Solidworks 2003 dimensioning help please

SW won't do this for you. I finally got his idea after seeing your fourth post:

1-Dimension to the corners you're trying to get. Place the dimension somewhere out of the way. 2-Right-click on the view, and lock focus on the view. 3-Sketch bent extension lines the way you want them to appear. If you use an angle dimension to control the bend, you can hide it. Right click on the dimension and select hide. 4-Place a dimension in the position you want your final dimension to be. This will only control the space between your extension lines. 5-Edit the text of this last dimension. Replace with several spaces. 6-Create a note on the drawing view. Click on the first dimension to link it's value into the note. 7-Drag the note into the blank space between the arrows of the last dimension.

This looks like a bug report. Too much time with the beta I suppose.

As a refinement, select the end of the sketched extension line when yo ucreate the note. This will create a note with a leader. Ignore the leader until you have the dimension linked into it. Then go to the note properties and turn off the leader. Drag it into position. Now the note holding the dimension number will move with the extension line if you make any changes.

There is another way to do this: as your angle is very small, why don't you create a detail view of the area and dimension that?

To create a 'shortened' dimension on the detail view you will need to select the bottom edge of the tappered bore (not the sides), this will create the dimension, you then RMB on the dim and make sure that the dim is NOT centred so you can drag it close to the detail view, then RMB on the dim again and select the display tab in the dialogue box and hide either the first or second extension line & dimension line. This should give you an acceptable dimension display that clearly shows what you are dimensioning to.

Merry :-)