Weldment in different Levels Of Detail

[Anonymous]

Hi everyone!

here's the problem:

i have a few noozles of a similar type, with a range of diameters, and i want all of them in one assy.

So i made an assembly and a rule that activates a certain LOD in accordance to parameter change.

I also needed to place a welding between some elements in the assy as shown on the screenshot.

so i've placed it and switched toanother LOD, and to my surprise it disapeared!

i've tried to suppress weld seams in diffferent LODs - but they're not connected anyhow((

also i inspected Rule manager - whether there are any parameters that can control welding - but no, none of them!

so what should i do now to have my welding in different LODs??

Inventor_pro_2015

[Anonymous]

i'm just wondering - does anybody know how to solve this problem?

or question's not correct?  or i made a mistake with the forum branch?

[johnsonshiue]

Hi! I am not sure if there is a supported workflow here. LOD is a memory management tool, not a design altering tool. In theory, assembly constraint and assembly geometry should not be affected by change in LOD, since cached geometry is used to compute assembly constraint or feature in LOD when a part is suppressed (unloaded).

I suspect one of the weld beads is created on cached geometry in one specific LOD state. When another LOD is active and the cached geometry is no longer available, the weld bead fails to compute. Could you attach an example showing the behavior here or send it to me directly ([email protected])?

I would like to understand the behavior better and see if there is a better workflow to fulfill the requirement.

Many thanks!

[Anonymous]

Hello John!

thanks for your answer,

i'll surely send it to you, but not earlier than om monday, cuz it's in my office, and i'm not sure that i'll reach there till the end of weekend.

as for using LODs to have different designs of one assy - well i decided to do so because when i used an "is.active"command in ilogic rule to suppress some parts - i had to write such a long rules, and with the LOD - it's only couple of lines...

i'll send you an assy, on monday, i hope, and i'll really appreciate whether you'll tell me a better way of doing it.

thanks again!

[Anonymous]

Hello again Johnson! 

sorry for a little mess with my accounts, didn't thought that I had two of them,  but now I figured it out! )

so I hope you'll find the files in the attachment,  there are assy and part files,  and also an excel file that I use to mange the parameters from the outside. 

probably the flange plugs will fail to load,  cuz it's my own library,  but that is not the main issue I believe. 

hope to hear some recommendations. 

Alex M

[Anonymous]

Anybody? 

Any ideas? 

[jtylerbc · Accepted solution]

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@johnsonshiue wrote:

LOD is a memory management tool, not a design altering tool.

---

Johnson,

In general this statement is true, but mcsumkin is using the one exception I am aware of.  When you use iLogic's "IsActive" function to control design configurations, you end up with LOD's just like you would from Suppressing a part. 

mcsumkin,

 would it be possible for you to structure this with your welded-together parts as subassemblies, and have the iLogic code swap out the subassemblies instead of swapping out the individual parts?  I don't know if that defeats the purpose that caused you to set this up in the first place, but it seems like it would be a way around this particular problem.

[johnsonshiue]

Hi! The following two files do not exist in the rar file. Could you post them here or send them to me directly ([email protected])?

ИД_ЛиП_стенка.xlsx

Усиливающий_Лист.ipt

Thanks!

[johnsonshiue]

Hi! John,

"iLogic IsActive" is not much different than activating LOD and overriding occurrence count manually. It does not change the fact that Inventor can only support one assembly definition at a given moment (except iAssembly). If the design requirement is to document an assembly at a given LOD state only and have the PartsList reflected the LOD state, "iLogic IsActive" will help. However, it works only for the active LOD not other inactive LODs. If you have multiple LODs and you create views based on different LODs, PartsLists will not adjust accordingly. This is because there is only one BOM table within the assembly, from which the PartsList derives the data.

To support multi-variation documentation workflow, Inventor will need to be able to create multiple BOM tables and keep them up-to-date. Otherwise, the user has to create multiple assemblies or iAssembly.

Many thanks!

