First Hands On with ST5 – Multi-Body

I was glad to download and install ST5 on my computer yesterday. It has been available for a couple of days, but I’ve been out of the office. My first impression of the download and install routine with Solid Edge was pretty good. The one hitch that I came across was that it looks like you aren’t allowed to have multiple versions of Solid Edge on one computer at the same time. Dave Ault mentioned that there is a way to make it happen, but it may not be an officially supported method. I’ll want to find out more about that. It would be nice to be able to run multiple versions, especially for comparison.

The first thing that I want to play with is arguably one of the most important changes in ST5 – multi-body.  For one thing, there has been this perception that SW has had an advantage over SE in multi-body modeling, and I’ll want to look into that to see if this new version turns the tables at all. If you are a current Solid Edge user, maybe you don’t make much use of the existing multi-body capabilities, and it might take some time for these new tools to catch on. There are a lot of uses for multi-bodies that don’t include trying to do assembly-type work in a single part. More on that later.

Solid Edge has had multi-body modeling for a long time. In fact, SE has had it longer than SW. SE handles multi-bodies differently, however.  Solid Edge uses the concept of Design and Reference bodies, where design bodies can be activated or deactivated, and only design bodies count toward part mass. ST5 adds the ability to have multiple design bodies. Body activation is a concept that doesn’t exist in SW. It’s like having the Merge option automatically on or off. Solid Edge’s implementation of bodies goes further, and some of the implications I’m not sure that I understand yet.

For example, under the Solids group in the Home tab, there is an Add Body option. This adds a Design Bodies collector to the top part of the Pathfinder, and the collector allows you to turn on and off the display of individual bodies. The image below shows the various states bodies can have in ST5. Design body, construction body, active body, inactive body. Design bodies are by default gray, and construction bodies are purple. Active bodies are opaque, and inactive bodies are transparent.

The part that confuses me is that to get bodies to show up in the Design Bodies or Construction Bodies collectors, you have to manually invoke the Add Body tool. Just extruding disjoint sketches doesn’t add a new body to the list, although it does add a new body on the screen. If a new body is created with the Split command, it is listed in the collector as a separate body.

This multi-body menu is another thing I like about Solid Edge’s implementation. It has separate commands for Union, Subtract and Intersect, with common names, and no cutesy crap. The SW commands are listed under Insert>Feature>Combine, and then within Combine you have to select Add, Subtract or Intersect. The Solid Edge way is just clearer and much more straight forward. Union, Subtract and Intersect are the words that were used to teach most of us the concepts of Boolean set math in geometry class.

One of the things I noticed immediately is that you can make fillets on multiple bodies at the same time in SE in both ordered and synchronous modes. This is something that drives me nuts about SolidWorks – some features such as fillets can only be applied to single bodies at a time, and when you have a lot of bodies that need filleting, you’ve got to find a different way of doing things. Hats off again to Solid Edge for coming up with a really practical way of working.

If you keep looking, you keep finding nice stuff. You can split one solid with another solid, instead of needing to make the tool body into a surface. That’s nice. That will save time when you need it. And when I say split, I mean split, not boolean. So if you have two solids that intersect, you can set one body to be the piece to be split into multiple bodies, and the other as the tool, and the result will be multiple bodies, not a single body with a chunk missing. There is also a set of default settings you can use to establish default behavior for hide/show. This would be like SW giving you the ability to control “consume” options (which they don’t).

The Split command has several options which let Solid Edge know how you want it to behave if the Split command creates a body that is not a valid solid. The concept of “manifold” vs “non-manifold” is not necessarily obvious. In essence, “manifold” means a set of faces that can be made into a solid without any zero-thickness conditions. This is something SolidWorks deals with very badly.

