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.