When you build a product in Solidworks do you start with all of the parts in one part file (if so how do you convert to assembly later?)
Or do you build each part in its own part file right from the start, then afterwards put together into assembly?
Unsure when it is better to use either method, or what the pros vs cons are.
Any tutorial links would also be helpful!
So what you are referring to is called parent modeling… (some engineers despise this it basically mean you create all the parts in one file and each part is made as a individually body within that file (i.e do not merge solids) you can then save out the individual solid bodies to their own part files, which then can be brought into a assembly. Thus if you make changes to the file that has all the solid bodies (the parent model) it will update all parts that are connected to those solid bodies.
This can be great when you have a complex surface that spans across multiple part and you want to ensure they all update in as few mods as possible. but the main model can become large, overly complex and very unstable… not something you want to be working with down stream while getting ready for manufacturing files.
One method I’ve heard of but haven’t tried myself, is start with an empty assembly file and start adding “virtual components”. Later when the design is finalized you can convert the virtual components into actual files. This will save you from having a bunch of junk files scattered in the folder/vault.
the truth in my mind is that it all depends on who you are handing it off to and how well they can work with the models. I have had manufacturing engineers and design engineers LOVE the parent model when i showed them - i had others who threw hissy fits.
down stream cad modeling is more about making sure the model is editable and doesnt blow up. Not too long ago there was a outside eng. resource you against instructions (to save time) simply used the scale feature when they needed to make a change to the models - it then got to a point where they said they could no longer make changes to the model and would need 3 weeks to rebuild it from scratch at a cost of X to me.
I used to do a lot of part modelling and making assemblies from it but it is slow and a lot of work to maintain relations that way. Making sketch or feature relations in an assembly as a part is a bad idea if you ever use that part in another assembly. Making parts internally to an assembly means they can only ever really be used for that (or has high potential to go crazy with missing references at a future date). I have mostly used multi-body part modelling for a while because as long as you really understand the history tree and parametric features and relationships a well-designed model shouldn’t break features if you change one at a later date. I think the ideal solution is using multi-body parts as a master model for overall forms broken down into multiple parts for manufacture and then using assembly to bring in all other fixtures and standard components.
A former colleague of mine used a master sketch (drawn in a part file) to create outlines for multi-body parts, dimension all the vitals etc, but not actually create any bodies (or surfaces). He would then insert the master sketch part file into a new part file at the top of the tree, converted whatever lines he needed, then created the part. Then in this latest part file he could add any extra features that didn’t have any thing referencing them, e.g. an extrude cut here or there, fillets, chamfers etc. Once all bodies were created, he’d insert the master sketch part file into an assembly and mate all the subsequently created parts off that (which saved on loading time since it is lots of smaller parts rather than one large one). Any dimensional changes, additional parts needed etc could be easily updated or added to the master sketch and would update across all parts.
This method is a bit of a cross between multi-body part modeling and modeling within an assembly.
And is of course much easier when using basic geometries - we all know converted splines likes to make life difficult.
I generally try to keep parts independent as much as possible, since as others have stated assembly relations have a habit of getting mixed up and not translating when you try to use things in new assemblies, and a parent model can get bloated at times. However, if I’m making any sort of (even mildly) fancy surface that straddles two or more parts or if two parts have complicated mating surfaces I will use a parent model. Despite it’s downsides it’s the only real way I know to make complex surfaces match and does a good job making sure that if you make a change to one part you will also make a change to the mating part (moving holes, etc.). If the model starts to get big, or if there are a lot of features on individual parts that don’t relate in any complex way to other parts I will often make a base parent part with the common geometry then use that as a base for other parts. I’ve found that Insert>Part works best for me for this purpose. If there are extra bodies that a particular part doesn’t need I can just delete them as the second feature. It seems to be a lot more stable than Save Bodies and is good at updating references if you change the name of the base part (just make sure everything is open when you’re doing a Save As).
There are quite a few presentation that you can pull down on these, among others, to choose from “Solidworks world presentations”.
That said good file management is paramount is going to key no matter which method is chosen. Top Down, Bottom Up, or Master Model. Some tips to keep in the back of your head…
Always overbuild and trim back to what you need.
Better to build a whole surface then break it up rather than build pieces to create the whole.
Don’t mirror if you can build the whole shape.
Keep an eye on the “Performance Evaluation” to see what features are taking “a long time” to rebuild.
“Enable the Freeze bar” (Systems Options---->General) but don’t just use this as a crutch for bad modeling techniques. Just because you can doesn’t mean you should.
