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multibody model: use ref. planes or body surfaces to drive key features?

Question asked by Travis Colley on Jan 7, 2011
Latest reply on Mar 3, 2011 by Jerry Steiger

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Hi there,

I'm building a multibody part with 3 parts:

PCB solid body

Top Enclosure solid body

Bottom Enclosure solid body

The PCB has components that drive enclosure ribs / holes etc.

To build a well-made model parametrically, can I simply use the surfaces on the PCB solid to drive the dimensions on the enclosure, or should I use those surfaces to create reference geometry such as a plane, and build my enclosure features using the reference geometry?

I see that if the specified part were to change, I'd have to change the component, which would introduce a new face, which would break those links.

Any other issues to consider when approaching these types of references?

Thanks

Travis

Jerry Steiger Jan 7, 2011 7:19 PM

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Travis,

You'll probably get a number of conflicting replies here. Personally, I try to limit my use of features in bodies being driven by features in other bodies or parts, for the reason you noted, that features may break. Another reason to limit the parent/child relationships is that many people like to break the links between parts when the design moves into production, so that someone unfamilar with the design can't inadvertently change a part model by changing another part. The less such features you have, the less to deal with and the lower the likelihood of problems. I like to use planes and sketches as masters to drive all of the features where I can. If you are designing the PCB from scratch, then I would have a master sketch with the outline, mounting holes, connector locations and other details that interface with the other parts. You can make that sketch a part and insert it into the PCB and each of the other parts.

Jerry Steiger

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Jerry Steiger Jan 7, 2011 7:19 PM
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Travis,

You'll probably get a number of conflicting replies here. Personally, I try to limit my use of features in bodies being driven by features in other bodies or parts, for the reason you noted, that features may break. Another reason to limit the parent/child relationships is that many people like to break the links between parts when the design moves into production, so that someone unfamilar with the design can't inadvertently change a part model by changing another part. The less such features you have, the less to deal with and the lower the likelihood of problems. I like to use planes and sketches as masters to drive all of the features where I can. If you are designing the PCB from scratch, then I would have a master sketch with the outline, mounting holes, connector locations and other details that interface with the other parts. You can make that sketch a part and insert it into the PCB and each of the other parts.

Jerry Steiger
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- Travis Colley @ Jerry Steiger on Jan 7, 2011 8:42 PM
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  Hi Jerry,
  
  Thanks for the reply.
  
  Here's more specifics on my process and "goals," I realize that different jobs dictate different approaches. For this case, I'm:
  
  Working as industrial designer (form, shape, user interfaces and usability) and CAD model / technical drawings for manufacture.
  
  I need to work with another group doing the PCB, and we specify the location of certain components, since lots of the PCB components are accessible to the user and subject to design modification in their position as well as size constraints, require iterative modelling / testing.
  
  I'm approaching using the solidbody mastermodel techniques.
  
  I want to have a fairly undefined but parametric approach for a master model, where I can manipulate a lot of top level sketch dimensions and propagate the changes to the solidbodies and then part files. I want to further carve and shape the outerform but also need to make adjustments for PCB components that change that affect user interfaces / plugs and ports, which has tighter tolerance and fit requirements. Some rib structures/ bosses / would also be affected.
  
  *** Jerry, when you note that you personally limit the amount of features driving other features, is this because you are you not worried as much about being able to have a lot of freedom to make propagated changes in your parts, or are you still able to achieve a model that you can easily change and propagate changes downstream because of your methods, and having everything is on one top level sketch? To clarify, you're not using the "save solidbodies approach"; you make a single sketch that outlines PCB components, mounting bosses as well as enclosure dimensions, ribs, outer shape and form references? Then you insert that sketch "part" into all the other component part files as the first part? Thanks for confirm or clarification on my description. ***
  
  I'm handling the encosure files myself, and not worried about shared or network scenarios.
  
  I'm linking various body features and sketch planes based on other logical bodies / faces / edges and planes. I have set up my file with a key origin and three base planes are established and referenced. My top level sketch is undefined but has key relationships, but I can freely move and drag various items and these are propagating well into the rest of the tree. I do get some broken references but so far they've been easy to fix or resolve.
  
