Help, does inventor have a function to create a sub assembly from parts in my assembly, a bit like the functioon make component from sheet metal

[engineeringGYNTN]

i have a question regarding assemblies.

does inventor have a function to create a subassemblies from parts in my assembly, a bit like the functioon make component from sheet metal.

i know it might be a triky one, but i heard solidworks has a function like it.

i have a big assembly of a steel frame for a barn and within i have:

- a frame generator, with ~27 steel beams.

- flanges to conect the beams. the amount of flanges comes to some where in the 100ss, the flanges are drawn inside a multibody part and made in to parts using sheetmetal-->makecomponent.
   some flanges are places seperately, and most are place with (circular)paterns. 

see a screenshot of the feature tree and assembly down below 

i want to make weld assemblies from each beam with their flanges. 

for this i normale export the beam with its flanges with[sheetmetal --> make component] but this only works in a part. and in a part i cant use frame generator.

also i use a ilogic that takes the part project number, assembly number, part number and part name, from the file name and places them in the information table in the bottom of a 2d drawing.

the weld assemblies are neded to make 2d drawing's to start fabrication. 

some things i was thinking about to solve the problem where:

- make 27 diferent level of detail.  ----> this would take a lot of time, and when making 2d drawings file names wil have to be put in again. witch doesnt work with the ilogic i use to fil in the details of the 2d drawing table. 

- some coleges colleagues sugested demote. but that wont work with the paterns. and doesnt create a new assebly file, to my knowledge.

anybody have any ideas?

if you need more information about the situation,

or more images from the model, feel free to ask.

Thanks a lot!

[ndion3644]

I'm currently facing a similar issue.

I can't demote any parts in my frame generator assembly that have been reused since Inventor sees those parts as patterned.

One workaround may be to use the "Simplify" function to create a multibody substitute part of your top level frame generator assembly. It is possible to use the solid body substitute part to push each solid body back into a standard assembly (non-Frame Generator assembly).

[ndion3644]

I should have mentioned demoting does create a new assembly file.

[cadman777]

Doing structures with Inventor is very difficult compared to using structural software.

Using the framegenerator (FG) is very difficult due to sub-assemblies and documentation. There are pros and cons with FG. I think there are more cons than pros. There's a lengthy thread (can't find it now) from about a decade ago discussing this. The biggest problem with demoting FG members is you can't UNdemote them. So if you have to make any changes afterward, you're screwed, esp. if you already have weldment drawings already detailed. That's the biggest reason I don't use the FG when doing structural. I use FG stictly for pipe railings. And even then it has 'issues'. So when I do use FG, I create all baseplates and other connecting plates as custom sheetmetal parts. But I believe the FG could be useful if you have iLogic to solve the problems.

Another option that some in here use (there's some threads I can't find now, but I believe SamB does it this way) is multibody parts (MBP). I never use MBP due to sub-assembly and documentation reasons. But I believe MBP could be useful if you have iLogic to solve the problems.

The way I do structural is:

1. make the wireframe where all the main parts (structural members) go.

2. make a library of base plates, connecting plates, end plates, and all other standard platework that's easy to reuse as different variations of the basic part.

3. Instead of using the FG, I save the structural member as a Custom (ContentCenter (CC) part.

4. Then I derive the main wireframe sketch of the structure into it.

5. Then I reposition the structural member's base sketch onto the appropriate line in the wireframe so it's perpendicular to the direction of the wire. I usually put it at the center using a sketch point and WorkPoint + WorkPlane on which the sketch gets Redefined. The Start/End planes go on the ends of the sketch line. And I usually delete the system sketch that comes in with the FG part b/c it breaks most of the time.

6. Then I add any base plates, connecting plates, gussets, stiffeners, knife plates, or whatever is needed to that member in an assembly.

7. Once you have one member like that of one particular shape (such as a w-beam or angle or channel), you can easily copy it to a new filename and reuse it in another assembly doing the same thing. Then you can RMB on it in the assembly and change the size of it if need be. It's real quick to make the change, esp. if you already have a library of parts like that for reuse in new projects.

8. I do that for every sub-assembly that's needed (column weldment, beam weldment, cross-brace weldment, etc.). 9. 9. The good thing about this is, most structures use multiples of the same column main part as well as beams, purlins etc. So once you get one sub-assembly of a particular structural shape made, you can just copy it to a new assembly (iam) file and add or subtract 'attachments' to it as needed. So for example, if the corner columns are the same as the mid-span columns, you can reuse either of them under a  new sub-assembly filename and change attachments.

