Inventor 2012 Inaccurate View Creation

[Anonymous]

We recently finished the upgrade from 2010 to 2012 and are now having issues with view creation. We are having problems with view creation on models migrated from 2010 as well as new models created in 2012. We extensively use frame generator with a custom profile library, all worked great in 2010.

When creating views sometimes the frame members are extended beyond where they are in the model (any beyond the envelope of the base skeleton.) Also smoetimes random frame members are short or missing from the views.

Occasionally this can be fixed by screwing around with the hidden line and shaded edit view options (switch it a bunch of times and occasionally you get lucky and everything shows up correctly.) If that doesn't work then you have to re-start the drawing from scratch and hope it doens't happen again.

Has anyone else seen something like this or have any suggestions for correcting the issue? This is absolutely killing our productivity.

[MariaManuela]

You already installed SP1 (launched at 30/8/2011)?

[Anonymous]

We have SP1 installed on all machines.

[Shiva_Sundaram]

Hi,

Can you please send me your dataset? We fixed a very similar issue in R2012 Sp1, so we would definitely like to see your model and see why this problem still happens.

To temporarily fix the issue:

1. See if you can open those particular problematic parts and rebuild them

2. Then switch to the parent assembly and update parent assembly

3. Finally switch to the drawing.

The problem should go away. Please let me know if this workaround fixed your issue.

Here's a link on a very similar issue.

http://forums.autodesk.com/t5/Autodesk-Inventor/Extended-lines-in-drawing-from-custom-frame-generato...

Thanks and you can contact me @ sundarsATautodeskDOTcom

-Shiva Sundaram

Inventor Development

[Anonymous]

Shiva, thanks for the reply. The file set is rather large, but is already at Autodesk under Subscription Case #06732840. I figured I'd try here also and see if others were having a common issue.

[MattH_Work]

Try turning off Background Updates from within applcation options. I've found a number of issue go away when reverting to the traditional view update method

MattH

[Shiva_Sundaram]

Hi,

I was able to track down your subscription report and got your assembly. I verified that view creations of this assembly in the different view orientations you have are working properly. And this seems very similar to the issue we fixed in SP1.

It would be helpful if you can give some steps to reproduce the problem - particularly what specific changes you made to that part which seems to be out-of-location.

Knowing those specific modeling changes would greatly help us identify the issue.

Please also give your your IDW so that we can see the actual problem.

The other questions I have are:

a. I presume that after applying SP1, you opened your drawing and updated your views.

b. Did you have any errors or issues when updating to SP1 (just trying to rule out the obvious).

Yes. we have had a handful of issues with Background updates, most of them should be resolved with SP1.

Thanks

-Shiva Sundaram

Inventor Development

[Anonymous]

Shiva, here is the latest update to the subscription:

Daren, the IDW that is included with the file set that I sent you was last updated in SP1. I just opened it again and updated all sheets...same issue still remains.

Workspaces\Workspace\Framing\2011\K110844\details\K110844-000.idw

Sheet 1, Views 3 & 4

Sheet 2, View 6

Sheet 3, View 8

Sheet 4, View 13 & 15

Sheet 5, View 20, 22 & 25

I can save the IDW again if you like, but I just re-checked the file set that I already sent you.

The drawing was created with 2010, opened in 2012 SP1 and all of the sheets were updated. Again, we tried this on 3 different computers here and still have the same problem. I currently have the pack&go file set open, updated the views again and still no luck.

[Anonymous]

I've been playing with this some more and did a "rebuild-all" on the model that this idw file is based on, then updated all of the sheets. It fixed a couple of issues, but not the majority. I double checked my version: Build:190, Release 2012 SP1 - Date: Mon 08/08/2011. The attached sheet shows a little more detail about what's missing...the longer you stare at it the more you see. Many of the other views still retain view errors, this is the best of the 10 sheets for showing them.

[Shiva_Sundaram]

Hi,

My apologies. I didnt see the IDW inside the "detail" directory. Yes. Now I can see the displaced components when I open the drawing.

Can you also let me know your Inventor Build Number. This can be found on the "About Inventor" dialog box. To access this, click on the question mark (pulldown) on the top right corner and click on "About Inventor..."

You had indicated that you "updated all sheets". When you open the drawing the lightning bolt on the left side should highlight. Did you click on that and find that your views didn't change? The update all sheets command will not do anything unless you have dirty views on different sheets. Could that be the problem?

Here's what I did to fix your issue.

1. Open the drawing

Method 1: Model Rebuild

a. Open the top level assembly

b. Rebuild ALL

c. Switch to the drawing, this will force view update of all your drawing views

*** This fixed all the problematic views *** 

Method 2: Single view update

a. "Click on View 3 on the drawing sheet.

     This will enable the second lightning bolt on the right side.

     Click on the view update lightning bolt. This should update the problematic view and fix it.

b. For each of the problematic views, could you do a single-view update. This will force the individual view to update and fix the issue.

I can't think of anything else which could potentially be going wrong. If you would like you can email me directly: sundarsATautodeskDOTcom

Thanks and hoping the above steps will fix your problem.

-Shiva Sundaram

Inventor Development

[Anonymous]

Shiva, I did the same thing as you did...some of the errors are gone, but most are not. Please see post 9 of now 11, I had tried your "method 1" already and it did get rid of teh really long pieces of extrusion...but it fixed less then 50% of the errors. Here's the latest reply on the support request (would it be easier to communicate with you and Daren through there then keeping up 2 speprate conversations?) Build 190 of Inventor Professional.

Daren, if this requires a "Rebuild-All" or migrate to update the files so that they will work is there any way to do the same procedure on all files that exist in our Vault?

The extrusion is created with the standard Inventor frame generator, however it contains multiple levels of detail that are driven by some iLogic code and triggered by editing the "profile_detail" parameter in the lower level frame assemblies. These features are not what is showing up (or missing from) the inventor views.

The majority of the inaccuracies (but not all of them) are showing up when the view is "looking through" clear polycarbonate panels.

The extrusion is not the only things missing from the views, but all of the "trimming" is done with a custom add-in package supplied to us by Synergis & IDS-Engineering.

[Shiva_Sundaram]

Hi,

Thanks for the clarification. I must have posted while you were posting 9. Ok. I think we are getting somewhere with this issue.

Yes. It would be ideal to take it offline and I don't have your email and hence the posting.

Yes. I agree there are multiple issues here.

Issue 1: Out of place frame-gen components problem. This appears to be fixed.

Issue 2: Some components are not shown correctly and appear to be hidden in shaded view.

This one is not an issue with Background Updates, but a probelm with transparent components not showing other components behind it.

Currently, the only way to fix this is to turn off visibility of that object OR make a hidden line drawing view :(. This is a problem we are looking at and hope to resolve soon. Apologies for this inconvenience and we will let you know if there is any other simple workaround.

Thanks

-Shiva Sundaram

Inventor Development