[jtylerbc]

All true.  I was thinking about his weld issue, and wasn't really considering the BOM implications of what he was doing.  I don't know how he's planning on using this, so it may not be a problem (he may actually want the multiple assemblies, and be using this as sort of a template).  I've configured some assemblies to work that way on purpose.  I think we would need more information from mcsumkin to know for sure if it makes sense for this situation.

That being said, iAssemblies may be a better way to go here anyway.  It's been a while since I've made a weldment iAssembly, but as I recall the welds either suppressed automatically when their parts were excluded, or you had the option to suppress the weld in the table (can't remember which at the moment).  That might be a cleaner solution to the weld issue than continuing to fight with the iLogic would be.

[Anonymous]

John,

Johnson, 

Many thanks to you gentlemen!

You made a really valuable remarks on BOM, because i'll definitely have to use it further.

I made a folder on my google drive, where i've placed an assembly with the excel "control" file, and sent a link to Johnson by mail. John if you either interested in having those files - i can also send you a link.

From my side I'll try to describe a problem here In a greater detail:

So, i have a cylindrical, steel (welded, and made of metall plates) storage tank. It has different openings on a side of a shell like manholes and nozzles. The set and qty of them may vary from one to another, as well as their diameter.

Each nozzle consists of: Shell (pipe), reinfocement plate, flange (or two, on the both sides), gasket, blind flange, and a bolted connection.

Flanges are welded to shell, as well as the reinforcement plate - you can see it on the picture i attachaed above, or if you'll reach the files.

I decided to make some kind of a universal assembly, that i can control from my external excel file, where i can specify things like diameter of the tank, diameters of nozzles, thikness of a plates that shell made of, and etc., and that in the end - could give me the final assembly with the set of nozzles that i need for a specific tank.

I made couple of rules for a nozzle shell and a reinforcemnet plate, to describe their behavior in case of nozzle diameter or a tank diameter variation (it wasn't very hard), and decided to have all the needed flanges, gaskets and blind flanges in one assembly to activate one of them, and suppress another in accordance to a parameters change.  

So when I'm switching LODs, nozzle shell and a reinforcement plate are still the same, so the weld seam between this two elements stays where it was, but flanges are replacing with another one - and welding there fail to compute.

After all, i made another assembly, in which i'm going to gather all the subassemblies of the nozzles and switch them "on" and "off" in the desired sequence, as well as specify their Location.

M.b. i should go the way that John had suggested, and create an assembly for every specific variant of a nozlle. but in this way i can't figure out how can i manage them later in the "fina" assembly. i mean switch them on or off, replace one with another.

wow - lots of text. Hope you could understand something!))

[jtylerbc]

I don't think I'm going to have time to dig into it far enough to need the files.  But one more thought based on your latest post - I've never used it, so I can't give much guidance on it, but I'm pretty sure there is a way to use iLogic code to change the active member of an iPart or iAssembly.  If you can look into that, you might be able to use it very similarly to your original idea of controlling LOD's with Parameters.  You would just be switching iAssembly members with Parameters instead.

[Anonymous]

Hi, John,

well probably you're right, and i have to use i-rules to change the active members of the assembly. I've tried a bit to assemble my nozzles this way yesterday, and finded out that ilogic can control "row changing" in iparts, but only for a "non-lirary" parts. 

In my case i use 50% of library parts, so i think my way is to create some assemblies with needed variations, and try to make ilogic to replace an assembly file in accordance to a parameter change - trying to figure out how to do it right now.

All this situation is upsetting me cuz - everything worked almost the way i needed it when i used the LODs changing, but now i have to invent something else. Discussing it with Johnson,  hope that he'll advise me something, because the LODs changing conception really brings a total mess into a BOM.

Thanks for an advice!

[Anonymous]

Many thanks to you gentlemen, once again.

As a summary i deсided to make a multiple subassemblies of the variations needed, to exclude possible problems with welding and conctraints in the higher level assemblies.