Inventor 2019 & 2020 projected geometry linking issues in assemblies

[jimmygunz37]

Hi,

I have been working on Inventor since 2006 (and AutoCAD since R1). I feel that the program was optimal (least buggy) in 2013.

Since i have upgraded to 2109 & 2020 i am experiencing many issues across the board.

- When working in assemblies - parts created within that assembly and projected from geometry from master part or previous parts has major issues with a simple/minor change. like to an existing depth or width of an existing cut. Which usually results in an entire 'trickle down' effect of editing parts sketches and features to accommodate a minor dim revision. This has forced me to (for the time being) to be using multibodied parts and it is a real PITA! especially when inserted into assemblies and using representations.

- leaving me with limited options at times (if they are available) - break link, or redefine (and even redefine isnt a help)

- i have researched, gone through all my options (cant seem to find anything checked or unchecked out of the ordinary), and have done an entire reinstall/repair of the software.

I dont know what changed or if options are required but the program seems less parametric than the 2013 version.

All in all, i have a huge list of issues (screenshots) and would like them to be reviewed and answered.

what would be the best way to do that as well? 

maybe they are all linked in someway to a specific option or something. but i am at a loss.

Please help.

James

[SBix26]

I'd suggest posting one issue at a time (in separate topics), and including screenshots, screencasts, and example files where possible.  In my experience, multi-solid master modeling is far superior to adaptive assemblies with cross-projected geometry, so I suspect it's a simple misunderstanding on your part that makes it so tedious.

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[Cadmanto]

You mention you started using Inventor 2006 the jumped in mentioning versions to 2019 then 2020.

Did any of these parts/assemblies originate in 2006 then you started opening them up in 2019 then 2020?

If that is the case, that might speak to some of your issues.  A lot has changed in 13 years.  Upgrading versions usually works best when doing it in smaller increments. 

Windows 10 x64 -16GB Ram
Intel i7-6700 @ 3.41ghz
nVidia GTS 250 - 1 GB
Inventor Pro 2020

[jimmygunz37]

a simple misunderstanding on my part? interesting... because it seems to be
isolated to 2019/2020 that this 'misunderstanding' happens. So i am
assuming it has to be an option that is off or not a standard on the
install.
yeah i stated i have multiple issues; but i am explaining only one, so a
decent answer from the 'experts' would be appreciated; and not the general
assumption that 'I' the end user is incorrect on this point. I have worked
on many large assemblies and do extreme custom design for fabrication all
day (across many disciplines) on inventor for about 14 yrs (including the
Barclays Center facade, World trade center memorial museum facades,
billionaire's houses interiors, major brands flagship stores across the
nation, etc). I do not claim to be a pro on any design software because
there is always more to learn; BUT i have had many unanswered questions by
autodesk professionals who instead of diagnosing the issue or recognizing
issues/bugs within the software say it the end user error.
send me a direct person or persons that i can be in touch with and will
send 6 months worth of screen shots (probably about 30-40) with the
problems called out and have them diagnose and/or see if they are all
related. I would accept a possible 10% probability that some may be my
error or means & method of building, but not all.

Thanks in advance for expert help.
James

[jimmygunz37]

NO, all assemblies and parts created in 2019 & 2020.

i did mention that i still like 2013... and 2006 is when i started. 

i have worked on almost all versions since 2006... 

when the program was updated every few years it worked, when it started updating every year there was a increase in program issues.

Also, try working on the Barclays Center steel & facade, the World trade Center steel and facade, or the plethora of other high rises i have done, or the ever changing flagship stores interior with a system of components/displays and only use multi bodied parts, aint happenin (efficiently).

[SBix26]

Can you give any more coherent, detailed account of the problem?  Or an example assembly that shows the problem?  I, at least, do not yet understand what used to work and doesn't now, though it seems to be related to an adaptive workflow.

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[jimmygunz37]

workflow,
start assembly.
create master part (with all detail features) as 1 part at the top level of
my assembly.
create production parts using the master part by way of projected line work
in sketches (within the assembly on 2019/2020)
part to part sketch have projected line work (and usually are from previous
parts).
1 minor change to EXISTING feature on top level (master) part and many of
the parts lose adaptivity/projected linework links. like small depth of
cut, or width of dado.
have to go through and edit almost all sketches on all parts to efficiently
manage the errors created by 1 change.
sketches require planes to be redefine (if even available in the drop
down), projected geometry all magenta (showing the lost link) and either
requires redefining of that linework/re extruding to recognize the
'redefined' linework, or i redraw and have to re define the extruded
profile (expected when redrawing)
other option is to break links, and that is a last resort or when i am at a
point of finalizing for cnc/laser fabrication; but that can potentially
cause errors (if further modified) for my final output files as i have to
check everything more thoroughly because there is possibility that holes or
parts dont line up, etc.

