Draft Preview?

[BillPIII]

I've been using Inventor for a few years now and haven't seen this. It created a base view with green marks and when I go to print it says

"One or more drawing views are currently draft previews. Draft previews differ from final views in quality and may produce visually different results. Would you like to wait for views to update before printing or smash the screen from irritation of having a new roadblock thrown in your way that we make no effort to remove for you? HAHA you ignorant fool you will never learn all the idiosyncrasies of our product".

Which I thought was a bit unnecessary.

It does make some effort actually. It sits there with a progress bar. This drawing is about as simple as I create and it can't get past the progress bar. The wiki help seems far inferior to the 2011 help as this should be a simple thing to find. If I print anyway, there is no line weight. So where is this little switch hidden to turn this off? I've already fiddled with background updates and the sunglasses are not checked and grayed out. I don't know how I never ran across this problem before or what could have changed. Given the performance of my computer, I don't think I need some low grade preview for drawings of this type.

[Shiva_Sundaram]

Hi Bill,

Draft preview indicates that current drawing view on the screen is actually a raster view and the precise view is in the  still calculating in the background. If you let the view go through the calculation process, the raster view will soon turn into a precise view.i.e. the green borders will go away and the browser will no longer display the green in-transient icon.

Then you should be able to print your drawing without that annoying dialog. The dialog is just a notification to indicate that the print quality of raster view may not match the final precise quality in terms of fidelity.

The whole purpose of the raster view is to enable the user to continue to work without having to wait for the view to finish calculating. This way, users can continue with other modeling or drawing operations while the views are being computed.

If you create multiple drawing views or work with models which are significantly large, then the raster workflow would greatly help reduce the time it takes to create drawing views.

However, if you only work with small parts and are only interested in printing AND would prefer to wait until all drawing view calculations are done then there are a couple of options

(a) do nothing - essentially wait for the views to finish calculating 

(b) turn off background updates - Application Options + Drawing Tab + Enable background updates = false.

Turning off the background updates will disable the raster functionality and revert back to Inventor 2011 behavior (the caveat is you will have to wait for a longer time for the views to finish calculating).

Hope that helps.

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[BillPIII]

Given your description, this had to be a glitch in my program. This was just a drawing for a burnout. It was a glorified circle from a part file. Nothing to take up processor and nothing unusual. But I couldn't get free from it and the calculation progress never moved forward.

[Shiva_Sundaram]

Hi,

Thats a bit strange. If you don't print what happens? I guess I am trying to see whether there is a problem with the progress bar dialog or with the view creation itself.

So, if you create a drawing view, if it is a simple enough part, it should first create a raster view (green borders) and then immediately turn into a precise view (no green borders). It would probably happen fast enough that you would not even see the progress bar.

Perphaps something is going wrong in the calculation of the precise view. Would it be possible for you to send me your part?

You can email me at: sundars@autodesk.com

Thanks

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[BillPIII]

Given my computer and how simple this drawing is, I shouldn't see anything like that and haven't until this point. It did seem like it may have snapped out of it as I was closing the file. So I'll need to check to see if it is still a problem but I am tied up right now. I can probably upload this one. I did get the progress bar but it didn't actually progress. It just sat there like it is stuck. This is not much more than a circle with two flat spots which is extruded a few inches. Nothing fancy at all and nothing that I should be able to see calculate. I could do it with microsoft paint. But if you print anyway, there is no line thickness to the part. The dimension lines are thicker. I'm not sure given my computer specs if I need these raster views anyway. It wasn't a bottleneck in previous versions.

[lark22]

I have the same problem with simple drawings that were created with Inventor 2010 or 2011.  Just "upgraded" to 2012, when trying to print small drawings that were fine in previous versions, I receive the draft view notice.  When trying to convert the views the progress "locks" and does nothing for at least 5 min. (more time than it would take me to re-insert the view and detail)  I did unclick the enable background updates and restarted Inventor, this fixed the problem.

[Shiva_Sundaram]

HI,

Sorry to hear your issues with the new background updates. Would it be possible for you to share your data with me. You can email me at: sundars@autodesk.com

Also, I am curious to know about having to wait a long time. Did you cancel out of the print dialog and were waiting or did you have the print dialog still up?

I presume, you tried to print but later cancelled out of the dialog. Just a note that, having the print dialog still up would block the views from finishing the final update. i.e. Inventor is not tied up processing some other command/dialog.

Also, would it be possible for you to do a simple test of re-creating the views with Background updates ON and see whether they are still taking too long.

Thanks

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[luacevq]

I used to have the same problem with the draft preview but it started to work fine when I uncheked the box you said. However, Bill also talked about another problem when you use the constraints, the sunglasses are in gray so you dont see the constrait preview. As a matter of fact, I have to move the piece after I click ok to the constraint for the piece to take its proper place, otherwise it stays at the initial place. I can still work but its a bit anoying.

I´m sorry if something is not well written, I dont write in english to offen.

[aosborne32]

I too am having a problem with the Draft Preview.  I have a fairly simple part with 54 holes, nothing else.  I am trying to close Inventor and get the message "one or more drawing views are being computed and display as draft preview.  The document(s) may be closed and pending updates will resume when the document is reopened."  It has been pending (green corners) for over an hour now.  Not sure what is taking so long?

[Shiva_Sundaram]

Hi,

Can you send me your model file and the type of view you tried creating? I can take a look at the issue.

