Physical properties N/A when positional constraints selected

[GermVanDerBij]

We use a lot of phantom assy's which include positional constraints, for instance a boltset (includes the bolt, washer spring washer and nut) where we can select the needed clambing range (for example 6mm between bolt head and washer). This boltset includes an iMate which coresponds with an iMate in some sheetmetal part. The boltsets are placed automaticly in the main assy by means of an addin, where the user can select the clambing range prior to placing the boltsets.

I've noticed that my main assy, where I place around 300+ boltsets, takes a lot of time saving when there's a positional constraint selected. Over 10 minutes to save...... when setting all positional constaints to master, the save command only takes a couple of seconds. Due to calculating the mass and centre of gravety it takes ages to save.

Is there an other way for this boltset to get the same result. Automatic placemant is mandetory, we use a lot of fasteners 😇 for instance; the 300+ boltsets are placed (and constraint) within a minute, including setting the positional constraint!

At this moment we use 2020 inventor, but tested the same setup on a 2024 inventor with same result.

[mrB_Young]

I'm not 100% certain of the question, but ... are you saving the files often? Do you have to update the physical properties every time?
What if you disabled updating of physical properties on save?  Is the saving time then improved?
If so, what if you leave it disabled and update the properties manually when you're finished with the assembly, limiting the re-calculating to just a one time thing?

[SBix26]

Starting in Inventor 2022, Model States will do a better job for you than Positional Representations.  Assembly model states can include/exclude components, control Model States of its various components, and control constraint offsets, among other things.  The latter sounds like exactly what you need.  For different clamp dimensions of your bolt assembly, you would create a handful of Model States with the only difference between them the offset distance for the mate constraint between the bolt head and the nut, for example.  After you create one MS, you can use Excel to add the rest-- a bit more efficient than doing it the manual way.

That might give you some incentive to move to 2023 or 2024.

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Sam B

Inventor Pro 2024 | Windows 10 Home 22H2
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[Gabriel_Watson]

From what I read in this forum on similar issues, usually, the recommended first thing to try is to remove "Express mode." Go to Tools -> App options -> Assembly -> uncheck "Enable Express mode." This option is supposed to help boost large assembly performance by storing cache graphics in the top-level assembly, which prolongs saving times.

Another hint is to verify for any iLogic you could delete to test if your save time improves.

Another check would be disabling any Add-Ins you are not using (as many as possible) to see if external influences like that affect your assembly.

Finally, of course, the network speeds should be checked. I know your save times on Master are fast, but if the iMate somehow is tapping into the Content Center bolts/nuts that are stored in a network drive, maybe that is a weird path Inventor has to tread in order to compute the constraints under Pos Rep. Just a guess here.

[GermVanDerBij]

Thanks for the repleys!

We intent to update to version 2024 later this year and will look into the Model State option.

We do have an iLogic Rule that uses the mass and area properties. I've put a massage box in front of this to aske the user if they want to calculate or not. I delibartly done this by a popup, because they may not forget to do so. The user can decide to calculate only when they are done engineering. By this, we only have to wait one time on a slow save.

I'm still looking for a way to quickly check if the assy contains pos. constraints. Only if it contains pos. constraints, the message should appear. Otherwise the full iLogic rule can run whitout any problems.

In our layout we also get this message where you can click NO and go on, but clicking NO is faster then waiting for an hour or more.... 😜

Still find it a little odd that the master positional constraint is super fast, but with choosen positional constraint it takes forever...... What's so different between these two? When I add new/extra boltsets in master positional, Inventor also needs to calculate weight, area, gravety and so on, and then it's fast..... 🤔

[mrB_Young]

In these models with positional constraints, are there "a lot" of constraints?
I'm not sure where to draw the line for what counts as "a lot", but I have seen that when you have "a lot" of constraints in an assembly and all the underlying sub-assemblies, then things can get pretty slow when you start manipulating them.

I'm not sure how Inventor process all these constraints, but my guess it runs through all of them and checks them for every time you do something.  Quite possibly in series, which could explain why this is a slow process, if you have "a lot" constraints.

My practice is to constrain parts as they would be in real life using as few constraints as possible, while still limiting all DoF.
(when I say constrained as they would be in real life, I mean contact surface to contact surface, or centre axis of holes. I've seen lots of people that would place things x distance from this edge, y distance from that, and the place another part in relation to the last part with another x distance, y distance.  My experience is that this doesn't end well when assemblies start getting large)

I don't know if that helps in anyway - but this is what I've observed/experienced over the years.

[johnsonshiue]

Hi! The behavior sounds like a bug to me. If possible, please share the files in zip here or send it to me directly [email protected]. I would like to understand the behavior better.

Many thanks!

[GermVanDerBij]

Thanks for looking into the problem Shiue.

We currently run Inventor 2020.5.4 build 400 (with Vault 2020.3.8 build 25.3.22.0) and I also tested the behavior on a Inventor 2024 build 153 (without Vault) where I noticed the same behavior.

We do have our Content Center localy installed, no network path's!

[johnsonshiue]

Hi! Many thanks for sharing the files! I see the behavior now. This is due to the bolted subassembly (101.449.477.iam) having non-Primary PosRep active. Each instance mass prop needs to be computed once in the Primary PosRep and then in the non-Primary PosRep. If they are all in Primary PosRep, the compute will be super fast.

I think in your case, use Model State might be a better choice. PosRep is good for showing components in different positions but the actual component positions are computed on the fly on demand.

I tried a simple test. If I activate the "Low detail" Model State in the bolted subassembly and make 300 copies, the mass prop can be computed almost instantenously.

Thanks again!

[GermVanDerBij]

Thanks for your repley.

I think Model State is missing the point. We use the PosRep to quickly add a boltset to an assy with the appropiate offset, so the washer won't be in the middle of the parts. I don't see how Model State shows the bolted assy in the correct position!?!?

I know, when default PosRep is selected, my assy saves super fast, that's not the problem. The problem arrises when alternate PosReps are selected. It takes Inventor forever to compute the phisical properties. We saved a lot of time by placing the boltsets with according offset by means of iMates (fully automated via our Add-In), but lost this time when saving the assy they are used in.

I created a work around for our purpose, so the iLogic rule only fires in the assy it self and not in a higher assy and only when some iProperty fields are zero and/or the user anwsers a qeustion with YES.

But I still think de Phisical properties should be calculated just as fast as in default PosRep!

[SBix26 · Accepted solution]

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@GermVanDerBij wrote:

I think Model State is missing the point. We use the PosRep to quickly add a boltset to an assy with the appropiate offset, so the washer won't be in the middle of the parts. I don't see how Model State shows the bolted assy in the correct position!?!?

Exactly the same way that a Pos Rep does.  You can change the constraint offset for each Model State.  See my initial reply above.

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Sam B

Inventor Pro 2024 | Windows 10 Home 22H2
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[johnsonshiue · Accepted solution]

Hi! Indeed, as Sam mentioned here, you can override the constraint value or any parameter value in a Model State. The only thing a Model State cannot do but a PosRep can is to override Flexible status. Otherwise, Model States can do much more the PosRep. In your case, I think you will benefit from using Model State.

Many thanks!

[GermVanDerBij]

Thank you guys for getting me at the right path 😊

I added the different positions in the Model State. At first nothing changed, so I tried a new constraint and there my offset changed perfectly. Turns out, I had to delete my PosRep first for the Model State to work.

Now I have to figure out how to access this via the API, so my automated placement can work with the Model State. 😏