[SBix26]

OK, I think I follow.  But without example files, I don't know how we're going to diagnose the problem.

However, if I understand correctly, you're modeling your components in a master part, inserting that part in an assembly, then creating components again by adaptively projecting sketches in the context of the assembly.  This seems like a very inefficient and fragile workflow.

Here's how the workflow goes for me:

• model parts as separate solid bodies in master part
• derive each solid to a separate part file
• assemble the parts in an assembly, all grounded at the origin (except those that need to move)
• make changes to the master part as needed, then update the assembly-- all changes are made to all components.

The advantage of this method is that there are no adaptive relationships to break; derived parts are much more robust than adaptive parts.  The lines of dependency are perfectly clear: assembly is dependent only on its component parts, which are each dependent only on the master part.  Also, the Make Part and Make Components tools ease the tedium of creating the derived parts and assembly.

Does this make sense?  Or did I misunderstand?

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Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[jimmygunz37]

i think i understand your method, but dont know how that can work
efficiently (or may not fully understand).
I have worked and made parts outside of an assembly, but that is mainly
when they are not a 'dynamic' or adaptive part. Like a piece of hardware.
But if that hardware is inserted into an assembly (physically constrained)
and i cut a hole or rabbet to accept it in another part. when i change the
physical constraint the hole should move too.
I build all of my contained within 1 assembly.
lets say for instance, a table.
I make 1 part that is the basic overall of that table and turn it to glass.
all the (fabrication) parts are created using the master for projecting
line work to create parts. all machine fab parts for Legs, table top,
blocking, skirt, leaf, etc...
i guess it could be fragile working if the program doesnt like it; but this
is simple parametric/adaptive stuff. I didnt have these issues (or at least
only 5% of them) when working on earlier versions (2014 being the last
before i started using a fresh version/comp with 2019).
i can bend/change my workflow to 'adapt' to the program, as it wouldnt be
the first time. But i am wondering what has changed on inventor that
suddenly it has become more notable and my workflow now no longer works
well.
again, before this being an issue user error (that is now not as effective
with the 'upgrade' and working in 2019/2020) maybe there is an option
within the program that is hindering cross ref geometry? maybe adaptivity
option somewhere that is new?

[jimmygunz37]

some screen shots of past projects.

[jimmygunz37]

Working on this panel right now for production.

besides the hardware, the items i am working on is basically the MDF face and the Ply (which is a mulitbodied part), & the bender board (projected off the MDF rabbeted face.

i just changed my rabbet for the bender board from .375" to .3" on the MDF face, by adjust the 1 sketch that is for the half moon rabbet (which is isolated because it is 1/4" more than the rest of the rabbets on this face. 

It then somehow knocked out a few of my radial blocking, it made the center rib (which is its own solid within the multi bodied ribbing part) at the bottom turn into a huge block and bust through the side of the panel , and a few other items... now i raised the EOP and addressed each issue, and sometime even just opening the sketch and closing, or editing the feature (but without doing anything) and then hitting ok updates the assembly... even the error management doesnt make sense (not even fixing anything at times, as i am pretty good at knowing what will pop and error and how to fix or worst case redo something with minimal issues), like its a bug in the program and it doesnt update through all the parts, or chokes until you revisit the sketch or feature and say 'hi' to it.... its ridiculous

[SBix26]

We probably need to hear from the Inventor developers or other Autodesk employees, but I believe that some things in Inventor have been "tightened up" over the last few releases to prevent certain kinds of corruptions from being created, so it's possible that Inventor is not as forgiving as it once was.  I can't think of any options that you could change to set it back to a more forgiving behavior.

I'd like to demonstrate the Master Modeling (or Muscular Modeling) approach with actual files.  Can you zip and attach the assembly and files that you show in your most recent image?

---

Sam B
Inventor Pro 2020.1.1 | Windows 7 SP1
LinkedIn

[jtylerbc]

Not sure this is practical (you'd need to still have some old versions installed), but it would be interesting to see an identical process followed in both an older and a current version, and see it work in the old and fail in the new.  Without that kind of supporting data, it's easy to dismiss complaints like yours as being user error, even though that may not actually be true. 