If you can include your machine configuration (OS, CPUs, RAM, hard disk size etc.) that would be helpful.

You can email me at: sundars@autodesk.com

Thanks

Shiva Sundaram

Inventor Development

Autodesk, Inc.

[Shiva_Sundaram]

Hi

We have posted a hotfix to address some of these recent instabilities with drawing updates in Inventor R2012.

Could you please get the hotfix and try your drawing view creation / update again and let us know if you still have any issues?

The hotfix can be found at:

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

Thanks

-Shiva Sundaram

Inventor Development

Autodesk, Inc.

[yenchiou.ng]

I have the same problem. Background update is on, when i tried to print it, it required me to update all the views and it takes at least few hours. Sometimes, i leave it update overnight. it is annoying. Do you have other solutions other than waiting for update or just turn on the background update? And, i cannot provide the files or models due to company policy.

[Shiva_Sundaram]

Hi,

I am sorry your models are taking a long time to calculate. It would really be very hard to guess what the problem is without seeing it.

Can you post your machine specs?

There could be other problems related to

a. very large data

b. threads being enabled in drawing views

c. shrinkwrap parts perhaps?

But mostly, views in general take long time if you have bad geometry or imported data which is bad. If you have imported data, please make sure you import them with "auto heal" enabled during import - this will fix issues and make downstream modeling operations better.

Finally, you can always turn off background computes (Application option + Drawing + Enable Background updates) and see if it fixes your issue.

Thanks

-Shiva Sundaram

Inventor Development

[BillPIII]

I had forgotten about this post and don't really remember the issue. But haven't had the problem again. It was so intermittent I couldn't track it down but annoying when it did happen.

[aosborne32]

It is an aggravating problem and to date haven't found a way to fix this, sorry. It doesn't always happen that's part of the issue. There isn't really a way to track the problem because it isn't an on going thing. -- Andrew Osborne CNC Programmer/Machinist 2391 Lexington Ave. Evansville, IN 47720 Main Line: 812.464.8521 Ext. 3 (ask for Andrew) Fax: 812.468.4176 Email:aosborne@specialty-tooling.com Specialty Tooling Inc.

[mflayler2]

Not to state the obvious, but have you just tried turning off the background updates if it is that annoying to you?

[aosborne32]

Yes I have, it didn't seem to affect it. We are running Autodesk Vault now and the problem has only happened once in the last 6 months so I'm not too worried about it anymore. -- Andrew Osborne CNC Programmer/Machinist 2391 Lexington Ave. Evansville, IN 47720 Main Line: 812.464.8521 Ext. 3 (ask for Andrew) Fax: 812.468.4176 Email:aosborne@specialty-tooling.com Specialty Tooling Inc.

[yenchiou.ng]

It is worse if u off the Background update, dont try it

[Shiva_Sundaram]

Hi,

I think there might be something bad or just not performant in the model. In most cases, the problem happens much upstream during the model stage. When generating drawings, the compute algorithms try to process the model geometry and if it encounters some badness, there is a potential for some slowdown. The problems could also manifest in the modeling world in such cases - although a little more obscure to reproduce.

Just as an FYI, all customer data is treated confidentially at Autodesk and never leaves our company. You can be assured of that. If you have further restrictions we are always happy to sign any NDA.

I have tried to put together a list of suggestions to help identify the problem and help fix them.

Search for the bad component

1. Open the model and drawing once again

2. Switch to the model and start delete a few components (you could start at the top or from the bottom)

3. After deletion, switch back to the drawing and see if it updates faster

4. If yes - then the problem might in one of those components you just deleted

5. Re-trace steps (3) and (4) again to narrow down the problematic component

6. At some point, the drawing will take a long time - the component which makes the drawing view go slow is likely your problem component.

Alternate Search post-drawing view creation

1. Turn the visibiltiy of all parts/subs in your model

2. Create the drawing view with (associative design views On)

3. Now, edit the drawing and UNCHECK (associative design views) in the view dialog

4. Now you will be able to turn on components from the drawing browser one by one

5. Start turning ON components a few at a time (starting from the top or bottom)

6. The views will recompute

7. The action which makes the drawing view slow will lead you to the problematic component.

Dealing with parts with 100s and 100s of threaded holes?

You may want to uncheck threads during the design process and turn on threads when you are ready to do final documentation so that you pay the penalty one time.

Composite surfaces or shrinkwrap parts

You may want to see if you can isolate any bad surfaces in your model and repair it (repair environment) in parts.

Imported parts

If you deal with a lot of imported formats, you might want to auto-heal the geometry during the translation process. This will help repair any geometric problems

Finally, as always, you can either send us the whole model OR a subset of the model and we are always here to help.

Thanks

-Shiva Sundaram

Inventor Development

[Colin_Reeve]

I got rid of mine simply by right clicking the view, selecting edit, and then unchecking " raster view only" at the bottom of the dialog. Sometimes I have to remove the associativity chain link from the "style from base view" and then remove the "raster view" on each view. Seems to get around it.

This always happens to me when I get a view which has a component that is complex, ie at least >300 occurences and it seems that the computer is beginning to struggle a little. By struggle a little, if the view does not move and rotate cleanly in an orbit then the computer is struggling.

Sometimes a restart works. But most times not.

Hope that helps some of you.

Col