What does this Assembly Message Mean?

[Cadmanto]

For what ever reason this message comes up when I have the associated drawing open

at the same time as the assembly.  It locks me from doing anything in the assembly?

Can someone please explain what this message means and how I can prevent it?

Thanks

Scott

[andrewiv]

It means that the iam you are viewing is in a different level of detail as the idw view.  Switch one or the other to match and you should be able to save.  Another option is to just close either file and you can save the one that's left open.

[Cadmanto]

I have been closing one of the files to get this to work.

But that is crazy.  I see what the message says and that the idw view is different,

but what does that mean in the bigger picture?  Why is the software not updating accross the

lines between the parametric files?  Isn't that what being parametric means?  When one file changes the other

one updates as well? 

How do you make them match? 

[andrewiv]

I understand, I've always thought that this is not the way it should work but we have to live with it the way it is.  To make them match you have to edit the drawing view to see which level of detail is being used and make it match the level of detail that is open in the assembly.  I usually like to use the master level of detail for everything, unless the file gets to be really big.

[jtylerbc]

Cadmanto,

Levels of Detail have some screwy behaviors, so I generally avoid using them unless I really need to.  What are you using them to do?  There may be a better way that lets you avoid the problem entirely.

[Cadmanto]

Ok,mine look the same as what you have shown.  Now what?

Are you telling me that if I change the hidden line viewing of individual components

in the drawing view it will not so called "match" the assembly and thus not allow me

to save the assembly unless I close it?

If that is the case that is just plain wrong!!!!!

[andrewiv]

It's got nothing to do with hidden lines, it's suppressing components to free up memory for large assemblies.  One other thing is that you have to make sure all views in the idw are using the same level of detail.

[jtylerbc]

Hidden lines and LOD's are completely unrelated.  The part of his screen shots you need to be looking at is the circled area referring to Levels of Detail.

If any of the drawing views are referencing an LOD that is different from the one you're using in the assembly, you will start getting the error message you described.  Levels of Detail are used to remove unnecessary components from memory, to improve computer performance.  By having two different ones referenced in open documents at the same time, you're telling Inventor to load and unload those components from memory at the same time, which confuses it.

[Martin_Goodland]

You should not be using LOD to define the drawing views. In the assembly model right click on the LOD in the browser tree and select 'Copy to View Rep'. In your drawing use the view representation to define the drawing view. If you tick the link box in the top right corner the drawing will update as you alter the assembly state for that representation, if you leave it unticked you will need to re apply the view rep to see the changes in visability. Leave LOD set to Master in the drawing view.

LOD is for memory management, so if your model has lots of parts in it but you don't want to work on them you can use a LOD to unload them from memory. As a LOD unloads components from physical memory (RAM) you can not have more than one active at a time, as one will try and load files back into memory that the other one will want to remove again.

These days with cheep RAM and standard PC's that can hold 24GB without issue LOD is not as big an issue as the days when everyone was on 32bit machines.

Regards

Martin

[Cadmanto]

Martin,

Thank you.  I tried RCing on the LOD in the assembly and "Copy to view rep" is not a selection.

[andrewiv]

You are in the master LOD in the assembly, which is where you want to be and that one cannot be copied to a design view.  Now just verify that all the drawing views are also in the master LOD.

[Martin_Goodland]

Right click over Levelofdetail1  at the botom of the tree. You can not copy the default levels to a View Rep but you can copy your own ones.

Regards

Martin

[jtylerbc]

Initially posted that you can't copy an LOD to a view rep - not sure I missed how to do that before, good to know.

What the others have said about LODs is correct - it is for memory management.  The fact that it makes components invisible should be thought of as a side effect, not the reason for using it.  Suppression and LOD should not be used unless you're trying to free up memory, and then only while you have the drawing and assembly set to use the same LOD if you need them open at the same time.

If controlling what components you see is all you want to do, you should be using Visibility and View Representations.  On the screen, View Reps and LOD appear to do the same thing, but behind the scenes they are very different.  You can cause yourself a lot of unnecessary trouble if you try using LOD where you don't need them.  Unfortunately, nobody told me that before I spent a lot of time doing it wrong myself.

[Cadmanto]

I had to completely close out of everything in Inventor, but when I got my assembly back opened

I found this selection.  I selected it and when I get my drawing back open I will let you know if this worked.

[Cadmanto]

What if they are not all in the master.  Should they always be set to master?

Is setting them to master going to mess with the hidden line settings I have implemented on the detail view to this point?

[andrewiv]

They should all be set to master to avoid the issue that you have been experiencing.  When you switch them to master it shouldent mess up your hidden line settings, but any part that was suppressed will now be visible in the view, so you should apply a design view to turn them off.