23 Replies Latest reply on Jun 1, 2018 3:54 PM by Henk Bruijn De

    Foreshortened Diameter Dimension

    Jay Johnson

      How do you add a forshortened dimension in a detail view? I've been looking through the help files on how to do it but can't manage to get it done. Instructions say "

      If you move a diameter dimension into a view where it does not fit, it is foreshortened." How do you move a dimension into a view? Already spent too much time trying to figure this out on my own. I need someone to tell me how to do it.

        • Re: Foreshortened Diameter Dimension
          Don Vanzile

          Tony Cantrell's method is the method that worked in this thread. (Make a tempory full view of the diamter dimension, then hold the ALT key down while selecting that dimension and drag into the detail view.  It would automatically foreshorten the dimension.)




          But for the life of me I can't get this to work now in 2010 or 2011.... Anybody know what happened to this?

            • Re: Foreshortened Diameter Dimension
              Jay Johnson

              This isn't only for diameters. I've also come across a drawing that uses a foreshortned dimension line for a length that has been cut off in a view. I fudged it by using a note with a leader but it is very time consuming trying to get the leaders horizontal. Also couldn't choose a double arrow so I had to put one leader on top of the other but offset to either side. They want to snap together, which eliminates one of them. I hope there is a fix for this. Maybe I'll get lucky and it'll be something included in 2011.

              • Re: Foreshortened Diameter Dimension
                Jeremy Feist

                holding the shift key shifts the dim to the new view (have to release the mouse button within the view boundary) and holding control will copy the dim to the new view.

                  • Re: Foreshortened Diameter Dimension
                    Jay Johnson

                    I think one other issue that is involved is that my model is an imported .iges file in which I saved it to a .sldprt file. Since it does not have the features included in the model, will it still find the dimensions?

                      • Re: Foreshortened Diameter Dimension
                        Charles Culp



                        You can dimension imported geometry just like native geometry, as long as it is a clean import. If the sides "look" flat, but are slightly un-flat, that can cause issues.


                        As per your original question... Create the view and dimension the full diameter or distance. This may require you to temporarily make the detail view larger (expand the circle to include everything), or whatever you are doing. Then you can resize it back down to the size you want on the drawing.


                        Then, after de-selecting the dimension tool, right click on the extension line, and select Hide Extension Line. You cannot change it to a double arrow, but you can hide the dimension line as well, by right clicking on it and selecting Hide Dimension Line.

                          • Re: Foreshortened Diameter Dimension
                            Jay Andrews


                            The article linked here does not seem to show what I am trying to do.  I'm trying to show foreshortened diameters in detail b.  I DID try increasing the detail circle to show the entire view then reduce it, didn't work any way I tried.  The 2.130 dim was just selecting the edge, and when I copied it over, it shows to scale, but doesn't show foreshortened.  The 2.192 dim, I selected the two edges to create, and if i copy one like that over to the detail, it puts the arrows 0 apart but with the correct dim value, and if I try to drag it, it changes to 0.000.  So nothing is seeming to work correctly here.


                            Is it possible to foreshorten a diameter looking from the side like this?  Is my problem user error?

                              • Re: Foreshortened Diameter Dimension
                                Jay Andrews


                                hmmm now I've gotten it to work for edge to edge dimension diameters, but not point to point diameters, like the leading edge of a taper wont work for me.  This is no good in this case, because it's specifically the point to point dimensions I'm trying to show forshortened.  BTW, they do come in as natural diameter dimensions in the original view before I try to move them over.  Bug or user error?

                                  • Re: Foreshortened Diameter Dimension
                                    Jay Andrews

                                    Just to share the portion that I have figured out on this issue...


                                    I made a second body in that part to dimension to edges at those points, then hide the bodies(hmm that's gotta flag the patriot act computers...)


                                    Anyway, so the first dimension moved(actually copied) over foreshortened no problem, no matter how many times or ways I tried it (didn't even have to enlarge the detail circle, it just popped in correctly foreshortened). The second would not move or copy properly, no matter how many times I tried.  So I erased the bad source dimension and redimensioned it.  Well then it copied over correctly.


                                    So my incompleted conclusion to share here is that it is the source dimension that seems to be afflicted with whatever the bug is.  So if it won't copy over, don't try over and over to copy that dimension, but delete and redimension in the source view, then try moving over the new source dimension, and repeat until it works properly.


                                    There may be a trick to create the good source dimension, but I haven't figured that part out yet.  I have to say it does work very nicely, when it works!

