Problem with drawing updating views in 2012

[tysonwitte]

Hi,

I am using Inventor 2012.  Frequently when making drawings, my drawing views get stuck with the green corners around  them and they do not update.  When I close the drawing file, I get the message.  " One or more drwing views are being computed and display as draft view"

When I re-open the drawing,  I get the same thing.  The green recycle arrows are in the browser next to the view.  The only thing I have found to cure this is shutdown inventor and restart, which is annoying.  Pressing the update button does nothing.

Any suggestions??

Thanks

Tyson

[Shiva_Sundaram]

Hi,

Would it be possible for you to send me your model(s) and drawings? I can take a look and see what the problem is. I suspect that either its taking a long time OR something went wrong with the background update that its not updating your raster views and removing those green corners.

Usually this is indicative of a problem in the model with some bad geometry. You can also try narrowing down the issue by suppressing some features (if its a small enough part file) and see if it fixes your issue.

Also, please check out working with raster views if you havent already done so.

http://wikihelp.autodesk.com/Inventor/enu/2012/Help/0073-Autodesk73/0611-Drawings611/0619-Create_d61...

Also, one more point is if you have any command or dialog active, the background updates will wait until you have finished your command before updating the views. Just make sure you have exited all commands and see if that fixes your issue.

I would be glad to take a look at your model and see if there is anything wrong with the drawing view update.

You can email me at: sundarsATautodeskDOTcom. If the files are too large, you can zip them up or I can setup an ftp site for you. Please also include system specs, ram and OS information.

Thanks and we apologize for the inconvenience caused.

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[tysonwitte]

Hi Please see the (2) attachments.

The drawing is only of a part, not as assembly.  The geometry is relatively simple, I do not see any problems with it. I am getting the green corners on my drawing and they will not go away.

Thanks

Tyson

[Shiva_Sundaram]

Hi,

Thanks for the model files. However, I was unable to reproduce this on my Win7-x64 environment with the released version. Can you please send me your computer specs (OS, RAM, Graphics etc).?

We have also released a hotfix to address some drawing instabilities in Inventor R20102. Could you please apply that hotfix and see if that fixes your issue?

http://usa.autodesk.com/adsk/servlet/ps/dl/item?siteID=123112&id=17235749&linkID=9242019

Thanks

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[mkoeppen]

I am having the same exact problem - when i zoom in to pick a piece of geometry to dimension - it dissapeers and the drawing is not up to date with the ipt i am making it from - yes the green corners are around all my views - does this have something to do with any previous version that piece was made from? the ipt was brought up to date when it was saved in 2012.

[Shiva_Sundaram]

Hi,

I would have to take a look at your model and drawing to figure out whats going on. Can you send them to me along with steps to reproduce, system specs (OS, RAM, graphics card info etc).

You can reach me at: sundarsATautodeskDOTcom

Things to try:

1. Please try the following hotfix and see if that solves your issue. If it does, then no action is required. If not, I can definitely take a look at your issue.

http://usa.autodesk.com/adsk/servlet/ps/dl/item?si​teID=123112&id=17235749&linkID=9242019

2. Keep Inventor idle without any command or dialog up and see if the raster view updates correctly and the green borders go away.

3. Do you have any translated data in your model - sometimes bad geometry can be the root cause of a drawing not updating correctly.

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[blair]

I have seen this as well, not often but when it does, I find closing the drawing and re-opening fixes the problem. Since updating to IV2012 I have only had this happen about once a month.

[danzco]

Several of the engineers at my work are having this problem sporadically.  Even after waiting for an unreasonable amount of time Inventor does not calculate any of the views; they just sit there with the green corners.

When I attempt to install this hotfix I get the message "Internal Error 2903. ixfAssemblyCopy"

At this time the solution seems to be to restart Inventor.  This is not really an acceptable solution.

If it's of any help, it seems to happen most ofter when trying to draw assemblies that contain tube and pipe.

[jason.dupree]

Has this issue been solved? I have two clients that are having the same problem.

[LFMarshall]

I also have this issue, multiple times per week and seemingly random.

For instance, yesterday I was updating multiple component drawings from an iPart.  I opened the iPart, regenerated all instances (approx 10), then went through and opened each drawing watcehd it update and reprinted.  On one drawing out of the entire group I had this issue, the rest updated as expected.