  I also want a CAD model to pass to plastics contractor to generate molds / parts. I assume these will be the derived part files I'll save out from the solid bodies. My split line is simply straight along a sketch plane, so I made my two bodies using two separate features: extrude (up) for the top enclosure. extrude (down) with unchecked merge result for the bottom enclosure. The same sketch is shared by both of these.
  
  Cheers for your help, I've seen many of your valuable comments and responses,
  
  Travis
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  - Jerry Steiger @ Travis Colley on Jan 8, 2011 2:11 PM
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    Travis,
    
    Actually, I do normally save parts from my multi-body master to generate the final parts; I just didn't want you to think that it is necessarily the right way to go. I've tried a number of methods and am still trying to work out the best one for our type of work. I don't typically use the inserted part, but other people have had a lot of success with it. One reason I haven't done much with the inserted part is that one of my colleagues seemed to have problems when he tried it.
    
    I try to base shared features on a shared sketch because that reduces the number of features that break later when I go back and change something in one of the features. As an example, if I make a boss on one body and then use converted edges off that boss to make a boss on the mating body, my second boss can have problems if I insert a change between the two features that changes the edges on the first boss, say putting a fillet in. Sometimes I will use a master sketch with only the geometry that is needed for the various top level interactions and then use other sketches based on the master that add detail for various features, just to keep the top level sketch manageably simple. Keeping it all in one sketch is better.
    
    Early in the design cycle it is pretty easy to make changes without breaking much. The models get much more fragile as you get more and more detail added in. (Fillets are a particular source of problems.)
    
    It sounds like you are pretty much in control of your parts, except the PCB. That makes it easy to build as much detail as you like in your master model, simplifying the task of keeping the pieces in sync. Do you have a good method for keeping in sync with your PCB designer? This is probably going to be a critical element. We use Altium for PCB design and Desktop EDA as the link. We can pass the PCB outline, height restrictions and critical component placements to the PCB designers and they can send us back solid models of the completed PCA. Our EEs often build the SW models for electrical components themselves, since they know best how they want the part oriented and where the origin should be. If it's a tricky part, they may come to the MEs with their requirements.
    
    One other point that is sometimes a little tricky is where to set the origin and how to measure your parts. We often end up putting in some details just to make the tolerance analysis and measurement easier.
    
    It looks like you have a good handle on what you need to do and are setting yourself up for success.
    
    Jerry Steiger
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Craig Pretty Jan 18, 2011 6:38 PM
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After designing a number of plastic cases for PCA's (Assembled PCB - our companies terminology which seems prevalent amongst the electrical guys), I have tried a number of different variants.

I have tried the fully in context assembly built with the PCA inserted as a part. I did not dimension anything off the PCA as it was constantly being revised. The top and bottom case were separate parts. I created controlling sketches in the assembly that controlled the parts (outline, profile, boss location etc). By using sketches in the assembly, you can do clearances and locations by hiding the cases. This works OK, but quickly gets complicated with many links between parts, or controlling sketches that suggest you could have just designed in 2D. The end result though was a robust model that as parametric, and changed with minimal cleanup to fix problems. The test of this was that another team created a large version of the design with no real problems.

I have done the insert part method. I do a lot of this for injection mould tooling and post machining of moulded parts. It is a reasonable way to do things, but the insert part and associated updating is quite horrible. Not particularly easy if you have lots of revisions of PCA. As you tend to immediately use your sketches for creating features they get absorbed and hidden deep in the design.

I have tried a few hyrbid methods between the two above scenerios and now prefer to work the following way;

Create an assembly with the PCA. Create controlling sketches in the assembly to determine where screw bosses, holes, PCA mounts, clearance levels, wiring etc are located. These sketches are not meant to define the entire feature eg, screw boss locations are a simple sketch to show positions, and not the entire profile of the screw boss. The sketches would not reference the PCA, as then you can quickly change revisions and then simply edit the controlling sketches.

