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Drawings will not update with part

26 REPLIES 26
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Message 1 of 27
Ross33
16414 Views, 26 Replies

Drawings will not update with part

I am having some issues concerning updating drawings. When a part (.IPT) is placed in a drawing, everything is fine (ie. the views represented in the drawing are up-to-date). Yet, when I make a change to the part (something as small as a dimensional change) it does not translate through to the drawing. This is also the case for iProperties.

 

I have been playing around for a while now, but have had no luck. The part is also an iPart, but this shouldn't matter.

 

If nayone knows why this is happening I'd love to here.

 

Thanks,

Ross.

26 REPLIES 26
Message 2 of 27
JDMather
in reply to: Ross33

Attach files here.


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Message 3 of 27
blair
in reply to: Ross33

Is your drawing set to defer updates?


Inventor 2020, In-Cad, Simulation Mechanical

Just insert the picture rather than attaching it as a file
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Message 4 of 27
Ross33
in reply to: blair

I also thought 'Defer Updates' may have been the issue, but it is not checked.

Message 5 of 27
drlamb
in reply to: Ross33

ake sure your drawing view is set to associative.

Donald L.

Inventor Product Design Suite 2016
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HP h8-1380t - i7-3820 @ 3.6 GHz
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AMD Radeon HD7950 3Gb
Message 6 of 27
mcgyvr
in reply to: drlamb

Since its an ipart try a rebuild all in the ipart factory. Autodesk knows about this bug but doesn't seem to want to fix it.



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Inventor 2023 - Dell Precision 5570

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Message 7 of 27
Ross33
in reply to: drlamb

I don't seem to have the option to 'set to associative'.

My 'drawing view' is not the same as shown in your image.

 

Also, I have tried updating all iParts within the family, but this has not helped.

Message 8 of 27
JDMather
in reply to: Ross33


@Ross33 wrote:

I don't seem to have the option to 'set to associative'.

My 'drawing view' is not the same as shown in your image.

 


 

I don't see where you ever stated what version of Inventor you are using?
Attach the files here.

 


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Autodesk AutoCAD 2013 Certified Professional
Certified SolidWorks Professional


The CADWhisperer YouTube Channel


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Message 9 of 27
Ross33
in reply to: JDMather

My apologies. I am using Inventor 2010.

Message 10 of 27
mcgyvr
in reply to: Ross33


@Ross33 wrote:

I don't seem to have the option to 'set to associative'.

My 'drawing view' is not the same as shown in your image.

 

Also, I have tried updating all iParts within the family, but this has not helped.


Not updating.. Rebuild all (its on the "manage" tab in the "update" section)

With all iparts I now have an ilogic rule to rebuild all before save. It works around this issue since Autodesk won't fix it.

A similar thing happens when you add design view reps to iassemblies.. They won't show up in the drawing edit view dialog until you rebuild all in the iassy.



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Inventor 2023 - Dell Precision 5570

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Message 11 of 27
JKJAxell
in reply to: mcgyvr


@mcgyvr wrote:

 

With all iparts I now have an ilogic rule to rebuild all before save. It works around this issue since Autodesk won't fix it.


-How did you do this? In iparts my iLogic options are all greyed out. I cannot create any rules or manage triggers...

 

Message 12 of 27
johnsonshiue
in reply to: Ross33

Hi! I assume that you have an iPart factory file where you are making changes to, while the iPart member files have been documented in the drawing. The reason why you are seeing the behavior is that the part files pointed by the drawing views are the iPart member files (under iPart folder). The changes you make on the iPart factory file has not yet reached to the members.

You simply need to open the iPart factory file -> go to the browser -> expand the table node -> select all members -> right-click -> Generate Files. Then the changes made in the factory file will be sent to the member files. Next time you open the drawing, the views should be up-to-date.

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 13 of 27
ilive42day
in reply to: Ross33

In the drawing right click on the drawing view and edit view. Then check the little box which makes the drawing view associative. The drawing view will now update.

Message 14 of 27
fsdolphin
in reply to: mcgyvr

@mcgyvr

With all iparts I now have an ilogic rule to rebuild all before save. It works around this issue since Autodesk won't fix it.

 

Do you mind sharing your code for the iLogic rule you are currently using for the rebuild all before saving files? 

 

The only method I found was the Rebuild() but not a RebuildAll method.

 

Would this be sufficient if I trigger the following rule before saving?

 

ThisDoc.Document.Rebuild()
Message 15 of 27
johnsonshiue
in reply to: fsdolphin

Hi! I must have missed some messages. Could you elaborate on what you meant by "Autodesk not willing to fix the issue"? How do I reproduce the problem?

Many thanks!



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 16 of 27
fsdolphin
in reply to: johnsonshiue

 

 

 

 

 

Message 17 of 27
johnsonshiue
in reply to: fsdolphin

Hi! I am aware of some iPart/iAssembly issues but I am not aware of a systematic issue blocking users from using the workflows. Could you elaborate on what exactly you want to achieve? I should be able to provide the best workflow accommodating the need.

Thanks!

 



Johnson Shiue (johnson.shiue@autodesk.com)
Software Test Engineer
Message 18 of 27
fsdolphin
in reply to: johnsonshiue

The short answar would be... to be able to use iParts/iAssemblies the same way Configurations are used in SolidWorks. Even if there are issues I would like to knwo what they are and what the work around is but we need to use iParts/iAssemblies. This is a must.

 

I little background about our company:

We are moving from SolidWorks to Inventor. All of our products have a lot of variations so we used to use Configurartions a lot in SolidWorks, about 80% of our parts/assemblies have configurations.

 

In this trhead I actually explain my procedure and why I'm afraid to start using iParts/iAssemblies without a plan.

http://forums.autodesk.com/t5/vault-general-discussion/procedure-for-checking-in-and-out-iparts-iass...

 

I have so many questions about iParts/iAssemblies but not a lot of people seem to be using them, most of my questions don't get answers or get one or two replies. It's hard for me to believe that not a lot of pople are using them.

 

http://forums.autodesk.com/t5/inventor-general-discussion/behavior-after-converting-a-standard-part-...

 

Not complaining, I really appreciate the help in this forum.

 

Thanks a lot

Message 19 of 27
BeKirra
in reply to: Ross33


@Ross33 wrote:

I am having some issues concerning updating drawings.

...

If nayone knows why this is happening I'd love to here.

 

Thanks,

Ross.


IMO the simplest thing you can do for the answer is attaching your IPT file here, as JD asked.

Please mark "Accept as Solution" and "Like" if my reply resolves the issue and it will help when others need helps.
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Message 20 of 27
Myles1
in reply to: BeKirra

We actually use iParts quite often with success.  Some times, however, there are issues with drawing views updating when an iPart has been updated, after the view was placed in the drawing.  The thing to remember is when you place a view of an ipart, or a view including an ipart, the view is referencing one of the members.

 

Make sure the member you want to be updated in the view is either checked out (if you're using Vault) or not set to read only.  Once the member can be generated (right click-generate files) the member in the view will update.  You can re-generate the member all you want, but if it is read only or not checked out, it will not update.

This works for us every time.

 

Hope this helps.

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