Level of detail 'failure' in drawings

[ONTRAK]

I work standalone (not vault), and each machine I design & is built is bespoke for the customer, this is usually additional brackets / water sprays etc as it is an underground mining machine.

So G.A. drawings / As Built drawings may evolve over the machine build.

I work with one level of detail in the master assembly and this is flagged with the most recent change / update

date  i.e. @ 30-11-2021.   a simple way for someone to find latest version.

I will disable / turn off 'visibility' & 'enabled' of components if customer has decided not to use them, save the assembly ensuring the date based name L.O.D. is the active level of detail.

I then logically, open the .idw file, and find everything that is not visible & is disabled in the .iam file IS STILL VISIBLE  ??,

and the added level of selection you have added to the .idw file browser for 'update model' one view at a time, instead of the global update button, spits it back and presents the message

"cannot update different L.O.D being edited"

even if there is no other  file open in the background of the current project, no other level of detail set - I delete older date named L.O.D.'s in the master assembly - and sometimes when I am adding a new view to the .idw file IT PROMPTS "CANNOT UPDATE DIFFERENT L.O.D. BEING EDITED" ??????   

Even when updating an existing .idw and taking the extreme timewasting exercise of deleting the views, purging the .idw file, closing .idw file, reopening and then re-inserting the L.O.D assembly views  can still fail.

WHY??????

Instead of concentrating on releasing new versions annually that are filled with problems / crashes/ and other issues   (or perhaps making changes to the program just to justify your employment) 

why not release every second year, a version (that is not a Beta version) that does not require updates / patches one week after release.   

If the programmers had to earn a living (on a item by item recompence) from the "little glitches ignored progamme" versions they release to the consumer (who pays a fortune for the 'privalege'?)   I think they would starve to death by the end of a week as they would have no income.

note that I do think 95% of the releases extremely good / functional - but fail in the little and most important details.

[SBix26]

You forgot one very important bit of information: what version of Inventor are you using?

Also, you forgot to "read the manual" regarding Levels of Detail.  They were never intended to be used as you are using them, they are (were) simply a memory management tool, especially back in the 32-bit days.  To turn off visibility of components, and maintain a variety of different "configurations", you need to be using View Representations, which allow you to save various states of visibility/invisibility; these can be used directly in the drawing environment to control visibility, and also to filter parts lists.

Or, better yet, move up to Inventor 2022, in which Levels of Detail have been replaced by Model States, and these will do precisely what you are asking, if I'm reading your post correctly.

---

Sam B
Inventor Pro 2022.2 | Windows 10 Home 21H1
LinkedIn

[ONTRAK]

Thanks

I use 2020 & 2021 as some suppliers / customers still using same, and makes
exchange of items easier and leaves them fully editable at the sketch level
UNLIKE stp , x_b, etc files

again I make the comment why a new version every year? For users like
myself it is time lost in download / install, migrate, load in my custom
files, learn the new functions, etc

when we are extremely busy and 2020 / 2021 does the job.

(or this is done on my own time)

Service pack update(s) in the interim year could change the load screen to
reflect a new version

eg next year your 2022 could display 2023 after an update, and have fewer
bugs, as it was not rushed to market.



Also your comment of "it was a 32 bit management tool" just highlights my
point that the little details are missed in the rush to outdo the opposition
and get the product to market.

Think most PC's have been 64 bit since 2010, and the 'management tool' is
still available in 2021.

Also I would probably 'Read the Manual' if the search engine took you to a
'user manual' description - not the actual 4652 results for Level of Detail
on the AutoDesk help page -

I do not have the time to explore all these for the answer I require.



Also I have done a few of the AutoDesk Accredited Training Courses, NOT ONE
OF THEM TAUGHT OPERATIONAL BASICS, no drawing sheet setup, Library
definition, etc, etc

I did on one of these courses learn how to take a pre-drawn Mouse body and
split it, add clips etc - all really useless in the industry I work in.



Regards John

[Gabriel_Watson]

FYI, your drawings load your model in memory as many times as the number of different LODs you use in different views. That sorta tells me you may need to double-check in the model if each and every LOD is saved there (switch to each one and save, ending on Master) before you open the drawing to update it.
I know it sucks, but when things go wrong (and thank the gods you don't have Vault to worry about), we need to work slower to find where the issue lies before we speed up.

I feel like your frustration could have been avoided if prompts were more informative of where the problem lies and how to fix them, instead of simply stating a "baby feels pain" cry. But it is what it is, and Inventor is not really your go-to software for very complex assemblies or workflows. We just stubbornly tame the wild horse to our fights.

[SharkDesign]

Are you previously a solidworks user? This is a common mistake for people transitioning and thinking that LODs are the same as 'configurations.' They are definitely not and should  be used in that way. Model States in 2022 was added to address this. 

As mentioned above, View reps are for showing different visibility of components and or colour alternatives. You can also lock these to stop new parts being added to their view. 

LODs no longer exist in Inventor 2022.

I personally think the updates, both service and yearly, at the moment are excellent. The Inventor team are working on 'Just Do It' features that are adding a lot of value to the software. Unfortunately some bugs will occur as Inventor is a pretty old piece of software now and it's very complicated to unpick the code to add in small changes as it can affect so many other things. 

If they are actual bugs, the team fix them pretty quickly. I have reported many bugs and had them fixed in the next release. In this instance though, it doesn't sound like a bug, it sounds like you don't fully understand the tool you are using. 

[johnsonshiue]

Hi! I believe you are leveraging LOD for Configuration purpose. For some cases, it may work well. But, for your cases with multiple levels of configurations, LOD may complicate things more. Like other experts already mentioned, LOD was designed as a memory management tool back in Windows 32-bit days. It unloaded files to free up memory, so that Inventor could load bigger assembly than 3GB RAM was allowed.

If I understood your requirements correctly, you may want to look into iLogic. Instead of managing configurations via LOD, you use a simple custom LOD (called iLogic or whatever you like it), then suppress the unwanted components using IsActive()=False. After you are happy with one variation, use iLogic Design Copy to spawn the variation (Replace Model Reference in the drawing accordingly). There are quite a few discussions on this process. You may want to take a look.

Many thanks!

[sundars]

Hi @ONTRAK 

LODs and drawings dont work so great particularly when you are documenting the same assy with different LODs in the same drawing document. 

(a) You could try working on one drawing at a time for each LOD

(b) If you have plenty of RAM and dont care about suppression, copy your LOD to a view representation and use ViewReps to document. That will get over the "cannot edit lod when its active somewhere else" issue. 

Thanks

-shiva

[gcoombridge]

I'll just add to the above comments by saying that a useful way of thinking about this is that Level of Details exclude suppressed parts from memory to increase performance. When you have an assembly with an active LOD open it is excluding certain components, then you open an idw with a different LOD it is trying to include them. As the files are referenced across the application and not only by the document, this causes the clash (the software is being told to do two mutually exclusive things at the same time). You can either persevere or improve your workflow by:

• only having EITHER the idw or the assembly open at a time.
• Right click on each LOD in the browser and select copy to view rep. Then use view representations going forward.
• consider using IAssemblies to build configurations for each customer (this may get out of hand).
• build a base assembly that will not change, make the BOM status phantom, add it to a customer specific assembly with additional sprayers etc...
• iLogic copy the assembly for each customer and make necessary additions.
• Upgrade to 2022 for model states.

You sound like you're using LOD's as a revisioning tool also? This would seem a bit limited to me as it can only by nature capture components that are included or excluded. Parameter changes in individual components, assembly constraints etc... will not be preserved.