Community
Inventor Forum
Welcome to Autodesk’s Inventor Forums. Share your knowledge, ask questions, and explore popular Inventor topics.
cancel
Showing results for 
Show  only  | Search instead for 
Did you mean: 

Drawing view crossed out

29 REPLIES 29
SOLVED
Reply
Message 1 of 30
cwhetten
27947 Views, 29 Replies

Drawing view crossed out

I am drawing a blank on this one:

 

One of our designers has replaced a model reference in a drawing, and now the drawing views all show up with the green boxes around them (raster views for background updates) and the browser shows all of the drawing view icons have a slash through them:

 

Drawing View Slashes.jpg

I have seen the raster views can get stuck and don't update, but I have never seen the slashes through the drawing view icons.

 

Does anyone know what the slashes mean?

 

-----------------------------------------------------------------------------------------
IV2014 Pro Update 2, Build 170; Vanilla Vault 2014
Win 7 Pro 64-bit SP1; Intel Xeon Duo @2.40 GHz, 9 GB RAM,
NVIDIA Quadro 2000, 1024 MB GDDR5

 

Cameron Whetten
Inventor 2014

29 REPLIES 29
Message 2 of 30
cbenner
in reply to: cwhetten

Is the model he replaced in your project?  I've never seen this either, but it looks like it's trying to convey some sort of broken link, like maybe it cannot find the file you are replacing with.  I dunno... wild stab in the dark.

Message 3 of 30

Hi cwhetten,

 

This indicates that the views are static Raster Views. Look for the Raster View Only checkbox at the bottom of the Edit View Drawing View dialog box to change the view from a static raster view.

 

Autodesk Inventor Raster View Only.png

 

You can use the browser right click menu to convert an individual view to/from precise or raster, or the right click menu in the display area and select Make All Views Precise / or Make All Views Raster to convert multiple views at once.

 

A related link, in case it helps:

http://wikihelp.autodesk.com/Inventor/enu/2014/Help/1283-Inventor1283/3181-Drawings3181/3215-Drawing...

 

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

Message 4 of 30

That's it, Curtis.  Thank you!

 

And thanks for playing, Chris!  Smiley Wink

 

Cameron Whetten
Inventor 2014

Message 5 of 30
SysDesign
in reply to: cwhetten

Drawing view locked in raster state at 12%.  Will not update over night or other workstations.  Assembly file size 4,187 KB.

Message 6 of 30

Hi SysDesign,

 

Please take the time to post your question with the details and information others would need to assist you. For example: system details such as OS, Inventor version, Inventor service pack level, how much RAM you have, as well as details about the model you're working with, how many parts are in play, what you've tried so far, screen shots, and so on.

 

Others are much more likely to take the time to help you, if you've taken the time to help them understand your issue and question.

 

With all of that in mind I can only guess that you've run out of system resources when trying to create a view of a large assembly, but this is only a guess. Can you provide more details on your system?

 

Also please do not create duplicate posts. See rule 4:

 http://forums.autodesk.com/t5/FAQ-How-To-Using-Autodesk/Ground-Rules-Please-review-before-participat...

 

 

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

 

 

Message 7 of 30
cmharb
in reply to: Curtis_Waguespack

I am getting this problem as mentioned above, but when i click on the tick box you suggest nothing happens, then when i look at the options again its re-ticked the box.

 

When i click 'make precise view' it changes nothing.

 

Meaning that i cant print any decent sized assembly drawings.

 

I have 32gb of memory so it shouldn't be a resource issue, atm its happening to an assembly with 227 instances and 126 unique parts. I've got to get this sorted as it makes inventor useless.

w7u-64sp1,iv14,intel.xeon.e5-2620 0 @2.00 2.00-32gb,gtx560-4gb
Message 8 of 30
marina.collet
in reply to: cmharb

I got a similar problem with a huge assembly drawing (over 10'000 occurences).

"Raster" option in the edit view window always remained ticked.

"Make precise" was missing from the context menu.

 

My solutuion was to save all components in order to get them all migrated to 2014 (open assembly, "I" menu > save > save all) 

Next time I opened the drawing, there were no raster view any more.

Message 9 of 30
iamerm
in reply to: cmharb

I'm experiencing this same issue today (& it's happened before).  Unfortunately, Chris's excellent suggestion didn't work for me.

 

Also, just as cmharb posted, when I uncheck "Raster View Only" & hit OK, nothing happens.  Immediately afterwards I edit the view again, & "Raster View Only" is checked again.  Very strange...

 

In addition to the annoyance of the view not updating, this also causes issues with balloons.

 

 

Message 10 of 30
Curtis_Waguespack
in reply to: iamerm

Hi iamerm,

 

Did you ensure that your files were migrated to the version you are using, as per HE_mcollet's suggestion? If not here is a link that might help you through those steps:

 

Migrate files using Task Scheduler

http://help.autodesk.com/view/INVNTOR/2015/ENU/?guid=GUID-873B3D0D-E1D7-4CF3-BFC3-1956B43389F2

 

If that doesn't help please post back to this thread to let us know.

