Sometimes I can make the value of a Sketch offset be driven by neighboring geometry, and sometimes I cannot. Why?
In the earliest versions of Solidworks, the command to Offset a sketch line
would only create a single, parametric relation. If you deleted the offset
dimension, you had also deleted the relation. But now a Sketch Offset can create
two relations - One Parametric relation that holds the dimension value, and one
Geometric relation that refers back to the original line(s). So, If you now delete
the Offset dimension, the geometric relation will still hold true, and you can then
drag the offset line(s) thru a range of positions that are all still parallel to the
originals. This is great for doing top-down design, because it means that the value
of the offset distance can be driven by relations other geometry.
This new Geometric flavor of the Offset relation is bi-directional. It can push
from the original lines TO the children lines - OR, if you constrain the children
lines somehow, they can push backwards on the parents. This is powerful, but it is
the source on an interesting limitation. It only works if the Parent lines are
native to the currently active Sketch. If you are trying to offset existing model
edges, for example, then you will only get the numeric Offset parameter, not the
newer geometric relation. This is because none of the sketch relations can 'push
back' on the 3D model geometry directly.
To overcome this limitation, identify all the model edges you wish to offset, and
instead do a CONVERT ENTITIES to get them copied as local lines in the current
sketch. Then you change these lines to construction elements, select them again,
and perform the sketch OFFSET command. Because the 'parent' lines are now local,
you will get the newer, smarter Geometric offset relation as well as the (optional)
Parametric offset distance. This is also why, if you try to offset model edges directly,
the “Add Dimensions” check box will be greyed out in the Offset dialog. But if you
first CONVERT the model edges into the sketch, and then OFFSET them, the
“Add Dimensions” option is active.