An example of a Split feature creating a non-manifold body is shown below. Here a rectangular block is being split by a triangular prism where the point of the triangle splits a face of the block. If the block were to split into two pieces (the piece inside the triangle and the piece outside the triangle) the piece outside the triangle would have a zero-thickness edge. Zero-thickness edges in CAD is one of those philosophical arguments that I never want to participate in. Some people claim zero thickness conditions should be allowed. But I think that’s silly. I think it’s just to cover up their embarrassment at not understanding or being able to visualize the problem. Anyway, in Solid Edge, if a split will create a zero-thickness edge (non-manifold condition), you have the choice to make it fail, or create two separate bodies. This is the correct way to look at the problem, from my point of view.

Something else I noticed is that in the ST5 What’s New, and even at some presentations at SE University last month, people seem to be advocating substituting multi-body parts for assemblies more than I am usually comfortable with. Granted, some of the reasons for not making assemblies within a part are different between history and direct modeling methods, with the direct methods removing some of the reasons to avoid it, but some of the arguments against confusing assemblies with multibody parts still exist. This is something I’d like to get reader’s comments on, if you’ve got an opinion. One of the reasons I argue against creating assemblies as a single multi-body part is that you have all of your feature histories tangled in one tree. If you are using Ordered modeling in Solid Edge, that’s still a valid problem, but if you are using synchronous, then it’s not a problem any more. With synchronous, you’re left with other arguments such as motion between parts, reusability of parts, part numbering/BOM/balloons, etc. as arguments against multi-body assemblies. There are still some valid uses for multi-body assemblies such as inseparable subassemblies, simplification, and purchased subassemblies.

There is a command called Activate Assembly Body. This is apparently used to tell Solid Edge which body to apply assembly features to when a multi-body part is used in an assembly. It looks like you cannot apply assembly features to all of the bodies in a multi-body part at one time. This just shows that an extra depth of thought went into implementing a wider use of multi-bodies.

And the last function I want to point out here is the Publish command. This has the functionality you need, with the ability to name parts and create an assembly. It doesn’t need to be more complicated than this. It just does what it needs to do.

One of the things I like best about Solid Edge ST5’s implementation of multi-body, and of SE generally, is that you don’t get the feeling that there are a lot of loose ends. I mean, this doesn’t look half-done (except for maybe the bit where disjointed solids don’t count as solid bodies). SW has 4 different ways to control inserting bodies into other parts that are almost the same, but different enough for it to matter which one you select. In the end, that’s just confusing. Solid Edge has done this in a much better thought out way, and has done it in such a way that they are giving the user a lot more control over bodies than the SW user has. I think that over time and more users banging on this functionality, more insight on ways to use it will emerge. ST5 is a significant stepping stone to whatever comes next. And of course you know that you can’t do surface modeling without having a robust method for managing bodies…




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  1. Matt,  Good review… and I’m looking forward to more of your insights on ST5. At lot of us here don’t have the time to explore these new capabilities, and tend to go right to the tools we already know, then start using new ones.

    Although I fully understand the definition of a MBP, my biggest question (and I’m sure there are others like me) is what’s a good example of a Multi-Body Part that shows the advantage of this workflow.


    1. Yeah, Bob, that’s a great question. It could be another post all on its own. This is where my experience in other software may start paying off, and I can maybe offer some answers instead of mostly questions. I’ll work up a blog post on applications of multi-body parts using examples from my work.

    2. Great question Bob….and I totally have the same thinking. Need SE to earn it’s keep first of all. Look forward to your new, more indepth, post on the MBP experience Matt.

  2. Bob the question is not to directly ask “show me the advantage”. Multi-body like any other feature is a tool and not a goal to reach. Learn how it work first then you will answer you question, not the other way around :-)

    Here some of my understanding as of now.

    When you start a project, you do not always want to commit to 3D. In many cases, you start from a plain 2D drawing  (draft or sketch)

    Design evolve and you need to start seeing some 3D. You can then use the convert to 3D if you have start in draft OR start extruding. At that point the multi-body will have a role to play to prepare your design for assembly design.

    Again design evolve and you need to start playing wit the assembly. This where you will use the publish feature.


    This will create a part-copy in the traditional section, keeping a link to the “Master”

    From there design continue to evolve and you need to separate the part-copy from its “master”, Either you move it to Synch or you break the link..

