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Should I model this as a single part or assembly?

Question asked by Rick Girt on Feb 16, 2010
Latest reply on Feb 16, 2010 by John Burrill

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Hey all...

As a new Solidworks user, I'm trying to wrap my brain around how to divide up assemblies into sub assemblies, and into parts. Some of the drawings we made before SolidWorks, a combination of machined parts and purchased items fixed together would still be considered a single part. I'm not sure if thats the best way to categorize things now...

Take the model attached for instance.

In my previous drawing the whole thing was considered one part. It's made up of several locking collars and some welded together round stock. Its obvious now that the collars and round stock can be separated as parts then insterted into an assembly.

But the items in red are all welded together.

How would you divide this up into components?

John Jablonski Feb 16, 2010 3:47 PM

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However, now after seeing it (using quick view....didn't know about that), I'd add this.....is this something you sell, or something you build a couple of in the tool room for in-house use? If the latter, you may be better off just making a part, and then giving the drawing to the guys in the tool room, who will make the assembly how they know best, since they'd probably just ignore any details around the weld areas that you give them anyway.

-john

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Glenn Schroeder Feb 16, 2010 3:19 PM
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I can't open your attachment without the part files.
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Mark Kaiser Feb 16, 2010 3:25 PM
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Any purchase off the shelf parts for us are a single part. The rest is usually how it fits your business/SW practices best.

For me, all the rods would be seperate configurations in one part file, and the collars would be a part file. For assembly, whatever you consider an assembly on the shop floor is an assembly in SW, usually...

*If you open the assembly file with 'quick view', you can see his assembly.
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- Glenn Schroeder @ Mark Kaiser on Feb 16, 2010 3:35 PM
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  I have to admit that I don't know what 'quick view' is or how to use it.
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John Jablonski Feb 16, 2010 3:38 PM
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Without seeing your assembly....each component of the weldment needs to be machined at some point, correct? Then each should really have it's own drawing, which would mean each should really be a separate part. then put them all into an assembly.
Then assemble your collars, etc to that assembly.

That's what I'd do anyways.

-john
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John Jablonski Feb 16, 2010 3:47 PM
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However, now after seeing it (using quick view....didn't know about that), I'd add this.....is this something you sell, or something you build a couple of in the tool room for in-house use? If the latter, you may be better off just making a part, and then giving the drawing to the guys in the tool room, who will make the assembly how they know best, since they'd probably just ignore any details around the weld areas that you give them anyway.

-john
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- Rick Girt @ John Jablonski on Feb 16, 2010 4:36 PM
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  Hey John...
  
  It's something that we make and use internally, part of a much bigger assembly. Chances are I could detail it how I think it should be made, and depending on who actually puts it together, it could be assebled any which way but...
  
  For the sake of keeping the drawing simple, I'm thinking it would be best to make the parts in red all one part file. After all, one wouldn't divide up the locking collars into their individual components for the assembly (screws and collar halves) right?
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  - John Jablonski @ Rick Girt on Feb 16, 2010 5:40 PM
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    After all, one wouldn't divide up the locking collars into their individual components for the assembly (screws and collar halves) right?
    
    I would not, no. However.....Ruland (for example) certainly would have separate parts for each individual component. In this case, three separate parts and drawings.
    
    As far as I am generally concerned, the lock collars are one part, since they are typically one thing that you pull off the shelf and throw onto an assembly. However (there's that damn 'however' again).....if you were to modify the collar halves in some way, then you -may- have to create separate collar half parts and drawings. At least for the one half, then create a new assembly, but again, since it's in-house, you don't really care too much about tracking each individual component. If it were sellable, it can go either way and depends greatly on how your MRP/etc system is setup. I can't tell from your assembly if the collars are modified or not. Is there a reason you don't use a 1-piece?
    
