SolidWorks 2010 Usability: Attach Annotations to Dimensions

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.

Select annotation text

Then, simply drag that annotation note on top of the dimension.

Selected text becomes apart of 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 attach in more ways to dimensions

  • 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.

SolidWorks 2010: Dimension Palette and Styles

Dimension Palette is a great new function in SolidWorks 2010 that allows the user to edit most commonly accessed aspects of a dimension, right from the main drawing view pane.

Simply highlight or LMB click on a dimension. A ghost image of its Dimension Palette will appear nearby.  Move your mouse cursor over the ghost.  This forces it to fully materialize.  (I’m reminded of Ghostbusters for some reason.)

Dimension Palette

From that point, many of the dimension’s attributes may be directly edited, such as tolerance style and range, dimension accuracy, and tolerance accuracy.  Also editable is text above, right, left and below the dimension.  Additionally, formatting is editable, including dimension position and justification, reference parenthesis, and inspection obround outline.  To aid in use of these new functions, small pop-up hint fields appear as the mouse cursor moves over each element.

Finally, the user can also quickly apply saved Dimension Styles (formerly known as dimension favorites) to the dimension.  This can be accessed by clicking on the gold star icon in the upper right of the Dimension Palette. Dimension Styles are much more automated than the old dimension favorites.  Not only does the user have access to any saved Styles, SolidWorks will also restore recently used formatting changes as Dimension Styles.

Dimension Styles

This means, when the user makes a change to a dimension, SolidWoks will automatically save the user’s change as a Dimension Style.  Automatically saved Dimension Styles will show up in the Recent tab of the Styles window.  These Styles only reside in the current drawing.  (In order to use these Styles in another drawing, the user will still have to save the Style in the same way dimension favorites have been saved in previous SolidWorks releases.)

To replicate the same changes to multiple dimensions, the user simply has to edit one dimension (preferably through the Dimension Palette).  From that point on, to apply those same changes to other dimensions, the user need only select the Dimension Styles button for affected dimension and select their previous change from the Dimension Styles window.

Basically, the user can paint any various dimension formats as Styles to any following dimension.  This is a very cleaver execution of a long standing Enhancement Request to allow dimension formatting to be quickly copied from one dimension to another.

Don’t quote me on this, but if I remember correctly, the current limit on the number Dimension Styles stored in the Recent tab is ten.  This may change at some point.  One added function I’d like to see within the Styles window is the ability to delete Dimension Styles from the Recent tab.  As always, with any great new functionality comes even a greater number of new requests for improvement.

Dimensioning of Slots in SOLIDWORKS for ASME Y14.5

This entry is part 4 of 8 in the series Dimensions and Tolerances

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.

Dimensioning Method (a)

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.

Dimensioning Method (b)

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).

Dimensioning Method (c)

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.

Foreshortened Linear Dimensions (Clipped Dimensions)

As mentioned in another article in this series, SolidWorks does not support the foreshortening of linear dimensions, except in views where both ends are visible in the view, such as break views.  Also mentioned was that foreshortening of linear dimensions doesn’t make much sense in most circumstances because both ends of dimension must be in view for a drawing’s reader to understand the callout.  As such, they are not supported by the ASME standard.  Even still, there may be some cases where it is necessary or desired to clip a dimension within detail or partial section views.

There is one potential workaround to allow this in SolidWorks, using a series of double arrow symbols created by Jeff Hamilton.  Jeff’s creation requires a modification to your gtol.sym file.  Unfortunately, to implement this change, you’ll either need to be a one man show or a CAD Administrator who has time to update everyone’s computers with the edited gtol.sym file.  This is because any symbols within a drawing reside in the gtol.sym file, and that file is specific to each and every install of SolidWorks.  Another drawback is that the user must visually and manually align the double arrows into the appropriate position.

Selection of double arrows

Barring these drawbacks, this is a pretty good solution for those who really need this function.  The file can be downloaded at this location:  Geometric Tolerancing Symbols Library Foreshorten Arrows Add-on.  Instructions on how to edit the gtol.sym file and use the new symbols are included in the download.  Have fun!

Color for non inserted dimensions

SolidWorks has many default colors for different types of dimensions.  On drawings, the two main types of dimensions are inserted (driving) and non inserted (driven).  Inserted dimensions are called such because they are inserted from the model.  Non inserted dimensions are created within the drawing itself.  I’m not going to get into the philosophies about which is better to use and when.  Let’s just stick to the topic that many times both are necessary on a drawing, and that they appear as two difference colors. Inserted dimensions are black and non inserted dimensions are grey, by default.

A problem pops up when using or printing the drawing while in Color Display Mode is on.  When this mode is turned off, all dimensions appear black, but so does everything else, including watermarks or lines on special layers.  So, many of us rely on the Color Display Mode.  When this mode is turned on, the user gets their colors right for other lines, but dimensions appear as both black and grey.  This can send a confusing message to someone who must later read the drawing.   Also, on some printers, the grey color may be washed out and unreadable.

Example of different colors

So, I have a quick trick to overcome this issue.  Simply change the color for non inserted dimensions within the System Options.   What color to use?  Well, if one still wants to know the difference between inserted and non inserted dimensions when editing the drawing, I recommend not picking black.  Instead pick the darkest grey available.  This will allow you to see the difference in SolidWorks, but such a difference will not be obvious in any printouts or PDFs.

To make this change in SolidWorks, goto Tools pulldown>System Options>Color heading.   In the Color schemes settings box, select Dimensions, Non Imported (driven).  Click the Edit button.  A traditional Windows color palette window will appear.  Use this window to create a very dark grey color and then assign it to one of the slots in the Custom colors area.  Choose that color as the setting and click OK to exit.  Then click OK in System Options to implement the change.

Color change location

All inserted dimensions will continue to be black, and non inserted dimensions will now be that dark grey.   Since this is System Options setting, it affects any drawing that is opened without having to enter the Document Properties area every time.  I’ve personally used this trick successfully for a long time.

Radius and Diameter Dimensions (switching these in SW 2009)

It doesn’t matter if the dimension starts off as a radius, diameter, or a linear diameter dimension (on a drawing in a model).  One can become another quickly in SolidWorks 2009.

Step 1:  To change a radius to a diameter, RMB click on the radius dimension.  Choose Display Options>Display as a Diameter.

Step 2:  To change a diameter dimension into a linear diameter dimension, RMB click on the diameter dimension.  Choose Display Options>Display as linear.

Unfortunately, there is no way to shortcut these steps from a radius dimension to a linear diameter dimension.  If starting out as a radius, both of these steps will need to be followed in succession to get a linear diameter dimension.  Same goes for the reverse.

One word of caution when switching to a linear diameter dimension though; it will often not come in aligned to the Y or X axis, which may render it unuseful for certain circumstances.