It's possible there are some bugs that have crept into the adaptive workflow.  It's also possible that you have some bad habits, but got lucky in the past and got away with them.  Or that you've let some good habits slip, and now you're making some errors that you didn't make previously.  We can't really know for sure what's going on without seeing examples of exactly what you are doing.  

I used to be a fairly heavy adaptivity user, but found multisolids, deriving, and parameter linking to be much more reliable and stable.  I still use adaptivity occasionally, but it is pretty infrequent.  I have used Inventor a similar amount of time as you (started on version 2006 or 2007).  In my experience, adaptivity has always been a bit tricky, and can be very unstable if not set up well.  At my company, it is jokingly referred to as "Black Magic".

I'm still stuck running 2018, so I wouldn't be able to see your specific files, but I would still suggest posting a simple example so that it can be looked over and suggestions made.  Doesn't have to be something from a real project - just a sample file set that exhibits similar behavior.

A few general suggestions I would give:

1. Use the least adaptivity possible to achieve your needs.  
2. Don't do anything through adaptivity that could be made associative in another way, such as through linked parameters.  All the other methods are more stable, so use them when you can.
3. As much as possible, try to reduce the number of different parts linked together through adaptivity, in favor of linking multiple parts to the same source.  Your "master" part is likely already pushing you that way.
4. Parts that are going to be adaptive should typically have their positions clearly defined with constraints, in a way that isn't affected by the adaptivity.  Vague positioning and adaptivity are a recipe for disaster.

Since you're already using a master part, there may be an intermediate option between adaptivity and multisolids.  Have you considered deriving sketches instead of projecting geometry?  That might be a bit more stable than what you're currently doing, at least in some situations.

[johnsonshiue]

Hi Jimmy,

I really want to help. But, I have hard time following the exact issues you are having. Please share an example here or send it to me directly ([email protected]). I am more than happy to take a look and understand the behaviors better. Based on my understanding of how things work, the workflow you are using remains unchanged. It is possible some settings (Tools ->App Options -> Sketch or Assembly) are not set to your desire. I need to see the files.

Many thanks!

[jtylerbc]

@jimmygunz37 , I'm not all that familiar with your terminology (my world is steel fabrication and a bit of hydraulics).  But I've produced some things that have some similarities in shape to what you show in your "screenshot for acad forum.png" image, even if the actual function is very different.

As I mentioned in my previous post, I'm still running 2018, so I can't see your files if you post them.  However, I can post files for you to look at.  I've attached a sample model that was culled from a training example I created a while ago for demonstrating multisolid modeling to new users at my company.  This is a "saddle", used as a transport stand for a pressure vessel or other cylindrical object.  It involves several flat plates, and one rolled piece (modeled as sheet metal so a flat pattern can be generated).  The model is set up to automatically maintain geometric relationships between the parts, but uses absolutely no adaptivity.  

Edit the "Layout" part, and then update the assembly.  The individual plates and the assembly will then pick up the changes you made.  This is a fairly simplistic example, but the technique can be much more complicated scenarios as well.  Note:  Pay no attention to the BOM from this assembly.  I stripped out some iLogic code before posting this, so plate thicknesses, dimensions in descriptions, etc. will not update to your changes.  

Edited:  It's late and I'm hungry.  The consequence of this is that I forgot to actually attach the example file I was talking about.  Fixed it now.

[jimmygunz37]

I am sorry i cannot, as these files are riddled with the client name and
are not released to public. i figured i would give a shot to reaching out
to the experts due to the email i received for the 1 day of feedback.
as far as inventor being 'forgiving' in 2006 you couldnt do a whole lot
without it kicking you an error, and in 2009 it seemed that lower level
parts on the timeline were allowed to be used for reference back up into
upper level and was necessary for adaptive productivity building.
Otherwise, you have to know exactly what/how you are building before even
starting. To me thats NOT parametric/adaptive drawing.

if you have a document or something that you think can help my workflow, or
a better process, please send me a link...
thanks for your help,
James

[johnsonshiue]

Hi James,

Please share your files with me directly on a cloud drive of your choice ([email protected]). Inventor does not have Timeline. Inventor uses browser.

Many thanks!

[jimmygunz37]

FYI,

looked up workflow for large assemblies and the method i have described i have been using is stated by Autodesk as being the most practical and stable... 'Top-down skeletal modeling' is the proper term... see for yourselves - https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2019/ENU/Inve...

And apologies i said 'timeline' instead of 'browser'... i know what it is (and seems so did you), was referring to the browser in chronological manner.

