Tag: dimension

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.

Foreshortening Dimensions (Radial, not linear)

[Updated to address changes in SOLIDWORKS 2016]

SOLIDWORKS provides for the foreshortening of diameters and radii dimensions.  Older releases of SOLIDWORKS didn’t allow for the foreshortening of linear dimensions (or clipped dimensions), except in break views where both ends of the dimension are visible.  When I first encountered this limitation years ago, I was concerned that SOLIDWORKS developers just simply overlooked this functionality.  After all, if one can foreshorten a radius, then why not a linear dimension?  I was even sure I could find examples of this already being done on other drawings in detail views.  I was trying to use an open ended dimension line with double arrows on the open end.  I may have actually used this method a couple of times back in my AutoCAD days.

But what didn’t SOLIDWORKS support this for many years?  The lack of foreshortened linear dimensions can be understood by reading ASME Y14.5M-1994 paragraph 1.8.2.2.  This paragraph established the foreshortening of radii.  Its title Foreshortened Radii seems to preclude these methods for linear dimensions.  But why?

The clue is the intent.  1.8.2.2. states that if the center of a radius is outside the drawing or interferes with another view, the radius dimension may be foreshortened.  Strangely enough, paragraph 1.8.2.2 does not specifically describe the just how foreshortening is demonstrated, other than to say the dimension line is radial to the arc.  It does reference a figure that shows radii centers repositioned with zigzagged radial and coordinate dimension lines.  The key is that the center of the radius is still within view.  The dimensions have known termination at both ends.

Allowed foreshortening of radial dimensions

There is an issue with using this methodology on any dimensions where the termination of both ends is not clearly shown.  Without both ends of the dimension in view (or known through some other way), there is no established way to determine where the dimension’s open end terminates.  It is an incomplete specification.  In other words, if I have a detail view and attempt to dimension to a feature not in that detail, the fabricator does not know the location of the other end of that dimension.  SOLIDWORKS previous limitation was not really a limitation after all.  It follows the drafting standards in a very logical way.

Disallowed foreshortening and diameter forshortening

Another thing SOLIDWORKS allows is the foreshortening of diameters.  Although this is not directly supported by the standards, it is common practice.  Unlike the foreshortening of linear dimensions, foreshortened diameters make sense since the other end of the dimension is known, even if it is not shown.  I’ll address foreshortened diameters in more detail a future article.

As of SOLIDWORKS 2016, foreshorten of linear dimensions is supported without restriction.  This was added for customers who still need methods to clip dimensions regardless to the issues mentioned above.