                                • Re: Foreshortened Diameter Dimension
                                  Michael Dewey



                                  This seems to work as a work around.  Is there a way to get a double-headed arrow yet? (sorry for the 2 year old thread revival)


                                  Edit:  Thanks for the link Paul (below).  I should have been more specific:  Is there a way to get a double-headed arrow in a section view and in a detail view yet?

                          • Re: Foreshortened Diameter Dimension
                            Brett Nagel

                            I've figured a few things out with regards to creating point-to-point foreshortened diameter dimensions in a detail view. I, too, was struggling with this for far too long! Here's how to add foreshortened poin-to-point diameters in a detail view.


                            Model Definition:

                            It starts with they way you define your model. I find it easiest to create a revolved boss/base feature with a sketch that contains a centerline with diametrical dimensions. THIS PART IS IMPORTANT! You need to define your sketch using the poin-to-point diameters you'd like to display in your drawing. Next, right click on the dimension you've just created and click "Mark for Drawing". Continue with your model until you're ready for the drawing.


                            Drawing Definition:

                            Insert your parent view for which you'd like to create your detail view. Create your detail. Next you will need to insert model items into the parent view, making sure you insert dimensions marked for drawing. You should now see all your "Marked for drawing" dimensions, including your point-to-point diameters. Next, while holding down the SHIFT key, drag those dimensions onto your detail view. Next, raise your hands in the air and yell "He shoots, he scores!". (NOTE: Last step not necessary, but highly recommended)


                            This worked for me! Hope this helps everyone. I still feel like the foreshortened dimension functionality is still buggy...

                            • Re: Foreshortened Diameter Dimension
                              Brian Guth

                              The best example that I have found on how to do this was through a video created by Javelin.  The first URL is to their page with photos showing how to do this.  The second URL is to their video actually walking you through the process in real time (the video link is also the last "image" on the page).  The only limitation that I have found is that you cannot get foreshortened dimensions to features that are only on one side of a part.  (i.e.  A boss or protrusion that is on only one side of a cylindrical feature.)  It will still give you a linear dimension that reflects the radius.  I hope that this helps!





                              • Re: Foreshortened Diameter Dimension
                                Matthew Lorono

                                SW2016 now supports foreshortened linear dimensions in detail view, crop views and also via the right-click menu for dimensions in any view type.

                                • Re: Foreshortened Diameter Dimension
                                  Henk Bruijn De

                                  Foreshortened diameters are possible in SW2018 Drawings, but is a PITA.

                                  I do not know for sure if foreshortened dimensions were fully supported in earlier SW-versions.

                                  First of all; the diameter dimension must be present in the model, driving or driven.

                                  If it is not in the model you can add it as a driven dimension.

                                  I'll explain further with an example of a small groove detail in a large flange;

                                  From left to right: front view, half section-view and detail-view.

                                  The half-section view is in "Hidden Lines Visible" mode

                                  The groove has ID of 1500mm, depth of 10mm, width of 30mm.

                                  To create the 1500mm dimension to appear foreshortened in the detail view, do following steps..


                                  1) Import all dimensions in the Front-view by: clicking on the icon “Model items” ;

                                  Source = Entire model,

                                  Destination view(s) = Front view,

                                  Dimensions = Marked for drawing + Not marked for drawing,

                                  Eliminate duplicates = checked

                                  Click   OK

                                  2) Delete all unneccesary imported dimensions in the Front-view.

                                  3) Now you can CTRL+drag the dimension of 1500mm to  the Detail-View, and also to the Half-section view if you like.

                                  4) In the Detail-View RMB on the 1500mm dimension => “Display options” => “Foreshortened”.

                                         (If you CTRL+drag the 1500mm dimension from the Half-section view directly to the Detail-view, the dimension is automatically foreshortened)

                                  Now you should have this as a result:

                                  The 1500mm dimension is foreshortened, but it has no zig-zag leader.

                                  I do not know why, but Solidworks 2018 does not allow zig-zag leaders for most Drawing standards.

                                  If you want zig-zag leaders do following additional steps.

                                  5) Tools => Options => dimensions => Linear =>

                                  6) Change the “Base linear dimension standard” to ANSI.

                                  7) Now you can uncheck "Automatic" and select the zig-zag leader.

                                  8) Switch to your Drawing and the result should be:


                                  I wish Solidworks could make this "simple" feature much easier.