DWG 'Update model' lather/rinse/repeat repeat repeat repeat.. and then repeat

[DavidWHouse]

I apologize if this is duplicative: I could not find a post that seemed sufficiently on-point. 

When I change almost anything about a sub-assembly of an assembly shown in a drawing (DWG), or in a part which is 'of' an assembly shown in a drawing, I often get the yellow lightning bolt, and and the right click menu features 'Update model'.  Then, too often, the round robin begins: select the indicated menu option and the offending assembly/LoD is loaded... And then it seems that almost regardless of what sequence of steps I follow thereafter to update the offender and save the new state of the DWG and IAM(s), I face an apparently patternless sequence where, on returning to or re-opening the DWG I am told that the same or a different sub-assembly needs updating. I have tried everything I can think of, including: using the either the small menu button either as 'local update' or 'global update' (and how do these differ, exactly?), rebuild all, rebuild all/update mass, etc.; updating the sub-assembly, saving and closing it, then returning to the DWG and saving it; updating the sub-assembly and saving it, then returning to the DWG and saving and closing it, then closing the sub-assembly and re-opening the DWG; and on and on and over and over.

Then, after a half dozen or a dozen rounds of this, perhaps because I have turned around three times and made a magic sign, it all seems to work, and the dreaded lightning bolts are held at bay. But not conquered, apparently, because not uncommonly everything will be well for a period, and then I will get the dreaded bolt on a sub-assembly were, as far as I can determine, I have changed nothing; but usually this involves a sub-assembly about which Inventor previously complained.

Making changes to iParts is particularly troublesome in causing this sort of not-so-merry-go-round. "Defer updates" is not checked.

So, what is the difference between 'local' update and 'global' update? What is the difference between those two and using 'rebuild all'? And most importantly, what exact sequence should I follow to put a stake through the heart of the lightning bolts, forever and anon, and why?

Inventor Pro 2018, all updates patched in, Win 10-64, etc.

[johnsonshiue]

Hi! I think I know what you are talking about. It is related to how Inventor updates geometry and files. First of all, Rebuild All should not be needed. The fact that you have to use Rebuild All to fully compute everything, there is a bug. If you have an example showing the need to use Rebuild to bring everything up-to-date, please let me know. Let me explain a bit the relationship between ipt, iam, and idw/dwg. An ipt file is a self-contained unit contains the geometry and all the data to create the geometry. Generally, an ipt file can be referenced in an iam file. The ipt file isn't aware of where it is referenced. An iam file is like a wrapper, pointing to multiple ipt and iam files. The iam file does not contain any geometry. Most importantly, it stores BOM table and the link to individual part and assembly files. The biggest difference between iam and ipt is that iam file can reference another iam fle, which also references yet another iam file. This can go on forever. An idw file is like a snapshot of an assembly or a part in a camera. It stores associative drawing views. When the geometry in the part has changed or the component changes position, the drawing views update accordingly. To put their relationship in a line, it is like Part -> Assembly -> Drawing. To have drawing view up-to-date, the assembly need to be updated. Before assembly is updated, the part needs to be updated. LOD is a memory management tool. It helps reduce the memory footprint of large assemblies back in the meager 3GB RAM 32-bit Windows days. Without LOD, Inventor users cannot build assemblies with more than 500 parts in those days. However, some users started to use it for configuration purpose, meaning one assembly represents multiple states or multiple designs. It works to certain degree but it is not meant to be a configuration tool. The trouble is that although each LOD can represent a given assembly in a different state, most of the update process still requires the assembly in Master LOD state. However, an assembly is only one file with one data stream. The changes in two different LOD states cannot be saved at the same time. You will have to close one of the document window and release the memory taken by one LOD state. Then save the change in the remaining LOD state. To properly update an assembly, it is better to activate Master LOD and update in the state. In drawing, if you need to use LOD, it is better to keep referencing one LOD state within one given idw/dwg file. Regarding iPart/iAssembly, they are best used as library components. They need to be authored and generated. Then store in the library for referencing. If you need to make change to iPart/iAssembly factory, make sure you generate the member files afterwards. In general, it is best if you can keep everything up-to-date. When a part is edited, all the assemblies referencing the part will need to updated. It is because the change in part (geometry) can lead to change among components within an assembly. I am sorry I have to write this long email. This is not a simple topic to discuss. There is definitely room for improvement. In the past, any change in a part or a subassembly would propagate. Now, only change affecting geometry or design intent would prompt the users to update. If you see unreasonable update request behavior, please let us known. Many thanks!

[DavidWHouse · Accepted solution]

Johnson, Thank you for taking the time. I appreciate. The explanation reiterated a number of things that of course I already know, but provided some additions as well. One small point: as I said, I am seeing the behavior in DWG, not IDW drawings. You say "If you see unreasonable update request behavior, please let us known." That's exactly why I posted, and I think that you were implying that when I 'Update Model" I should at some point choose the Master LoD, update and save the assembly/sub-assembly with that applied. I will try that. Even so, beyond that, I appreciate a clear suggestion regarding the best sequence of steps when eliminating yellow lightning bolts, or information about what best practices might prevent them from appearing, as they seem to do so often for me.

[johnsonshiue]

Hi! For Inventor, idw and dwg are equivalent. The major difference is that idw cannot be opened in AutoCAD, while dwg can be opened in AutoCAD without conversion. Another difference is that dwg can contains AutoCAD block definition but idw cannot. Besides these, there is no difference in idw and dwg and how the drawing views are updated. Regarding updating drawing views referencing assembly in non-Master LOD state, there should be best practice documentation on Autodesk Knowledge Network. You may want to search it. In general, when you modify an assembly, you want to make sure the top-level assembly is up-to-date per Master LOD. An optional step is to check "Prompt to save recomputable changes" in Tools -> Application Options -> Save. This will ensure the all the affected files are saved after they are updated. After the assembly is up-to-date in Master LOD, close the assembly. Lastly, open the drawing, update, and save. Please feel free to share an example if the update behaviors do not make sense to you. I am more than happy to take a look and see if there is a logical reason to the behaviors. Many thanks!

[DavidWHouse]

So, I have been trying this process, based on the information you provided: When the DWG wants a model (assembly) updated, I use the provided menu option. That loads the assembly in question, with the specific LoD used in the DWG applied and active, then returns me to the DWG as the active window. I select the tab of the assembly/model to be updated, select the 'Master' LoD, and save it to disk.

As such, I have accepted your response as a solution.