around text can now be added within an annotation note!
The following example has borders added to text using only this new method. No <> tag symbols where used:
Access to this functionality is in the same place as before, under the Border heading within the Note PropertyManager. The only difference is that the border selection now responds to highlighted text within the affected Note. In fact, it only responds to highlighted text now.
Because of this new functionality, some behavior has changed with making flagnotes. As of Beta 2, notice that they will no longer directly attach to a leader unless they are round (Circle border). Some may like this, others may not. Another behavior that might need to be taken into consideration when using these borders is that spacing between lines may be affected, as also shown in the example. Also, this functionality is not supported within dimension callouts.
There are a ton of subtle improvements in SolidWorks 2010 to improve its usability. Many of these improvements might seem small now, but once one is reliant on the new functionality, it will seem like we’ve always had it this way. Attaching annotations to dimensions is now easier with expanded capability. Here’s a couple of examples showing-off these new capabilities.
Drop Annotation Notes into Dimensions
It is now possible to drag an annotation note and drop it onto a dimension, to become apart of that dimension callout. First, LMB click and hold on the annotation note.
Then, simply drag that annotation note on top of the dimension.
The result is that the text from the annotation note is now included within the text of the dimension. One limitation is that the dimension field still does not support borders around selected text.
Attach Annotations to Dimensions
Other types of annotation that can be attached to dimensions include GD&T feature control frames, datum feature symbols and surface finish symbols.
- Annotations and their leaders may now be attached directly to extension lines.
- GD&T annotations now may be dropped right into a dimension callout and then detached with the use of the handles in the upper left corner.
- Annotations may now be moved around extension lines, and more easily moved from one attachment to another.