 

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

Message 11 of 30
swalton
in reply to: iamerm

I have had this issue too. 

 

I added the "make views precise" command to my radial menu when I have a drawing view selected. I can use that command to bypass the stuck checkbox in the Drawing View window.

 

I have also installed Service Pack 2.  I have not had to open a big drawing after installing the service pack, so I don't know if that will help.

Steve Walton
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.

EESignature


Inventor 2023
Vault Professional 2023
Message 12 of 30
iamerm
in reply to: Curtis_Waguespack

Curtis,

 

Thanks for your reply.  I saw that suggestion, but I honestly haven't tried it.  Migrating files using Task Scheduler is a whole separate issue for me.  If you're bored, you can read about it here:

 

http://forums.autodesk.com/t5/Vault-General/Task-Scheduler-Migrate-Files-From-Vault/m-p/4339838

 

This one got escalated, but never resolved.

Message 13 of 30
iamerm
in reply to: swalton

swalton,

 

Thanks - that's another good idea.  I may try that in the future.

 

Today I fixed the issue by closing & then reopening Inventor (which leads me to believe this might be some sort of memory issue).

 

Please mark this post as the best solution ever:  restart Inventor.  Smiley Wink

Message 14 of 30
chase35
in reply to: cmharb

I had the same problem, however I had only one part, so I could confidently assume that it was not a memory issue.  Right clicking and selecting "Make All Views Precise" had no effect, nor changing them individually.  

 

What worked was going in to Inventor Options, Drawing, and Clear the Enable Background Updates box.  

Message 15 of 30
5103141590
in reply to: chase35


@chase35 wrote:

I had the same problem, however I had only one part, so I could confidently assume that it was not a memory issue.  Right clicking and selecting "Make All Views Precise" had no effect, nor changing them individually.  

 

What worked was going in to Inventor Options, Drawing, and Clear the Enable Background Updates box.  


Had the exact same results as chase35. "What worked was going in to Inventor Options, Drawing, and Clear the Enable Background Updates box."

Message 16 of 30
MikahB
in reply to: 5103141590

+1 on this. Very odd.
Mikah Barnett
All Angles Design
Product Design Suite Ultimate 2014
Windows 7 Professional x64
Intel i7-3770k @ 4.5GHz
32GB DDR3-2400 RAM
GeForce GTX 670 4GB
Message 17 of 30
Matt
in reply to: cwhetten

I'm having the same Raster problem. I've tried everything listed here except for the task scheduler option, as I need our IT department to work on the server. 

I haven't got a large assembly. I have been using a step file from one of our manufactures in China. I've repaired the body, applied some direct edits and modelled  on top/to the surface for our changes.

I've tried shutting down and restart, enable box in the options, raster view box in drawing view, Make all precise from the right click, added it to my radial menu(right click), saved all as 2015 version I'm currently running on.

When I initially place my plan view, this is OK. All the projections, are stuck at raster. I've tried placing them manually and aligning which hasn't worked. 

I'm sure I've just had the second service pack added, as I have the freezing home page issue recently.

Message 18 of 30
mwadkins12
in reply to: cwhetten

This worked for me, but results may very...

 

Go into Application Options and under the "Drawing" tab, uncheck "Enable Background Updates" towards the bottom. Apply and close.

Then in your model tree, go to the view with the forward slash going through it and right click and choose to edit view.

Once in the edit view window, click on and check "Raster View" and click the Okay button.

After it updates, save the drawing and repeat the process, only instead of turning "Raster View" on, you will be turning it off (or unchecking it).

After it updates again, it should remove the issue, at least it did for me in Inventor 2016 Pro.

 

Hope this helps some.

Message 19 of 30
gijsheufkens
in reply to: iamerm

That's funny, restarting Inventor worked for me as well.

Message 20 of 30
josh
in reply to: marina.collet


@marina.collet wrote:

I got a similar problem with a huge assembly drawing (over 10'000 occurences).

"Raster" option in the edit view window always remained ticked.

"Make precise" was missing from the context menu.

 

My solutuion was to save all components in order to get them all migrated to 2014 (open assembly, "I" menu > save > save all) 

Next time I opened the drawing, there were no raster view any more.


Just wanted to add a +1 for this. i was having the old "nothing would make the view non-raster" issue and this worked for me. Thanks for the idea marina.

---------------------------------------------------------------------------------------------------------------------------------------------------------
Product design suite ultimate
Complete 3D Concepts
 photo Autodesk_Inventor_2015_Certified_Professional_Badge_zpsf8iygufo.gif

Can't find what you're looking for? Ask the community or share your knowledge.

Post to forums  

Autodesk Design & Make Report