Multi-Body Modelling

[DeanLong]

All,

I saw the TC topics recently and Multi Body modeling is still one of the topics. Before I get flamed by everyone for my thoughts, I have a few honest questions.

What is the big push to include this functionality to Creo?

Is it because Catia, SW and others have it and we need to be like everyone else? In other words, because of interoperability?

Is it that TDD is too: complicated, restrictive, confusing, "Add your own reason"?

What is the advantage to adding this complexity to individual part files that you cannot get from discrete part files?

I am interested...

This thread is inactive and closed by the PTC Community Management Team. If you would like to provide a reply and re-open this thread, please notify the moderator and reference the thread. You may also use "Start a topic" button to ask a new question. Please be sure to include what version of the PTC product you are using so another community member knowledgeable about your version may be able to assist.

[TomU]

I wonder if it's needed to fully support the unite capabilities.  How else would you reuse an existing multi-body part from another CAD system in Creo today???

[TomU]

I will say that from a file management perspective, it is very helpful to have a multi-body part represented as a single component.  For example, while a nitrogen gas spring, or hydraulic cylinder really is an assembly, if you're not the manufacturer you probably don't want to manage it as such.  It's much nicer to treat it as a single part number and single model in Creo (and Windchill) while still having the ability to manipulate it like an assembly (change stroke length, etc.).  Today you can do this in Creo, but you have to be super careful to keep enough of a gap between the different parts or they will instantly merge into one solid.

Frequently we will take purchased assemblies and combine them into a single model, just because we don't want hundreds of individual assembly components cluttering up things.  I don't really care what pieces a manufacturer used to create a conveyor (for example), I just want the finished conveyor as a single model.  I think it would be slick if PTC provided the ability to turn an assembly into a single multi-body part (and maybe even back again.)

[dgschaefer]

Aside from Tom's use case for assemblies that you'd like to track as a single model, I'v also sued multi body modeling in SW to create complex shelled parts. 

Imagine a box that's open on two sides with a center wall somewhere in the middle. Create two separate bodies, shell each and then merge them. 

I've been in many situations where I needed to shell partly from one side and partly from another. Being able to split it into two bodies, shell and then recombine would make that easier.

Or a part that needs to have two areas shelled at different thicknesses.  Model as separate bodies with their own shell features and merge them.

Once you have the option available, you can imagine things it'll let you do easily that having a single solid doesn't allow or makes difficult.

I do like that Creo treats a part as a single component.so I wonder if there would need to be a separate designation for an assy treated as a single item like Tom describes.

[DeanLong]

I concede those are pretty good reasons.

For the "multi-Shell need that you described Doug, I have just created quilts with offsets and then merged them. Granted each use case is unique and one technique is not the catch all.

I guess my original interest was concern over whether this added functionality would become, over time, the rule or the exception to the rule.

[huggre]

In my opinion, the lack of support for multi-body parts in Creo is a major problem.

In my company, this problem primarily relate to welded assemblies.

A typically welded assembly in my company (oil & gas) consist of hundreds of steel plates welded into complex steel structures.

As we do not do in-house manufacturing, we do not create individual drawings and part-numbers for the individual plates in the structure (only for the structure itself)

Without the support of multi-body parts, we have to manage thousands of models within our PDMLink system that really have no practical purpose other than slowing us down when doing activities such as: Add to/Refresh Workspace, Check In/Out, Revise, Promote etc.  

[JonathanHodgson]

That's a good use case.  For the most part I'm pretty content with the 'one part = one part' philosophy - but yes, I've occasionally tried doing (small) welded assemblies with individual parts, and it gets to be a pain with even five or ten 'sub-components'.  I've generally given up and accepted that it'll just be a single component, but I can see there are major limitations with that - such as wanting to do views of individual sub-parts on the drawing.

[dschenken]

Weldments are a vexing problem. If one presumes full fusion welding, then there is only a single part at the end. Even fillet welding without full penetration makes for an inseparable assembly, so the end product is still one piece.

I've thought it was better for certain weldments to build them as a single solid and just use datum curves to mark the separations, but this pushes the work of figuring out the welded shapes to the welding group. I'm fine with that as they are the ones that need to account for how much distortion they will introduce. Often this is not a popular opinion and people want the individual parts with no effort. I tire of developing a set of parts which will weld OK and have this supplier or that have differing opinions about what they see as an optimal solution - experts in fabrication coming to incompatible solutions? Go figure.

Do multi-body parts allow each of the parts to be a different material? Is there an internal name for each of the bodies that go beyond some feature name or manual grouping of features?

At the end some of those problems are with the tools that Windchill exposes. At some level every one of those separate globs needs to be tracked by the software.

[TomU]

At the end some of those problems are with the tools that Windchill exposes. At some level every one of those separate globs needs to be tracked by the software.

I would argue that Creo should be aware of them only and Windchill should not.  I want Windchill to see this multi-body part as a single entity.  In my mind, that's one of the main purposes.  Separate drawings could potentially be handled the way simplified reps are handled now - same model but different configuration.  I think if you need to start assigning different materials, you probably should be building as regular assembly.

[DeanLong]

This was one of my first thoughts when Hugo and David mentioned weldments. Would one get very lucky that every single part of the weldment be the exact same material? I am sure that would be case at times, but not always. Then one is faced with the age old scenario...model everything separate or model as just one, I.E. multi-body, and then deal with the fallout.

For my money...given all the advantages and disadvantages of all methods, from .prt, to.asm, to .drw, to WTPart, to WindChill et al...I use quilts in one model that I can solidify individually as required (or not) in order to create the main weldment. Layers are my friend for controlling the "screen spaghetti". I then PubGeom out the quilts to part files if needed and solidify there. Everything is parametric and updates with revisions in the main. This way I do not have to drag around the whole main weldment just to show small portions and/or areas of interest. Now, refs in Windchill can get a bit challenging as the part count goes up but I like having explicit files to allow me as many backdoor "trump" cards as possible. If the supplier just needs the main...they get one file. If they need specific info on a particular area I have options. If I need to detail a specific "weld" or special requirement, I have options. Parts of differing material can be addressed, I have options. Do you get the notion I like options?

My $.02

[sdesaulles]

If Creo included multibody parts they wouldn't be able to charge extra for the "Advanced Assembly" module. I was shown the functionality in SolidWorks and realised that all the skeleton model and copy geometry complexity could be eliminated, along with a £1000 a year to PTC to maintain the Advanced Assemble extension.

[dgschaefer]

Multibody in SW and skeleton modeling in Creo are not directly comparable.  Yes, they both are top down design tools, but skeletons with copy & publish geometry features give so much more flexibility.  I'm confident that I win enough business and save enough time to justify the expense of AAX many times over.

I've had projects that I only accepted on the condition that the client allow us to use Creo instead of SW because I didn't think we could meet their aggressive schedule without Creo's skeleton modeling tools.