Raster View Artifacts stuck in .idw

[TBuccieri]

Just got done with >20 drawings. Going to print and I get "One or more drawing views are currently in raster state......". The thing is:

-none of the views are green boxed

-no views have red lines through them

-none have "Raster View" checked in the Drawing View dialog

-"Make Precise" isn't available upon RMB

-"Enable Background updates" has been off since day 1

I copied a drawing and erased everything. This is what you get on screen.

Empty Paper

And this is what you get upon Print Preview.

Print Preview

There's nothing in the Browser so where is this image coming from? 

Inv2019.3

[johnsonshiue]

Hi! Could you share the files here or send them to me directly ([email protected])? I would like to understand the behavior better.

Many thanks!

[TBuccieri]

Thanks for the offer, John. I'll send you a file, first thing in the morning.

[nate.wilgus]

I am having the same issue. The only solution I have found has been to erase the page completely and redo it. I can safely copy everything from the page with the artifact, so that leads me to believe it's connected to the page somehow.

[todd_cannon]

Try this: First go to the respective assembly file and do a "Save All". Next go to the drawing file and update all sheets and then "Save All" again. Check your drawing views. I have had this fix the issue for several of my users.

Cheers,

Todd

[johnsonshiue]

Hi! Have you tried tuning off "Enable Background Update" (Tools -> App Options -> Drawing)?

Many thanks!

[LFMarshall]

Just encountered the same/similar issue.  2019.4

All views were up to date, but i received a raster view notice at time of print.

Background updates were turned off.

From a pdf I could see that the geometry in question was coming in on Layer 0.

Turning this layer off and making it a non-printing layer did not remove it from my prints.

Tried copying sheet to a new drawing, did not resolve the issue.

Like was previously mentioned I created a new sheet and replaced my views to get around the issue.

Created a new

[johnsonshiue]

Hi Larry,

It has been a while since I looked this case. I vaguely remember the cause to the original issue was that the idw file was converted (saved as Inventor dwg at one time and there was some viewports or geometry added to the dwg file). Then it was saved back to idw. That is where it happens.

If you have access to AutoCAD, you can try the following. Open the idw file in Inventor -> save as Inventor dwg. Open the dwg in AutoCAD -> Purge All -> Save. Open it in Inventor. Does the artifact still exist?

Many thanks!

[rik_pfau]

We've got a drawing with the same issue. I tried your suggestion of purging everything in AutoCAD, then re-opening in Inventor. The artifact still exists. The solution of copying all of the views, etc to a new sheet seems to be the best option.

[sundars]

Hi All,

This is actually a problem related to a leaked drawing view preview object and not related to a raster view or Enable Background Updates or AutoCAD objects.

We have been chasing this issue for a couple of months now - so far we have had 2 reports come in (INVGEN-24750) but have no way to reproduce the problem. We think that it was a problem introduced in Inventor 2017 or 2018 when a user created a drawing view preview but aborted the view after a series of preview operations (e.g. changing view orientation or any recomputable options in the view dialog). We fixed a similar problem in 2019, but since we have no steps to reproduce this leak, we are not sure whether we covered all the issues.

If you have anyway to reproduce this issue from scratch, please contact me or @johnsonshiue or post steps to this article - it would be of huge help to us in understanding this issue and fixing it.

As a workaround, the best way is to copy the individual views into a different sheet or drawing and delete the original sheet. That should solve the issue. Avoid copying the entire sheet as the leaked object will also be copied.

Thanks

-Shiva Sundaram

Email: sundarsATautodeskDOTcom

[sundars · Accepted solution]

Hi All.

This issue was also reported in https://forums.autodesk.com/t5/inventor-forum/realign-auxiliary-views-command-creates-hidden-raster-...

We have fixed the issue and the fix should be available in the latest updates for 2020 and 2021.

Thanks

-shiva

[4thAxis]

I'm using 2022. my views are stuck in raster view, I never enabled it anywhere, check box in "edit view" is unchecked, I went into the application options and disabled background updates, still in raster view.

Just tried copying to a new sheet and that still fixes the problem.

Details:

I created a mold of this part first, then exported the face that will be the part, into a DXF. I then made a sketch and inserted the DXF. I extruded the part from the sketch that is using the DXF.

I used the part in an assembly and the assembly in an IPN, as well as Inventor Studio.

[sundars]

Hi @4thAxis 

This issue looks dataset specific where the view itself has not been converted into a precise view. It's possible that the something went wrong with the background compute. It doesnt look like the original issue described on this thread which is about orphaned previews. I assume that you can edit the view and can also highlight it from the browser.

In anycase, if you can share your model with us we will gladly take a look - please email part/drawing to "sundarsATautodeskDOTcom.

Thanks

-shiva

[jversteegUGNLW]

This issue is not fixed. Still can happen in 2022

sundars workaround: copy the individual views into a different sheet or drawing and delete the original sheet still works

[sundars]

Hi @jversteegUGNLW 

Can you reproduce this issue from scratch on Inventor 2022? If so, we would greatly appreciate steps to reproduce and a dataset. If it's an old drawing, yeah, then that would explain the issue.

Thank you

-shiva

[jversteegUGNLW]

I was unable to reproduce this. The drawing was of a new part just drawn yesterday. It had issues as soon as it was placed in sheet space. (Didn't have any line entities in view one to auto dimension off of.) I tried to re-create today and just can't get it to happen. It occurred on two out of three drawing files in the batch yesterday both of which are now corrected. 

[sundars]

If you are able to share your model with me I am happy to play with it to see if I can reproduce it using previously known workflows. You can email it to me at: sundarsATautodeskDOTcom

Otherwise, lets continue to keep a watch on it.

Thanks

-shiva

cc: @t_pcoll