Now what i constantly see is someone asking for sample files.. if there are settings on my machine screwing up, you wouldnt see the issues; and yeah i guess then would have a control to work from... but until you assume i know what im doing (not just getting 'lucky' - as i dont think i would be trusted to pioneer 7 & 8 figure fabrication jobs from conception to installation) and something is amiss and/or has changed since 2013/2014 versions... adaptivity and having to backtrack all the way into sketches of each part to reset, redefine, or jump start updates to take is a/the problem that i didnt have in previous versions to this extreme or extent... i believe i have all adaptive options checked and dont know what other things may be affecting... and for now lets assume my workflow and parts are not the issue and lets see what suggestions come about, or any others that may have the same issue.

[jtylerbc]

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@jimmygunz37 wrote:

FYI,

looked up workflow for large assemblies and the method i have described i have been using is stated by Autodesk as being the most practical and stable... 'Top-down skeletal modeling' is the proper term... see for yourselves - https://knowledge.autodesk.com/support/inventor/learn-explore/caas/CloudHelp/cloudhelp/2019/ENU/Inve...

That article isn't wrong.  However, it is written in such a generalized way that it doesn't address the multisolid technique we've been mentioning directly.  However, it is implied.  The section about "Skeletal Modeling: Single-Part" mentions "Use Derive and projected geometry to create parts and subassemblies.".  

The multisolid techniques that have been mentioned are based on the Derive method, so they are one method for doing what is described in the article.

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@jimmygunz37 wrote:

Now what i constantly see is someone asking for sample files.. if there are settings on my machine screwing up, you wouldnt see the issues;

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That would be a reasonable thing to consider if such setting existed, but they don't. Settings for adaptive projected geometry are either turned on or off.  There is no option below that to make it any more or less stable.  If you are getting adaptive geometry in the first place, the relevant settings are turned on.

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@jimmygunz37 wrote:

but until you assume i know what im doing (not just getting 'lucky' - as i dont think i would be trusted to pioneer 7 & 8 figure fabrication jobs from conception to installation) and something is amiss and/or has changed since 2013/2014 versions... adaptivity and having to backtrack all the way into sketches of each part to reset, redefine, or jump start updates to take is a/the problem that i didnt have in previous versions to this extreme or extent... i believe i have all adaptive options checked and dont know what other things may be affecting... and for now lets assume my workflow and parts are not the issue and lets see what suggestions come about, or any others that may have the same issue.

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You seem to be taking the questions about your workflow a little too personally.  We're not questioning your workflows because we think you're incompetent.  We're questioning them because the adaptivity-destroying options you keep mentioning simply don't exist, so the problem has to be somewhere else.  That leaves pretty much leaves two possibilities:

1. A problem with your workflow.
2. A change to the software.

We (the users on the forum) can't do that much about the second, so we tend to focus on the first.

[jimmygunz37]

2020 seems to be the issue as i am seeing it... just worked on 2019 for weeks/months without a crash or geometry linking issue on 'small' 100 part displays/cabinetry... i had to work on 2020 for a few components and built them primarily as a multibodied part as i know it helps because it essentially eliminates cross part failure issues... but within 4 hrs of working on a fresh file, it crashed 3x... and now a few weeks later having to make 2 minor dimension adjustments of 1/8"; 50% of parts (including content center parts) not in the multibodied part either have physical constraint issues or projected geometry issues in the sketch (like 1/16" off)... which BTW is BS... all options for adaptivity and cross part reference are on... so had to rework, redo, error manage the hell out of jigs and constrained parts... it is really a joke that this program has 'evolved' to be less than what it was... now i know someone above said they may be focusing on improving other areas of the program... that is kinda funny, being that i still see such pain in the ass issues that happen like every 2 mins of modeling that really cause workflow/speed to suffer - like selecting a profile to extrude, then switch to a cut, and somehow it always tries to cut air/opposite the 'solid', when i would think the program should be intuitive enough to know it should flip (used to be)... and that seems to vary like you hit the flip first, then then hit cut, it goes backwards and always does some idiotic alternative... or when patterning features they always tend to be opposite of the solid.... and there are many more little issues like this that are now in the new and 'improved' 2020 that werent as prominent as with prior versions... maybe they should focus on things like that and core program function prior to upgrading and expanding advanced functions.

I have designed entire highrise building facades with 1000's of parts/assemblies over months & years of being  engineered prior to fab, client revisions, asbuilt conditions, etc in earlier versions and have had less issues. I couldnt imagine having to error manage those builds in 2020.... smh... GREAT JOB AUTODESK! F 2020!