    Then you do in-context design at the assembly level. Synch will kick in to help you.

    My advice,  play with the tool and see where it fit in your design, Some time you only need a quick detour using the multi-body to resolve a design task ( Phoenix 5 pins is a good example)

    As i often say lets start with this…….

  3. Excellent article Matt!   Multi-Body is another reason I chose to leave Solidworks and move to Solid Edge.

    Solid Edge gives me the capability to design in the program. To be able to start with a basic idea and as it evolves break it up in the individual parts that makes the finished product is exactly how I like to design.

    A product idea always starts as a total concept and then evolves into the individual parts as the design develops.  So Solid Edge is giving  the ability in CAD to do what I used to do  building and working with prototypes.

    Solidworks for me was just putting my mostly finished design in CAD for the most part.

    So thanks Solid Edge for understanding the design flow and developing a tool to work as my design process does.

  4. Matt, the fact that disjoint lumps don’t automatically become different bodies is by design and has been this way in Solid Edge since day 1. Our assumption is that just because you may need to design disconnected stuff, does not make it different parts per se. It may make sense to design say the interfaces with other systems and then connect it together later even though its a single part. What you’ll see is that Solid Edge will automatically join these disjoint lumps into a single body when the connecting structures are designed.

    We could have changed this when we did our ST5 work on Multi-Body, but feel like the existing paradigm is equally (if not more) productive and has long standing precedent with existing users.

    1. Dan,

      The “lumps” vs “bodies” distinction is maybe not obvious, but I get what you’re saying. Maybe you could offer some control to hide or color “lumps”. Why would bodies produced by one method be treated differently from bodies created by another method? I guess I just don’t understand why the concept of “lumps” is needed. You can do the same thing with bodies, can’t you?

  5. Maybe I shouldn’t have introduced the term “lumps” (this is a Parasolid term). Basically, all I was saying is you can have disjoint “stuff” that is part of the same body and Solid Edge has always been this way by design. I guess the easiest explanation is that body creation in Solid Edge is very explicit — In the absence of declaring a new body, the system assumes it is part of the same body, whether disjoint or conjoined. The key thing is that the “Active” body is always trying to get whatever you are creating and glom it onto itself. Maybe an example will help:

    Case 1 — Disjoint Single Body

    1. Protrusion 1 — part of Body 1

    2. Protrusion 2 (disjoint from Protrusion 1)  — still part of Body 1, though physically disconnected

    3. Protrusion 3 (which materially connects Protrusion 1 and Protrusion 2) — What will happen when you place this is that it will AUTOMATICALLY merge all the stuff into one glom of stuff. There are no booleans here. This is because it is all one body in the first place and the system is therefore trying to continually join it all together each time a feature is added.

    Case 2 — Disjoint Multi-body

    1. Protrusion 1 — part of Body 1

    2. “New Body” command – start Body 2

    3. Protrusion 2 — part of Body 2

    4. Protrusion 3 (which materially connects Protrusion 1 and 2) — will become part of Body 2 because it is the active body — Body 1 (protrusion 1) will not be automatically joined, since it is a separate body

    5. Optionally boolean bodies 1 and 2

    So if you are really designing “one thing” where at times it may have several different disjoint pieces, you don’t really need multi-body for that, as the system will continually be trying to join it all up. But if you are designing things where its important for them to be distinct  for a large portion of the process (like a tool body and a mold plate), then multi-body is the way to go.

    It sounds a bit complex when you write it down, but I think it will make sense if you try it.

    1. Dan, I understand how it works, just not sure how much of an advantage it is in light of what you give up. I like the Design/Construction body distinction, but can’t see how the lump/body distinction is a benefit. You’ve basically got to plan it out beforehand if you want to use a body as a lump rather than as just another body.

      Since I’ve got you here for the moment, I see you can mirror bodies, but it doesn’t look like you can copy them, move them or pattern them. Am I missing something?

      1. Matt now that ST5 is out

        Here a screenshot  of a small project i try.

        I was able to pattern a body along a curve inside the Synch.environment


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