I am not able to insert model items into a drawing file, and the problem it related to this topic (see here). It was not a problem to insert model items in SW2007 (currently using SW 2009 SP 5.0 Win XP x64).
I have tried selecting the sketch / feature when inserting model items from the model tree without success. Even importing the entire model does not bring in the dimension. Is this another bug, or is it a document setting issue?
SolidworksDrawings And Detailing
Are you trying to apply the dimensions to a section?
Is the section line in front of, or behind, the location of the sketch?
No, I am not trying to apply the dimension to a section. I have also tried to insert the model item by selecting directly from the feature or sketch in the model tree. This does not work either, or does importing the dimensions from the entire model.
Can you reproduce the problem on a new part?
Can you ZIP and post the part and drawing for testing on other machines?
Chris,
Can we assume the dimensions in your model are "Marked for Drawing"?
I have attached an example of the problem I have had when attempting to insert model items into the drawing (SW2009 x64 Edition). Although most of the dimensions are inserting, I cannot get the overall length to insert, which is the first item in the model tree. There maybe other dimensions as well that are not inserting.
I also do work in Pro/Engineer, but most of my time is in design of parts / assemblies and not detailing, so I could be overlooking something that is a simple fix, or it could be a bug.
It's because the sketch containing the length dimension is outside of the Sheet Metal features.
If a Blind length is used (instead of the Up to Vertex), the dimension is included in the Insert > Model Items.
Kevin,
You were correct about the using a blind length to get the dimension to insert into the drawing. However, as I needed the overall lenght (part is mirrored) to be the driving dimension, I came up with a trick.
The solution was to create a sketch of the perimeter as a surface feature (planar) so the length dimension of 26" could be inserted into the drawing as a model item, than use a "delete body" feature to remove the surface reference surface. If the part is a fully developed with dozens of features, then this is a quick work around instead of remodeling the part.
Lastly, why are sketch dimensions not permited to be inserted directly into the drawing (without attached feature)? There are times when it would be helpful to have layout sketch dimensions appear in the drawing, and I believe I can do this in Pro-E (Pro/Engineer).