I use a multibody part for the case (this allows the entire form to be created, then the case split to create the two halves). Use the controlling sketches to drive the critical parts of the case design. I wouldn't reference anything off the PCA.

This gives some advantages in that you can easily drop a new PCA into the assembly. You can even have both revisions of PCA in together to compare and contrast. You then edit the controlling sketches . You can use mates to move the case relative to the PCA which is heaps easier than move body.

When sending out I would do a save body and then further save these as Parasolids or STEP files so that they are dumb solids with no ability to change the design.

I guess all the decisions on which way to go come down to experience, and the likelihood of having to revise the PCA or for someone else to edit the model. Don't be afraid to change plans part way through, as from experience hammering away at an unstable model can chew through more hours than a rethink and remodel.
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- Matthew Perez @ Craig Pretty on Jan 19, 2011 9:18 AM
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  Craig, I have another possible version for you. At least how I do this sometimes. I will define a bolt pattern for a pcb(which doesnt change between our revisions of components) and insert that as a sketch block into a multi-body part. This allows me to insert Part and reverence the sketch block to locate the pcb in the part. You can have a specific PCA file where you dump the latest revisions or break link when inserting the part. The sketch block should have enough info to locate your part.
  
  I dont typically dimension to the pcb but use it as a visual reference in most cases. Like you, ours changes more times than i care to count and im currently working with an old revision trying to modify a new housing to work. I found the sketch block setup works alright for me because our circuit guys dont always play nice with the hole patterns. It allows me to edit the sketch block for any bolt hole changes to the card easily.
  
  Travis, as jerry and craig mentioned there are many ways to do this. In my situation I usually dont get a full PCB or PCA model which makes things a bit more difficult. For references I will usually start my models so that the PCB(or one of them) is on a plane. Some of my housings have the PCBs screwed into them so there are no reference issues. Others have the pcb sandwiched between parts. In those cases I will use the Offset from plane end condition in my feature. Before you get started you can create an Equation that is simply "PCB_Thickness = .07" or something like that. Any references in the model such as the offset from plane end condition can be linked to this. This allows you to easily change it without finding the features in one go. When possible I use the Equations dialog before a model to define things like Wall thickness, 60 or 75% wall thickness(for plastic ribs and things) and so on. These get references in sketches by linking dimensions(they are on the drop down) or editing feature dimensions. My reasoning for this is that I have been handed models with hundreds of features before, if the plastics house says you need to change this rib thickness or something along those lines, one edit and an update takes care of the whole model.
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  - Travis Colley @ Matthew Perez on Jan 30, 2011 12:24 PM
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    Thanks for sharing your process too, Matthew.
    
    I've ended up with a multibody part for the enclosure top and bottom. As suggested, I called this file MasterModel. I shelled, bossed, shaped, and worked the parts all within the master model file. I also built a blocky PCA in the multibody part which I used for references in some cases. (This product has a number of larger PCA components with interfaces to the outside user, in different areas of the product, so lots of positioning and fit issues between PCA and enclosure design. Sometimes PCA changes were not a problem, but some did cause broken references. I learned which kinds of ref's are better than others. I also learned how good it is to make sure the main origin and reference planes match up in all your part files, for ease of mating.
    
    I saved the bodies, and have the saved parts reassembled in an assembly file. So now I have an assembly file, a multibody part file, and the saved bodies part files. I'm not sure yet what's the best or most efficient. I also have a "good" PCA assembly file with real component parts modelled on the board, which is used in the assembly.
    
    One problem, as noted by Gerald Lacy, is the way solidworks renames multibody parts. I found myself renaming the parts quite frequently in the mastermodel file (the multibody part file) because SW would change the names and the order of them in the feature tree all the time. And, I haven't totally figured out how SW names the part files created using save bodies, and manging those links, but that should come along as I work more with this method. (Thanks to everyone for their help and suggestions with this process! )
    
    Initially, the multibody top and bottom parts were first created in the feature tree by 2 extrusions:one upwards and one downwards, with merge unchecked. The parting line was the sketch plane, the initial design involved a straight parting line. Later, I had to move to a varied curved parting line, so my two initial parts had to be built differently. I was worried this would wreak havoc on the feature tree as I had to delete those inital two bodies, with a lot of features and designs applied to them. However, I was very happy that I was able to re-derive the top and bottom bodies without too many problems. The new halves were created by extruding one body and then splitting the overall form using a curved surface (I drew the parting line profile, the made this into an extruded surface, then used the extruded surface to split the part.)
    
