First off, let's start with the design table way. The easiest way to get there is to create two configs with everything different that you can foresee as being different among your configs. Then insert the table and let it auto-create - this will populate it with all the differences. Now open that DT in an external window and set up all your configs. Close out and you have a part file with all the configs controlled by the DT. Then for the drawing, pick a config, detail it, and save the drawing. Make sure you save it! Now do a save-as on the drawing, giving it the name of the next config, so you are now in the new drawing. Edit the properties of the drawing view and change to the proper config. Clean up as necessary.
But if you have individual part files, it's a bit different. For the drawing, pick a model file, detail it, save the drawing, and close it. Now do a File/open, select that drawing, but don't open it yet. In the lower RH corner you will see a button labeled References - click that to bring up the dialog. Double-click on the name of model file and browse/select the next one. Finish opening the drawing, clean up the dims if necessary, save, and then repeat.
Thanks for this, I have recently moved from Solid Edge and couldn't figure out how to do this.
in addition you can right click on a dimension and say "configure dimension"... this brings up a table where you can add configurations and the differences for that dimension. The next dimension you configure will list the configs you have already created and you can update the values for that dimension. It is like building your design table but without using a design table to build the configs. I have done this and left it out of a design table and also done as Wayne says to then auto-create a design table after this (just gets you a little further along)
PS: there is also a "configure feature" for suppression states between configs
From the open file window you can click on the references button in the lower RH corner.
This opens a window with all the file references. Double click on the file and you can go and select a new file. Close the window(s) and immediately open the drawing.
The drawback is that the new file must have all the same features etc or the dimensions will become dangling.
I have used this method but I much prefer the design table route.
You could also look at doing this through Solidworks explorer.