If you “have” to have a pattern of 1000 holes create it but make a configuration with it suppressed and an alternate version with a possible graphics texture version of it.
Generally save fillets towards the end of the modeling.
Use features and not sketch fillets if possible. A lot more levels of functionality and can always suppress/unsuppress features.
Generally larger fillets first then smaller ones.
File “Pack and Go”…this gathers up all files associated with the model, drawings, renderings…etc.
Give names to features that are important. (we’ve all had extrude 15 at least 100 times and no one knows what that is)
Short and Sweet Snap shot…keep in mind you’re never limited to just one method. Any or all of these can be used in combination but generally not recommend if sharing with others or even for the sake of your own sanity and not creating circular references.
Master Model - one thing to consider is that you don’t have to just take the multi body model right into an assembly. You can also leave out certain details in that first master part file and insert the bodies into a second tier of part files and add the additional details there and then throw these into the assembly. Keep in mind that all dimensions with this method are contained in the master part file and not in the 2nd tier or assembly so if that’s needed for down stream then you’ll have to add in the drawing…possibly use some MDB if applicable. SW HQ would benefit greatly if they’d added this kind of functionality where dimensions can be added to the 3D model to drive it. There’s also no way to make a body within a part file “light weight” or “SpeedPak” which is huge in terms of making larger files easier to work with.
Top Down - Virtual Parts are “great” but confusing if you’re really not paying attention to if a file is or not. Upside is that one part files can drive one, ten, all or on an as needed basis. Generally not a good idea to reuse models made in this way unless it’s saved out as a different file name and all external references are broken. (once broken this can’t be undone). Because the other files can be loaded as light weight or even SpeedPak this “can” ease up on the strain on your CPU. But again KNOW what’s weighing down your computer through the performance evaluation, what you think it is and what it could be can sometimes be different. For ever external reference made just know that it adds to overall rebuild time.
Bottom Up- The most straight forward method. A lot of this is really product, company, and workflow dependent. Also downstream vendors consideration is always nice. Most “flexible” in terms of possible reuse of models in other projects and also for the creation of drawings if needed. Though the other models can’t be seen, once inserted into an assembly the ability to edit there is totally possible. (POKE POKE…hey SW HQ if you’re reading this, allow for more than one part file to be edited at once).
This really is only scratching the top of the modeling method ice berg but hopefully it’s a start…
As others have said, there are pros and cons to both Top Down and Bottom up modeling approaches. Professionally, I always just ask the customer at the beginning of a project if they have a preference for how they’d like the models constructed, or if they have any special protocols or design guidelines. It’s an easy question, and quickly clears up any ambiguity!
Depending on the complexity of the model, there are a few different ways I normally go:
Simple parts or parts that will be re-used multiple times in a model: - Model these parts in a blank part file from the origin and then use mates to constrain them in an assembly file.
Complex parts with multiple interfaces to other parts: - Insert a blank part into an assembly and then copy the mating features surfaces into the part by doing an Offset Surface (offset = 0). Depending on the maturity of the model, I’ll determine whether to allow these surfaces to remain linked through the assembly by toggling “No External References”. If the mating surfaces are liable to change, it is usually safer turn on “No External References” so that the links are broken. Use these surfaces to build features from. But realize that if the parent geometry changes, you’ll probably have to do a full rebuild of the model.
Complex parts with surfaces that continue from one part to another (i.e. housings):
_- For this, you need to create a master model. Depending on the expected level of complexity you’ll want to either:
Just make the outer surface and cutline sketches/surfaces (very complex, high feature count), break out the surfaces into individual part files and then build features from these surfaces/sketchs
Fully build all the parts in a single model and then break out into individual part files_
As to the OPs question of “how do you convert to assembly later?”, I use “Insert Part” and “Delete/Keep Body” to break out a single part file into individual part files. To do this, you open up a blank part file and select Insert > Insert Part from the top menu bar, and then select your master file. From there, you’ll be able to select what information you want to carry over into the new model (i.e. bodies, surfaces, sketches, etc). Once the geometry is copied in, then select the “Delete/Keep Body” feature in the Direct Editing toolbar. Then select the body or surfaces you’d like to keep and then press ok. This way, the parts are linked and will update as the master model is updated, but you can build new features onto it with a simplified model tree.
I only build multiple parts in a part file when the sketches and surfaces are interrelated.
Whenever a part is either independent of the others, a moving part or better defined with matings, it will be added in an assembly.
The same goes for pieces of an assembly that are only mated with a few relationships, then they will become subassemblies.
Starting from a master model containing all the base surfaces is a great approach.