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Green brackets around my drawing view? Why?

24 REPLIES 24
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Message 1 of 25
zma1013
19379 Views, 24 Replies

Green brackets around my drawing view? Why?

For Inventor 2012?

IV2012

Windows XP SP3 32-bit
Intel Core 2 Duo 6400 @ 2.13 GHz
Nvidia Quadro FX 3450/4000 SDI 256MB Vram
2 GB Ram
160GB HDD
24 REPLIES 24
Message 2 of 25
mcgyvr
in reply to: zma1013

I'm not using 2012 yet but I seem to remember there is a new process as the drawing environment supports multicore now. Drawing views are initially placed as raster images or something and then when you are ready/done you need to hit some update or generate views or something button to get the final real display.



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Inventor 2023 - Dell Precision 5570

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Message 3 of 25
johnsonshiue
in reply to: zma1013

The green brackets indicate the view is not yet precise. The view is still being computed in the background and certain operations on the view are not allowed during the process. In the past, the user had to wait until the view is fully precise to do anything in Inventor. With high speed drawing view, you are allowed to perform other tasks while waiting for the view finishing compute. For more detail, please go to the following link on Autodesk Wikihelp.

 

http://wikihelp.autodesk.com/Inventor/enu/2012/Help/0000-What's_N0/0001-User_Int1/0011-High_Spe11

 

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 4 of 25
cgalliand
in reply to: zma1013

Is there a setting somewhere you can turn this off?

I am having the same problem and the green corners do not go away.

Message 5 of 25

I am wondering about this as well. I have been away from my computer for 2 hours and the drawing views are apparently still not fully updated as the green boxes are still on the views. How long should this take?

 

Thank you

 

Jim

Jim

Inventor Premium 2013 SP1.1
Vault 2013- plain vanilla version
HP G71 notebook
celeron cpu w\ 4gb RAM and 64 bit system
Win 7 home premium

Ya, my boss has me running my personal machine at work.
Message 6 of 25
blair
in reply to: zma1013

You should be able to turn off the Enable Background Updates from the Application Options>Drawing tab. It always seems to take longer to update the drawings from the Drawing enviroment if the assembly requires updating.

 

Also check that you don't have any other instances of Inventor running or you have Windows Hotfixes that need to be installed on your system.

 

Possibly a system re-start might flush any un-released memory.


Inventor 2020, In-Cad, Simulation Mechanical

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Message 7 of 25
blair
in reply to: zma1013

Aplication Options>Drawing> Differ background updates.

 

You could make sure that your models are up to date befor opening the drawing. You 2Gb of memory is your biggest part of your problem.


Inventor 2020, In-Cad, Simulation Mechanical

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Message 8 of 25
cgalliand
in reply to: blair

I did this, It's in options. I noticed that once I unchecked the box I had to delete the view that was on the drawing already and insert a new one. Not sure why, it just worked.

Message 9 of 25
mcgyvr
in reply to: cgalliand

I would NOT disable that option..

The green brackets SHOULD be there when the view is out of date and is updating.. If its staying for a while there are other problems.. But to turn off automatic updating is just not a good idea IMO.



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Inventor 2023 - Dell Precision 5570

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Message 10 of 25
KF090
in reply to: mcgyvr

Why is this not a good idea? 

(FYI - I agree that it's not a good idea I just want to see what your reasons are)

Message 11 of 25
blair
in reply to: zma1013

It's a two part problem, your hardware (memory) is not up to running Inventor properly. The differ background updates will help your performance but you will loose the ability for drawings to update in the background.

 

It will get rid of the green corner hash marks but drawings will be out of date and will update when you open the next page of your drawing. You will need to wait while it updates.

 

If you were at least on Win7, you could use a thumb-drive for additional memory. Your currently list only 2Gb of memory on your system. This means you will be using your hard-drive as a tempory swap/cache which is extremly slow.


Inventor 2020, In-Cad, Simulation Mechanical

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Message 12 of 25
Ray_Feiler
in reply to: blair

To add to what Blair has said about system memory being low the minimum requirement for video memory is 512 MB.


Product Design & Manufacturing Collection 2024
Sometimes you just need a good old reboot.
Message 13 of 25
wimann
in reply to: KF090

I would suggest that it is, in fact, not a bad idea to turn the feature off. At least until it works properly. What I've observed is that having the feature on allows your views to update in the background which is great but then the user has no option of loading the full view by choice, the user instead has to wait which, depending on the size of the model, can take hours.


What I would suggest is to have the feature turned off until Autodesk integrates a button that can load the full view on demand. One might argue that the "update" button near the application menu will perform this task but after having just attempted to utilize it, I can confirm that it does not, in fact, load the full view and remove the green brackets.

 

The logic behind this option is solid, but you'll spend more time waiting for the view to eventually load then you would to have the view load all at once when the drawing is opened.

 

And to confirm, the option is toggled under Application Options/Drawing "Enable Background Updates". Untoggling disables the option but note that I've not found a way to remove the property from views to which it has already been applied. In other words, a view with green brackets must be deleted and replaced (with the option turned off) in order to remove the green brackets. There may be another way but I've not yet found it if there is.

-Will Mann

Inventor Professional 2020
Vault Professional 2020
AutoCAD Mechanical 2020
Message 14 of 25
wimann
in reply to: blair

In response to my previous post, I've found the button I was missing. If you right click the view, one of the options in the menu will be "Make View Raster" which will add the green brackets to a view if they're not already there. Once they are there, right clicking the view will have the option "Make View Precise" which will update the view and remove the green brackets. So with that said, and to correct my previous reply, I'd say the tool seems like a useful option to have enabled. I don't see why you wouldn't have it turned on at all times.

 

Thanks.

-Will Mann

Inventor Professional 2020
Vault Professional 2020
AutoCAD Mechanical 2020
Message 15 of 25
Jeroen.Rijckaert
in reply to: wimann

Same problem with Autodesk Inventor 2015. One of the views on the drawing shows green corners, which do not go away. Open assembly file, update everything, save assembly file, but the green corners are still there. Saved the drawing, closed Inventor, restart Inventor, but the green corners are sill there. Waiting for some time, but the green corners do not go away. Only after right-clicking the view and "Make View Precise" the green corners go away. But why didn't they go away automatically in the first place?

Message 16 of 25

Hi! The green brackets mean the view is not a precise view (vector). It is a raster view (pixel). There are two ways to get raster views. First, the view is set to Raster on creation. Second, the view is still being computed and the raster view is shown in the meantime. Go to Tools -> Application Options -> Drawing -> "Enable Background Update." When this option is checked, raster views will be shown during compute.

Many thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 17 of 25
ARushton8504
in reply to: blair

I have had same problem. Solved by updating model first then update drawing.

Message 18 of 25
johnsonshiue
in reply to: ARushton8504

Hi! The behavior you are seeing should be as designed. It is because the drawing views are associative to the model geometry. If model geometry is not up-to-date, the drawing views cannot be up-to-date.

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 19 of 25

2019 and this is STILL a problem...

 

Autodesk, this is becoming a joke!

Message 20 of 25
blair
in reply to: robert.rice2573J

Something within the view generation is taking a while to build. I would be looking at opening the IAM and doing a full rebuild and save, then close the assembly. It should reduce the time it takes to generate the view.

 

Build times are also dependant on hardware and the number of directories Inventor has to search through to "build" the model.


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
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