How to save a particular Assembly configuration view and put it on a drawing?

I'm going to take back what I said below. There is nothing like doing it to know what -not- to do

I find it absolutely impossible to drive mechanism assembly relations with family tables (pin). You cannot get to, for instance, the angle dimension in a pin constraint to populate the family table that I can see easily. However, if I use a conventional constraint system, like planer/axial coincident and then an angle between planes, I can pick up that dimension in a family table by simply clicking on it. I don't know what PTC is thinking here and I'm sure there is a way to drive this... probably with relations... which create other limitations in flexible components.

So for your question, I created family table instances in the assembly model. I constrained the movable side of the "book" with a plane for translation, the axis for the hinge, and an angle for the page. I created two family table instances in order to vary the "angle" dimension of the angle constraint. One at 170 and another at 5. I now create the drawing with a model which uses the instance with the 5 degrees setting, and I also Add the model as an instance of the 170 degrees setting. Now the drawing has 2 models which are simply instances of the "original".

You make one of the models active in the model tree. You then place the view. It will be of the orientation you choose for that instance. Next I activate the other instance. I again place a view a drawing and now the book is the alternate instance. I can then manipulate each view independently and I can even give them an alignment with view properties.

Flexible models will not help in this instance. This would only be helpful if you have 2 levels of assembly for which there is no need from what I see in the original post.

What version of Creo/WF/Pro-E are you using... and is it an academic version? I can provide an example if you have the full version of Creo 2.0.

There are a number of ways but I recommend assembling the "book" twice and making the second a flexible component where you change the 180 degree angle to another angle. Only the flexible part will change.

I will warn you, however, that accessing that parameter and making it flexible may not be as simple as it might appear at 1st glance. It is not quite as simple as changing a feature's dimension value, although it should be.

If this isn't working for you, you can also look at family tables. In that case, you might have a similar problem accessing the value, and then you might try a more conventional angle constraint rather than the pin. Again, your drawing would have multiple instances of the part; one open, one closed.

I'll have to try it to see exactly how it is done. I just remember that assembly constraint dimensions are harder to get at than feature dimensions.

Let me know if you are not having any luck with either and I can see what we can do.