[Shiva_Sundaram]

Hi,

First, to address the install issue reported by "Danzco"......

I believe this error could be related to applying an Inventor R2012 RTM hotfix on top an R2012 SP1 Installation.

The following hotfix is more appropriate when applying on top of R2012 SP1.

http://usa.autodesk.com/adsk/servlet/ps/dl/item?siteID=123112&id=17804781&linkID=9242019

This should hopefully resolve the install issue.

If you continue to have this problem, please let us know what your install version is and what hotfix you tried to apply.

Secondly, regarding the problem related to those green corners (raster views) not turning precise,

It would be helpful if we can get some extra information on the problem.

1. Do those green corners never go away? How long did you wait?

You should be able to hover over the green icon on the browser and see a progress indicator as a tooltip indicating % completed. In most cases, it might be actually related to a problem in the model (bad geometry and such) which could potentially affect the drawing view.

Can you send me the dataset (iam, ipt, idw) and I can try to reproduce the problem and investigate the issue.

You can contact me at sundarsATautodeskDOTcom.

Thanks

-Shiva Sundaram

Inventor Development

[danzco]

Shiva,

Thanks for your response.  It's encouraging that Autodesk folks read the forums.

When I first tried installing the hotfix is was indeed after installing SP1.  After your post I tried again and was able to install it.  The only thing I can think of that's changed is that I installed the multi-issue hotfix that came out yesterday (DL17804781).  Perhaps that had nothing to do with it, but it worked.

If I have any further problems I'll be sure to report back 🙂

---

It would be helpful if we can get some extra information on the problem.

1. Do those green corners never go away? How long did you wait?

---

One time I let it sit there for about 20 minutes while I was working on something else.  None of them ever went away.

---

You should be able to hover over the green icon on the browser and see a progress indicator as a tooltip indicating % completed. In most cases, it might be actually related to a problem in the model (bad geometry and such) which could potentially affect the drawing view.

---

I didn't know about the progress indicator; thank you.  The specific model I was working with when I first posted did not have any bad geometry that I was aware of, but I suppose there could have been some weird stuff in there as some of the models came from vendors.

I would like to reiterate that this has been a continual intermittent problem, so it's hard to gauge whether or not it's only a few assemblies or not.

[Shiva_Sundaram]

Hi,

I am glad you were able to get the hotfix installed. If you have a reproducible case with the raster views not turning precise, please let me know. I would be very interested in taking a look at the problem. Sometimes, when models come from vendors, they may have translated the parts which could potentially lead to problematic geometry which could cause the view compute to take a longer time. You could also isolate problematic components by turning them off in the drawing (or model) browser and see if the problem goes away.

Let me know if I can be of further assistance.

Thanks

-Shiva Sundaram

Inventor Development

[DRLTKSE]

I have the same issues. Once I had to leave a drawing over night to get it to update! This is after waiting all afternoon for it to update.  

I do have translated files in my assemblies, but this is unavoidable for the work I am doing. 

[J.Engen]

Good News!

I have had this problem and after much troubleshooting it looks like there is a solution! These "green corners" are a designation of a raster view, meaning that the precise view is not being calculated. 

The solution is to use the "Make View Precise" feature..

1) Select the view that is causing issues.

2) Right-Click and select to make view precise.

Have you got a lot of views all giving you the same problem, perhaps an entire drawing set with multiple views on multiple sheets?

Whenever I have problems like this that are causing me heart-ache, I try to customize my interface to make the problem more manageable. 

Go to the Ribbon and select "Customize User Commands"

In the Marking Menu Tab, select Environment -> Drawing and Sub-Environment -> None Selected 

Determine a command to bump off (many people do not use the easy-swipe feature so could be almost any, but for those of you who do use all of them, move onto the "Ctrl + ..." sub environment and select one there. 

In the Search box type "Precise" and it will give the two options of "Make All Views Precise" and "Make View Precise"

Add the appropriate command to your Menu and swipe away all of your annoying "green corners"

J.Engen

[Colin_Reeve]

See my post here, it might help;
http://forums.autodesk.com/t5/Autodesk-Inventor/Draft-Preview/m-p/4380080#M480628