    From the looks of it, to be competely correct, speaking in terms of MRP/inventory tracking, I think you would need to purchase the collars, separate them out physically in stock, with one part number for one half, and a second for the other half, and a third for the screws. Then create an assembly of the round bars with the one half, then insert -that- into an assembly with the other half + screws......All of which you don't really need to do with something fabricated & used completely in-house.
    
    -john
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Daen Hendrickson Feb 16, 2010 4:49 PM
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Always many ways to skin a cat...

Since you say the tubes are welded, I would create a weldment part for the red tubes, a weldment part for the gray tubes, a notional library part representing the purchased collars (that is if the manufacturer does not have a ready made CAD model available), and then bring it all together in an assembly.

The weldment part drawings contain the cut list of the individual pieces. The assembly drawing shows how it all goes together.

Daen
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Brian Rasco Feb 16, 2010 4:52 PM
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I second what John said, it depends on what you're using it for and how closely you need to keep track of the individual parts. For in-house use, you can give the basic drawing to the shop and get it made.
But if you're going to need to keep track of each part, for maintaining an inventory of all the pieces, you need a seperate drawing or at least a seperate ID# for each piece on a "cut list" . That way you can make a BOM for the assy . and each component will have a line item entry.

What I try to practice on drawing methodology is to make my documentation such that I can either send the prints out to our own shop or some other shop across the country. You may start out making one or two of something, and then all of a sudden need a hundred of them and purchasing needs to get all the pieces quoted outside.

Lastly, having a part file for each basic component allows you to assign a material to that part, so that you can get the assembly mass/c.g. later.

part files incl. configs -> welded sub-assy file
sub-assy files + machined assy. features -> machined sub-assy file
machined sub-assy file + indiv. parts + purchased components -> main assy. file

Please keep in mind I can't open your file, this is just for general reference.
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Kenneth Barrentine Feb 16, 2010 4:55 PM
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3 red tubes = 1 part (weldment)
2 gray tubes = 1 part (weldment)
(2x) 1 collar = 1 part
add them all to = 1 assembly

option, if the collar is welded to red tubes then;
3 red tubes + (2x) collars = 1 part (weldment)
tip: insert the collars into the weldment and mate (yes, mate inside the part)
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Jeremiah Feist Feb 16, 2010 6:42 PM
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Our rull of thumb is if it has a separate part number, it has a separate file (either an assembly or a part). And no other files exist. so if that do-dad has its own part number, it would get a file, if that part number has a BOM, then it is an assembly of teh appropriate parts.

