Manage drawings generated by Intent

[MarkBrouwersIntent]

Hi,

First of all ,a happy newyear and good health to everyone  !

I've got a question regarding drawings generated by Intent . 

When I add some annotation to a drawing, I loose them a soon as the drawing gets regenerated when rules change. Is there a way, besides adding annotation through intent rules, to keep these annotations.

I'm thinking of following workflow : sales creates a model and makes drawing(s), complete with all of the dimensions/annotations/remarkes. Then the customer wants some alterations which makes the rules to change. which results in a new drawing, meaning I loose all of my work completing the drawing. Is there a way that makes me retain all of these manualy annotations ?

I use a application that allows CAD-unaware employees to generate a Inventor model. I've created functions within this app to place dimensions by allowing the user to select some geometry in the drawing. But  nothing ensures me that this geometry will still be present when some rules change and therefore breaking my model by generating errors. How can I intervene in a child rule when a required parameter is not valid anymore (can this be done with try...catch).

 What is the correct way of working ?

Cheers,

Mark

[JackGregory · Accepted solution]

This is a topic that often confuses people.  It is a complicated topic in the Inventor API and driving drawings via rules is even more problematic, because of the naming problem.

First, when Intent/ETO is creating a drawing, and a change is made that will invalidate a view, Intent throws the old view away and re-creates a new one.  This is why your non-Intent annotation "disappears".  Intent knows nothing about it.  The solution is to "Adopt into Intent", which is a right-click menu item on the dimension after you create it.  Then Intent will know about it and re-create it when the view is re-generated.  We would love to be able to just keep the old view and regenerate just our stuff (much like an assembly works), but the Inventor API just doesn't let us do that.

But now if you have adopted the dimension, Intent can only go by the example it was given to create the rules.  These typically point to some curve entity, which is the projection of a model edge (usually, silhouette and section cut edges are more complicated), and Inventor isn't consistent about which of potentially many edges it selects to show in the view.  The next time the view updates, we could get an entirely different edge, and the one our rules are referencing is not present, and the dimension will fail.  This is called the naming problem.  Rules need to identify everything they deal with, and CAD systems typically don't name everything, or keep names through changes.  So the typical solution is to reference a known point instead, typically a workPoint or some other thing that will not disappear.

The bottom line?  Rule-based drawings are very difficult, for you and us.  We strive to do the best we can with what we are given.

All of the above doesn't really address your workflow question, but at least it shows why it is going to be a problem.  Other customers may have some ideas on how to maintain manual changes, but ETO out of the box cannot.

[Lesoux]

I think you need to design factory file what you use in Intent such that cover all possible configuration your future part/asm. Add entity names on edges, faces and vertices as many as possible. Add working points and axises as well, it will help you avoid some issues in the future. It's not easy and you can spend a lot time, but result will be awesome.