There are a few ways to do it. One is to make the section big enough to see both sides, place the dimension, then shrink the section back. Anothe is to place the dimension into the original view, then ctrl-drag or shift-drag into the section view. Depending on whether you use control or shift, the type of section, the current phase of the moon, your height, and a few other parameters, you may or may not be able to right click and set it to be foreshortened.
Is this broken in Solidworks 2013 too? I can't get the dimension to drag while holding shift or control. Varying applied force to keys and/or buttons does not seem to change the results.
I tried using the oversized section trick. A dimension was produced. But it seems that the leader must be pointing toward center line. I can't seem to keep a single leader and have it point from center line to the diameter. And forget about a double-headed leader pointing to a centerline that is not there.
It doesn't work in 2013 either (as far as I know). I tried Mike Pogue's suggestions but with no sucess. I challenge anyone who knows how to do this post a sample part drawing showing this accomplished. For those of us that work with large round ring parts this can be fustrating because the best way is to always use cropped section view and put the diameter dimension there.
I just started using Solidworks for the first time last week.
I could really use, and would really appreciate, a step by step instruction list explaining how to do this properly. The manufacturing operation sheets that I have been tasked with will at least have a chance at being a little less confusing.
Edit: Thanks Mike for the response.
Here is how you can dimension your bolt circle dia.
in front plane draw your flange OD, ID and centerline for a boss/base revolve operation and draw you B.C. Dia. in construction lines
finish your model drilling ect.
create new drawing show top view (drilling)
create your section view
find the section view in the feature tree list and find the original sketch with your B.C. Dia. in construction lines
select sketch -----right click show.
Dimension B.C. Dia.
then Hide the above sketch
select your dimension---- right click select hide dimension line do this two times
Note you will have to draw in your centerline in section view
ps using 2013 x 64 edition SP3.0
If the dimension exists on the model, it can be inserted as a model item either the section view or the parent view and dragged over to the seciton view by holding down the shift key. Linear dimesnions for diameters/radii that are inserted model items are the only type of linear dimensions that are automatically foreshortened in cropped/detail/section views. If you find that you need expanded dimension foreshortening functionality, you can vote for an existing Enhancement Request in your Customer Portal. This will help us determine the importance of this type of functionality in consideration for future enhancements for SolidWorks.
Dragging and dropping dimensions in a drawing can be tricky. Here is what I have learned about it, just click on the drawing view, insert, model items,(make sure in the dialog box it says the correct drawing view) and do a ctrl drag or shift drag over. There is a little more complication to it that just clicking and dragging it also depends on where your original sketch is in relevance to the drawing view. If you were to draw your sketch for the model on X plane and your drawing view is showing it on Y plane then you will have to have the section view where the sketch is in order for it to import the model items correctly (not all the time). This rule I have found out also applies to detailed views, but with detailed views you always have to keep it relative to the detail circle for ex: if you draw a detail view on the top right side of the part keep the drawing view on the top right until you are done dragging your dimensions then you can move the view wherever you please. The main key is making sure your details and sections are located on the same planes(or area) as your sketch for your model for this to work nicely (you can have them off the sketch and sometimes it still works but just not as well). If you cannot put them on the same plane then do as directed above and drag the line past where you want import or drag your dimensions and then drag it back up ex: if you drew a sketch and dimensioned it from the right plane then you have you view on the top you should be able to drag the detail or section view just past half way of the part and make sure you drag the dimension in the same corresponding spot on the detail or section view(this makes a difference). Always make sure that where your dragging your dimension in a drawing it is near the spot it was dimensioned from on the sketch for the best results. Again this is what I have found works best for what you are trying to achieve it always helps to always make your sketches in thought of how your going to view it on your drawing (if you like to import your models and drag drop them which i highly believe in). Dragging and dropping will also give you the desired jog looking line for your diameter.
Message was edited by: Raul Bueno