When adding dimensions to a drawing, the dimension lines disappear. This is only happening in this one detail. See picture.
What version of SW are you on?
I'm using SW 2016 SP 2.0.
I have seen this before with 2016. I believe it's been reported to SW but can't find the exact SPR. Is it just this file it is happening with? Have you phoned your VAR to report?
Just this file. I have not phoned my VAR yet as I have a deadline looming. Thanks.
is this a "model dimension" or a "smart dimension" placed on the drawing.
This is with a smart dimension. I have now run into it in two separate drawings. It only appears when I'm using smart dimensions in a detail drawing view (Insert>>Drawing View>>Detail).
I had the same problem so, I have contacted my VAR and this is what I got...
This is a known regression from 2015 SP5 which was reported in SPR 916189 'Extension line is missing in detail view, when adding the dimension by Model Items or Smart command.'
I am happy to report that it has been implemented in the latest development build of SW 2016 SP4 which will be released in late June.
1. Expand detail view boundaries to cover the entire part. This 'adds' the missing extension line back.
2. Shrink detail view boundaries to its desired size ( i.e. 'cut' the component again). The extension line remains .
I'm having the same issue with SW2016 SP5. I create a detail view 2x the size of the parent view, create a centerline from two parallel edges in the detail view and then dimension from this centerline. No matter what I do, one of the extension lines will not display unless the dimension is placed on the opposite end of the centerline that I want it to be on. Attempting to move the anchor point, move the view to another sheet, etc. all do not work. If this was covered in SW2016 SP4, apparently they did not migrate the fix with SP5!
I'm seeing the same thing. Could it be the scale of the detail versus dimension scale?
Do you have dimensions assigned to a layer that is turned off?
Is it a Model Item sketch? In other words, is this the sketch dimension used to create the feature and you're importing it into your drawing. If yes, it appears that the dimension is attached to something that is cut-off in your detail view.
If you drag the dimension a long distance off the view does the extension line appear?
I've had that happen in the past and have worked around it by picking different features. First screenshot shows how I would normally dimension (pick the component [one blue line], single click) and the second screenshot shows the workaround (picking two different edges [two blue lines])
I'm running 2016 SP4 btw ...
Good suggestion John. Sometimes picking an intersection point works as well.
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