Jeremy
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Derek Bishop Feb 16, 2010 7:05 PM
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If you use multibody weldment parts remember that you can use relative views to detail up the individual bodies.
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John Burrill Feb 16, 2010 8:40 PM
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It did matter at one point. But since Solidworks 2003, it's mattered less and less with each release.
Take a look at Solidworks 2001-the last release to be a pure germ distinguishing parts and assemblies.
In that release, a part file contained a single solid body and you took a part and inserted it into an assembly to mate it with other parts.
Solidworks 2001plush came along (there was no Solidworks 2002) and you could turn a single part into an assembly with the new split feature, whereby you create a sketch that determines where a body could be paired out into multiple components. This was usefull for creating furniture like tables and cabinets.
Solidworks 2003 introduced multi-body parts but it was implemented more to open the workflow of defining parts instead. Bodies coudn't be repositioned, hidden or have their appearances modified.
With the weldment functionality introduced in 2004 came the first behavior of a part file as an assembly. You could create a cut-list of structural members and detail them individually
In 2005 you could reposition and pattern a solid body within a part, making it easier to simulate switches
In 2007 you could add mates between bodies to position them (though not all assembly mate types were supported)
In 2008 you could store new part definitinos within the assembly file as virtual components, so you could model something like a hinge as an assembly and only have one file to deal with. God help you if you checked this file into the vault.
In 2009 they added the ability to apply materials, appearances and display states to bodies within a part as though they were components of an assembly, so now you can model an inseperable assembly like a leadframe as a single part and get correct mass properties and simulation results from it. You could also propogate assembly cuts to the part level at your discretion.
In 2010 assemlies, you can take an external component of an assembly and make it virtual (very useful for o-rings and stuff that has to be modified to fit one particular assembly), detail a specific body within a part without having to configure it.
And in 2011, according to the Solidworks World presentation, you'll be able to create an exploded view of a weldment right in the part and you'll be able to create cut sweeps, chamfers and fillets in the assembly.
So if you watch the trend, the distinction between file types is barely discernable. I'll throw out a prediction that after a couple of releases, there won't be sldprt and sldasm files. There will only be a model file. What becomes more relevant is how the component is managed in your ERP system and re-used by other CADDER's.
For the present, there are a few criteria that have helped me in determining if I should model a component as a part or assembly.
1) if it's an off-the-shelf part like a hinge, it's going to be inventoried as a single item both in stock and in the assemblies where it's used. I will never have to account for half of a hinge that we buy from McMaster Carr. Today, I would model this as an assembly with virtual parts so that I can get the dynamic motion (flexible assembly). I also take this approach for things I have to take apart in exploded views, like a lamp with a screw on mounting bezel. For an bananna plug, I'll model it as a single part and then have configurations to hide and show the insulator. The point is, that if I don't have a hinge-pin part number in my ERP?MRP system, I'm going to try to avoid having a seperate file for one.
2)If I have to create a dissasembly of a COT's item I'll model it as a fully realized assembly with external components. At one of my jobs we bought a AK-47's whole, entered into stock under one number and then had to create a drawing where we took it apart and entered each component that we kept into inventory as a new number. We numbered the individual components as dash-numbers and used derived parts to create machining details with our modifications.
3) if a part has a drawing that requires an ECO to change, I will model that part as a seperate file. I learned this lesson the hard way. When I was starting out at one company, I was crazy in love with configurations and modelled five top-level assemblies in one file. I even used configurations to track revisions. One assembly feature later, I realized I made a mistake. No, I only want to affect part numbers that I have permission to change-or at least know I'm changing. Virtual components and part bodies are invisible to most PDM systems.
4) if a part is counted individually in a BOM, I will model it as an individual component and instance it in the assembly. We had this guy where I work now who spec'd eight dowell pins for a base-plate bom and then proceeded to model them as pairs so that he wouldn't have to apply as many mates. Not only did this make the BOM quantities and every type of query mechanism report the wrong number of pins in the assembly, The dowell pin model couldn't be used for anything else. This happens a lot with harnesses. CADDER's will model a backshell joined to a connector, despite the fact that they're two distinct items in the BOM
5)Conversely, for stuff like Solder, process parts (bent terminal ends, rolled eyelets, swaged rivets) and epoxy, I consolidate. I insert a new part and model everything applicable for one part number to one assembly step. If my drawing instructions go 'stake the transmitter with 2216 epoxy, put on the cover and then stake the cover in place, I'll model two epoxy parts with the same number. If my drawing says stake in locations shown after assembly, I'll model one part. What I won't do is model a blob of epoxy and try to copy and mate it in 30 different places.
6) Finally, a word about logical assemblies. Solidworks 2010 appears to have the ability to make a subassembly dissolve in a BOM. This could suggest some awesomeness. For example, I'm modeling an enclosure assembly with about 60 parts that are assembled into large groups and then joined at final assembly (think of the way you build a kit model of a car). Potentially, I could join the components forming the lid into a virtual sub-assembly with fewer top-level mates, easy selection and hid-show and my BOM and file server would look like I had only a single level. However, the 'promote' control in configuration manager only works for indented BOM's (whereas the 'show as single component when used as a subassembly' seems to work in all modes). When Solidworks gets this feature documented and functioning correctly, I'll probably make assembly collections for things like fastener stacks and brush-holder assemblies, just to make them easier to manage.
OK, so there's more than you wanted to know. Good luck.
CAD naked
John
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Should I model this as a single part or assembly?

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