This has been a pain in the rear end for as long as I can remember... however there are a number of ways in which a sneeky CAD person can fix such an issue.
1) A direct approach would be to create a note in the drawing and type in the following...
Obviously 'CirPattern1' should be replaced with the name of the feature and 'Part1' should be replaced with the filename of the part model. Make sure the address is correct then add a speech mark " before and after the address. If typed in properly the address will be replaced with the referenced dimension. However... keep in mind that like all dimensions reference in notes if you change the name of the feature or the filename of the model... THE DIMENSION WILL NO LONGER BE REFERENCED... however if you change the names back then it will reestablish the link.
2) An indirect approach would be to create a property in the part file which references the dimension...
Obviously 'CirPattern1' should be replaced with the name of the feature. Also add a speech mark " before and after the address. Name the property appropriatly and set the type to 'Text'. This can then be inserted into a note in the drawing. It will update but any tolerance information will be lost in the transfer. To include tolerance info would take some additional coding which may or may not be possible. Ive not looked into that one much myself.
3) A nice indirect route if you dont mind an additional sketch in the part model.
Before creating the pattern you can create a sketch, perpendicular to the pattern axis, with two lines in it eminating from the axis. One line should be set to the direction of where the first feature to pattern is and the second should have an angle dimension off of line one. Now create your pattern and then an equation. The equation should use the angle from the sketch to drive the angle in the pattern. The dimension in the sketch can then be imported into the drawing. This dimension will update and will allow the pattern to be driven by the drawing. It will also allow transfer of tolerance... as long as you tolerance the free sketch and not the pattern.
The equation could be setup the other way which would allow the pattern to drive the sketch... but really thats just daft.
4) Another way is to go into the drawing, create a section view cutting through the pattern, create centre lines between the FIRST and SECOND element in the feature. Then dimension that. You can then if you want create a note and click on that dimension to insert it into the note, then you can hide the section and section line. YOU NEED TO MAKE SURE however that the dimension is created using the FIRST AND SECOND ELEMENT OF THE PATTERN or else it will not update... instead it will loose connection.
5) Type it in a note.. but I dont recommend that one!
Hope this helps!