Drawing Views NOT behaiving

[luke]

I created a view representation and then used it in a drawing. Later I added a new part to the assembly from which the representation was created and the new parts were added to my view on the drawing also. The problem is that the new part added appears in all my drawing views and causes the views to expand to incorporate this part which messe up the drawing totally. T fix this i have to go into a view and select a different view rep, OK that then edit the view again and select the original view rep. OK that then the view is correct again! This is very time consuming. PLEASE HELP!!

All my view representaions are locked as I create them so this is not stopping this issue.

Many thanks in advance.

Luke

[Curtis_Waguespack · Accepted solution]

Hi luke,

We might need more information to figure out what is going on, but the first thing to check is to see if your drawing views are set to be Associative?

To check this, edit the drawing view and look for the checkbox:

Also what version of Inventor are you using?

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

[ic198]

Also try right-clicking on the view in the Browser and select 'Apply Design View'. This makes the view update to the parts currently shown in the View Rep (it does the same thing as you changing the view rep, and then chaning it back, but in one less step). If you set the view to be Associative (see Curtis' post) you won't need to do this at all, but you can't set manual overides on visibility.

[luke]

Thanks for your reply Curtis,

I am using 2013 professional.

I see that my associative is not checked? Is this my problem?!

I still don't understand though that if your view is locked in the iam why it changes in the dwg if you add a part to the iam?

Anyway thanks and look forward to learning more about this.

Cheers

Luke

[luke]

Thanks ic

Yes that 'Apply Design View' works like a charm compared to what i was having to do!!! Thanks.

See my reply above please I still don't understand why a locked view is able to change?

Thanks

again

Luke

[tsreagan]

The view is ONLY locked in the Assembly, and the drawing may or may not conform depending on the associative box.

When you place it on the drawing the associative box has to be checked,  FYI  it remembers it's last setting.

So if you placed a view with it unchecked, in the next drawing, it will be unchecked by default.

This feature lets you connect or disconnect your assembly view from the drawing view for on the fly drawing edits, without having to go back and adjust the assembly view.

T.S.

[luke]

Thanks T.S and all others for your help.

After working through it I am now on top of it! Thanks again.

Luke