10. Then you can just reposition it in the assembly by re-Constraining it to the base wireframe sketch part (that's already inserted into the assembly).

11. One thing I use that main wireframe sketch part for in the assembly is as the Grid. On the 0'-0" plane in the main wireframe sketch I put the grid, and then 'Include' it in the drawing plan view.

12. Doing it this way saves me the headaches associated with sub-assembly creation and drawing production, as well as repetition.

13. One thing I forgot to mention is, if you need to make the main part members without using the CC, you can do as some in here do (can't recall the threads) and use a library of structural shapes in the form of Inventor Sketch Blocks. I could've used that technique many years ago on a number of projects had I been smart enough to think it up. Oh well!

Anyway, maybe that'll give you an idea of another way to do structural work in Inventor that saves time and effort.

[engineeringGYNTN]

I tried what you said,

i first made a simplified view of the assemly using: assemble --> simplification-->simplify view, [see image simplify test step1 ] 

this swiftly made a new view in my assemply and was easy to select the beams and flanges,(als when they are in a patern) you can just clickon em in your view.

at this point i tried 2 diferent steps:

-tried it with a second step in before making the 2d drawing--> i copied the new simplyfied view to a level of detail. [see step 2a] ----- result ---- when i tried to make a 2d drawing of this situation, i got a what i wanted to see, but when i inserted a BOM i could see every part in from the big assembly, (so close😁)  switching to the new levelofdetail also gave me a error [see image]

-create simplified part from the new simplified view: assemble --> simplification-->create simplified part. I selected the option to maintain each body as a seperate solidbody.. -------result-----when i tried to make a 2d drawing of this situation, i got a what i wanted to see, when i inserted the BOM it showed it as one part, and not al the flanges that are on it seperatly. a positive point was, that this function creates a new part and that works with the ilogic for the details on the information block on the 2d drawing.

both these options result in that i have to make the BOM manualy. i dont see that as a solution because this would take a lot of time, and is very prone to mistakes.

what im thinking of:

-create simplified part ---> is there a way to zoom in the BOM, so that the flanges become a seperate item?

-levelofdetail ---> is there a way to swiftly set al the supresed stuf to , BOMstructure--> reference, this makes it that they wil not be visible in the bom, but it would take a lot of time to do this for each part.

thanks for your time.

[swalton]

I don't have a good answer for your workflow request. 

I would avoid creating any new workflows that leverage Level-of-Detail.  Autodesk replaced LOD with Model States in the Inventor 2022 release.  

Per this post: https://forums.autodesk.com/t5/inventor-forum/model-state-frame-made-usung-fg/td-p/10237379

Model States do not support Frame Generator.

Anything you develop now that uses LODs will need to be updated or changed when you move to newer releases.

[cadman777]

FYI: I've tried to make Inventor do structural work for many years now, and it just isn't suited to it.

Instead, I have various methods for Inventor that work in various scenarios.

If you want a cost-effective solution to structural work, then you might try ParaBuild.

Give their demo a test run and see how easy it is to use.

If I did a lot of structural work, I would get ParaBuild instead of Tekla Structures.

I also demo'd Tekla's Educational version and found it has a huge learning curve and is way out of my price range.

Otherwise, I think you're going to have to find a balance between what you WANT and what you CAN do with Inventor, just like I have over the years. Let's face it, if out-of-the-box Inventor still doesn't have useful end plates, gussets, stiffeners, copes and blocking in the FG, then it certainly won't have anything useful for structural work for some time to come. I've been waiting for a DECADE, and still nothing worth talking about. The fact is, there's no money in it for  the Autodesk INVESTORS, so I doubt it'll ever get any priority in development. Besides, they already have Revit and AdvanceSteel. So WHY should they waste resources on Inventor for structural?

[A.Acheson]

If I get the request you want to detail sub assemblies that have been modelled in the top level assembly? You said you wanted to make weld assemblies, was there any operation in there that can’t be detailed on the drawing?

If there isn’t then design view representation I think is the correct workflow. This would avoid a redo of the work which generally comes with a redo of the model gets reused. You simply pick the parts you want to include in a sub assembly, ensure you try out the invert selection filters. Then create a view per this view rep in the drawing 

and then retrieve the partslist per the view rep. 

[engineeringGYNTN · Accepted solution]

Thx everyone, your responses help a lot, i came to a solution.

see the document below,

the document is in dutch because i wrote it so my colleagues can use it as well. 

[greysonjordan20]

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[greysonjordan20]

I am also faced same issue few years back, I overcome this by some procedure by searching in google and some forum pages.