    I found that when I needed to make a somewhat "major" change in a feature higher in the feature tree, I had more sucess if I rolled back to the point where I was making the changes, then rolled forward small steps at a time, it seemed to reduce chance of feature "christmas tree" (errors and warnings).
    
    Also, it seemed frequent that a feature error simply could not be fixed by editing the feature, but by simply deleting and reapplying/ redoing / recreating the feature on the same sketch would sort out the problem for SW. (Other problems were sometimes fixed simply by saving, closing, and reopening SW. I'm sure everyone has learned a sequence of fixes that includes this method. Maybe SW should create a new feature: a big red "shutdown and restart" button to make this frequently used solution easier. . . . (just kidding).
    
    Travis
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    - Jerry Steiger @ Travis Colley on Feb 2, 2011 12:17 PM
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      Travis,
      
      Looks like you've learned a lot about how to use multibody parts. I've found that it is best to name or rename my part bodies as early as possible in the feature tree. If you name them immediately, the name tends to stick. If you forget and SW goes through its normal process of changing the name with each added feature, then a name added later doesn't seem to stick. That's a real pain, as you have discovered. I have no idea why SW behaves this way.
      
      Jerry Steiger
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      - Travis Colley @ Jerry Steiger on Mar 3, 2011 3:18 AM
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        Hi Jerry, thanks again.
        
        Yes, I like naming things right away too. I used to be lazy about this, but I've learned in other applications, like illustrator: naming layers and entities is essential to keeping organized and working fast. Nonetheless, Solidworks does like to sneak up on you doesn't it? It's like it's using the "witness protection program approach" to renaming one of your solidbodies every once in a while. And of course, if you have about 6 or 7 solidbodies created, you'll see them all listed in the tree, but wait, now, one of them's missing . . . .there's some new solidbody, where'd that that guy come from? (renamed after some new feature you created somewhere along the way). So you gotta rename him back to his old name, but hmmm, which one was it now, gotta deduce from all the other ones. . .who's missing? What's the name again? It's like a little memory game for stress relief, I guess.
        
        I find the folders are good for organizing each solidbody into. (but there are some places in the tree it seems I don't have the option to set up a folder where I would really like it.)
        
        It gets complex as you save bodies, those popup windows with check boxes sure look funny, I can't really tell what's happening as files are saved and if I should be naming them or autoassigning, etc, but I think I have the hang of how Solidworks links a saved solidbody to a part file, and then how the part files can be put into an assembly, where it's easier to move things around. The SplitPart feature gets involved too there and not sure what's the best, but, it'll come.
        
        Is it normal to have six or seven SaveBodies features in the tree, or is it more typical to just have one solidbody?
        
        Anyways, cheers! Solidworks just crashed on me so gotta go and see if I lost anything.
        Travis
        
        ***ps: solidbodies are also renamed if you roll the tree back and forth
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        Jerry Steiger @ Travis Colley on Mar 3, 2011 8:36 PM
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        Travis,
        
        As I said, SW seems to want to rename bodies unless you change its name immediately after or as you make the first feature. The other thing that really gives me trouble is that SW keeps a list of all of the names I have given bodies and won't let me reuse a name. If I name a body Battery Door and then SW decides to rename it, I can't change the name back to Battery Door, I have to call it Battery Door 2 or some other name. Very frustrating!
        
        I really don't know whether multiple SaveBodies features or a single SaveBody feature is more common. I tend to work on all of the bodies and then save them all at once, but I don't have any particularly good reason for doing it that way. I agree that the user interface seems needlessly confusing.
        
        Jerry Steiger
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multibody model: use ref. planes or body surfaces to drive key features?

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