Replace Model Reference - inventor 2014

[MBeerman]

I was re drawing all of our previous drawing to make the all similar when I hit a really annoying snag. I tried to use  the  replace model  in a drawing and all of the dimensions just disappear. I don’t know if there is a setting that is different but if you take a look at my screen shots you can see what is going on. I can replace the inside Box view, and all the dimensions stay the same… that great but as soon as I try to change the assembly view all of the dimensions disappear. Why can’t they just stay on the drawing so I can reattach them? The only thing that is changing is the height of the box. They are oriented the same way and they are on the same plans.

[mrattray]

[MBeerman]

Thanks

That solves part of the problem but why does it not recognize were the dimensions are it is really not that different.

[rdyson · Accepted solution]

This might help:

[LT.Rusty · Accepted solution]

Most of the time this happens because the geometry is created by a different feature. If you take your model and save as with a different file name, then change a few dimensions in a sketch, and then use Replace Model Reference, your dimensions will almost always (99.999999% of the time) come through with no problems. The issue comes up though if you have a model that is not related to the old one, or if you are using different features to make the similar geometry. For instance, let's say you have a metal plate with some holes in it, and you want to move those holes around to different locations, and you want to chamfer the edges of the plate. A dimension on the outside of your plate will get lost, because the edge that was used to create it depended on, say, Extrusion1, and when you added the chamfer feature, that edge no longer existed. Therefore, Inventor doesn't know where to put that dimension, even though the model is still - in your words - "really not that different." As for the holes, if you go in and edit the sketch that locates the holes, then there's no problems - the dimensions in the drawing will stay just fine. If you delete Hole1 and use a new sketch to create Hole2, though, you'll need to either create new dimensions in the drawing or attach them in the new location.

[mrattray]

In addition to L.T.'s comments, I'll chip in that assemblies add an additional level obfuscation. Even the same exact part if placed into a new assembly will be seen as "different" to Inventor. For example, if you use the "demote" tool to create a new assembly and then use the "replace model reference" command to swap the parent assembly out for the demoted one, Inventor will see it as "different" even though it is, to your practical eye, not.

[Curtis_Waguespack]

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@MBeerman wrote:
... but why does it not recognize were the dimensions are it is really not that different.

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Hi MBeerman,

Just to add to what LT.Rusty and mrattray have said, when you place a part file in as assembly and select the top face of the part, from a programming standpoint you're not really selecting the face of the part. Instead you're selecting proxy geometry representing that part face, This proxy geometry is created at the assembly level to represent the top face of the part.

Why do we need proxy geometry of the part's top face in the assembly, rather than just using the part's actual geometry you might ask?

Well what if you were to place 2 instances of the same part file into the assembly? How are the two top faces (the one on the first instance of the part, and the one on the second instance) going to be told apart?

There's a bit more to it than my short explanation covers, but that should give you an idea of what's in play here.

I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com