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.
Attach files here.
The CADWhisperer YouTube Channel
Is your drawing set to defer updates?
ake sure your drawing view is set to associative.
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.
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.
@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.
The CADWhisperer YouTube Channel
@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.
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!
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.
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()
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!
I'm assuming you are asking mcgyvr, right?
I have seen the out-of-sync issue before, in fact we actually stopped using iParts after seeing that but coming from SolidWorks this is a must and we are thinking to give them a try again that's why I want to find out the work around.
You haven't seen or heard of any issues with iParts/iAssemblies? I tought this was a well known issue since even our tech support guy recommended us not to use them.
Thanks
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!
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.
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.
Not complaining, I really appreciate the help in this forum.
Thanks a lot
@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.
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.