How can I add a linear Foreshortened dimension in a detailed view?
let's say between A and B :
At present I select Smart Dimension tool and select A point in detail view and then select B face and place the dimension.
then right click the right extension line and select Hide Extension line.
then right click Dimension line and select Hide Dimension line.
I was looking for a simpler way ( if any) and possibly having the Foreshortened Diameter appearance.
thank you
John, I'm on SW 2017 SP0.
Here's what I have:
I don't know why the selection of Foreshortened is grayed out?
Do you have any idea?
In my case no matter I right click the leader or the extension line or the text, the context menu is the same.
any further help is much appreciated.
thanks
Not sure if your question was resolved. But I'm haveing the same problem. I'm on 2016 sp5. The drawing I'm editing has foreshorten dimension on it. If you right click to foreshorten dimension, foreshorten will show up in the Options. But if I add new dimension I can't get it to work. I tested it on another computer that doesn't have SP5. It worked fine on it. Is there a way to this manually? or something?
Looks like he has the 'text position' set to in the middle vs. yours is set to over the dimension line. That may be why it can't foreshorten it.
We are having the same problem John Pesaturo mentions . Foreshortening is working in 2016 up to SP 3, but disappears for detail views in SP 5 (for example). Anyone have a work around? Oddly, it works in other views like section views, etc, but not detail views...
Please make sure to report this to your VAR. Dimensions should not be disappearing, even if functionality was removed (which is wasn't, so this is possibly two bugs from one issue).
I'm not sure if there is a bug, but one thing you can check is that foreshortening should be automatically applied when creating a dimension by selecting a feature in the detail view and then a feature that only appears in the parent view. To manually set a dimension to foreshortened, you'll need to RMB click on the side of the dimension line you wish to "remove/hide".
This may be a left field answer to the issue but is it possible that your dimension is not to a diameter or radius? I am using 2015 and it appears as though foreshorten display option is only available when dimensioning to a diameter or radius.
Foreshortening of any linear dimensions was added in SW16. There are different display methods for the dimensions based on the standard since ISO based standards handle foreshortened dimensions differently than ASME.
How to dimension the center after foreshortening the arc dia or radius? In this case is it possible to dimension the center (after foreshortening) to an edge of the box?
To the best of my knowledge a dimension from selecting two entities,points, intersections, etc can not be made into a linear foreshortened dimension. a single selection line dimension automatically foreshortens.
Upon trying what Matthew suggests making a selection in a detail view and a selection in the main view it will create a linear foreshortened dimension however if the detail view is pulled from a section view the dimension doesn't happen.
Roger, thank you for the feedback. If this is not happening in conjunction with section views and detail views then it looks like you are experiencing unexpected behavior that should be reported to your VAR for further processing.
Habib, What version and service pack are you on? I'm on SW 2016 SP3.0 and it seems to work fine. Someone else was having the same problem as you are just yesterday but with foreshortened diameters not working properly but he was on SP5.0 if I recall.
Regardless, the same answers apply ... It should work the way you've described. If the settings are different on your machine you may have to do it manually, but it should be as simple as right clicking the leader and selecting the "Foreshorten" option. Just note you can't select the text or the extension lines as those selections will not give you the foreshorten option.