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.Â 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.Â As such, they are not supported by the ASME standard.Â 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.Â Jeff’s creation requires a modification to your gtol.sym file.Â 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.Â 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.Â Another drawback is that the user must visually and manually align the double arrows into the appropriate position.
Barring these drawbacks, this is a pretty good solution for those who really need this function.Â The file can be downloaded at this location:Â Geometric Tolerancing Symbols Library Foreshorten Arrows Add-on.Â Instructions on how to edit the gtol.sym file and use the new symbols are included in the download.Â Have fun!
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.
Foreshortening a radius dimension on a drawingÂ is easy.Â The option to foreshorten a radius is found when the radius dimension is highlighted by looking under the heading of Display Options in the PropertiesManager pane.Â (Note: this foreshortening option will not be available if dimensioning a full diameter within the view current view, even if the dimension is shown as a radius.)Â Â Â Once this option is chosen, the radius dimension will appear foreshortened with a zigzag radial line.Â The user can then adjust the shape and location of the zigzags, as desired.
This is easy enough.Â I am covering this basic how-to tip as a lead-in for the more complicated task of foreshortening diameter dimension in an upcoming article.
[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 126.96.36.199. 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. 188.8.131.52. 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 184.108.40.206 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.
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.
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.