assambly or multipart, what is best? What are benefits of one or other?
Let's confuse him even more and throw in Virtual Parts in there.
You need an assembly of individual parts when:
Multibody modeling is necessary when:
Reasons you should avoid multibody modeling:
If you're still lazy but slightly smarter, you'd use virtual parts in an assembly. But you will at some point save them out to individual parts.
Except for some specific situations, generally, we don't recommend multibody modeling in place of an assembly of parts. It depends on what you're doing, but 95% of the time, it's going to be an assembly of parts.
Answer: It depends.
That's asking for a lot. Please refine your question a bit more. What type of industry, products and workflows do you use/require. Then we can narrow down an answer for you.
I use both, often in the same project. As Ryan McVay said, it's difficult to answer a question that's as general as yours, but I'll give it a shot. I mostly use multi-body Parts for steel structures that are welded together, and occasionally for lumber (though I rarely deal with that segment of the industry). I use Assemblies for pretty much everything else.
I know many people will model something as a multi-body Part first, and then break the bodies down into separate Parts before inserting in an Assembly, and I know there are legitimate reasons to do that, but I never do.
Its a good question. I like to use both together.
Multibody is quick and there's no external references to consider.
You have lots of powerful features available at the part level that are trickier to do in an assembly ...but I think detailing is sometimes awkward.
Obviously if you have any moving parts you need an assembly.
I try and break it down logically into multibody parts that make a good drawing by themselves.
BUT I'm a joiner doing woodwork, not proper engineering, and I always struggle to get cutlists to work properly
It all kind of depends. If I have to build it in the shop and need a bunch of part #'s then it is an assembly. If I am sending it out and getting it made by someone else or I am receiving it in as one part # I may go multi body to keep the files from getting goofed up.
When you say multi part, are you talking about parts made in context of the assembly?
In my business approach, what determines this primarily is how we acquire it physically. It's mostly BOM-centric, mostly assemblies, and I could mostly care less if any component is multi-body or not, as long as we're assembling it to other items and not manufacturing each item.
* If we make the item, it's a part, usually multi-body for Cut-List. Example: weldment skid base or supports
* If we buy the item, it's usually a part, and it is irrelevant how many bodies are in it. Example: pumps, valves
* If we buy a very large and complex item as one part, then I make it from MFR approval drawings as an assembly, where I have made the components from scratch (from MFR standard drawings) to assemble this specific instance of the item. I select all subcomponent parts and specify to exclude from BOM. I also use subassemblies within for repeated arrangements, such as overhead roll doors or a wall section with louver vents and trim inserted. Example: fabricated sheet metal building
* Exception cases: When one distinct item available separately but purchased as paired with another object, I create a sub assembly or a derived part. Example: Rosemount Differential Pressure Transmitter paired with 5-valve manifold or a Pressure Indicator paired with a Diaphragm seal (2 separate purchases) where the subassembly is then glycerin-filled by a third party and remains inseparable through our processes.
* Invisibilia: When I model a Canister Filter, I do not bother modeling the filter that goes in it because it is unseen as assembled, but yet it needs specified (series, model, micron size) and purchased anyway. I make a dummy part with no bodies, and fill out its custom properties. Then I mate it in the assembly to be located at the logical origin of the matching canister filter. This way, the BOM balloons for them at least point to the center of the housings to show that the first gets 100 micron, second gets 50 micron, and third gets a 10 micron filter. This additional info is redundant with the P&ID.
When using Routing, that's a whole different beast where BOM logic is overridden by ease of simplicity. I often create a Y-strainer subassembly that contains a smaller sized blowdown port, nipple, and blowdown valve, instead of defining a separate Routing Specification for the smaller size in an isolated and limited scope. I could do the same thing with a Tee, reducer, nipple, valve, and plug in a drain branch, or where swage nipple reducers are needed to adapt a NPT calibration column into an otherwise buttweld system. In each of these cases, all modeled parts need purchased and populated into the BOM, but only the root item is defined with Routing Assembly Connection Points where it attaches with the rest of the same-sized pipe train.
Our models do not require Motion or Simulation. Someone with more experience with those add-ons can advise differently if that is your aim.
In the end, decide what you need out of the software, and tailor each small decision towards your intended results.
Do it better next time, or even right now, if you find you've painted yourself into a corner from earlier decisions that do not align with goals - at least until you've learned broadly what is needed where and how it alters your work flow.
Only one answer will only suit you well if you are only doing one thing. Some people can indeed get away with that.
If your intended results conflict with each other, be prepared to do it multiple ways, or build in the adaptability that you need.
S. Leacox wrote: When you say multi part, are you talking about parts made in context of the assembly?
S. Leacox wrote:
I assumed it was referring to multi-body Parts.
Assy because you can have each component drawing easy (allmost the time)
But multipart sometimes if need to make or a die to trim
Or structural member
You must to be a clear strategy according to your projet, it defines your succes and a fast drafts to exchange to your team or it will be your nightmare. If you think about it for 5 minutes before will gives you a correct plan to start it.
Hi Glenn, is correct, I referering to multi-body parts.
Depends on the application. Assembly for when I need a BOM and multi-bodied part when I need to represent an assembly say a purchased part, but want the physical attributes of a part.
assembly or part?
with being able to select bodies drawings come just as easy with an assembly.
with no need for part #'s I did this as a part, and detailed out each component on a drawing. waiting on a few friends in the wood working business to get me a quote on it.
On Wood I will make it as part multi-bodied of course indeed! On dies maybe my best choice will make it an assembly. Do you have automatic max dimensions to each component and a custom material on multi-bodied to make a BOM?
I think you have to consider what you do to answer your question. The guy I learned the SSP method from, John Stoltzfus, I believe doesn't use multibody parts in his workflow. He's a very advanced user and assemblies work great for him. And he's developed and refined an excellent workflow for what he does. However, I do completely different work and I use a mixed assembly/multibody part workflow (I am no where near the expert he is).
If we had a little bit more info on exactly what you model it may help people give you more targeted advice.
This is website of company: http://www.cdiexhibiciones.com.co/productos
Actualy, the most models are multi-body parts, in some cases multi-body parts in assamblies, the products that manufacture are forniture, combine diferents materials how: Wood, shett metal, metal pipes, glass, steel shaft...
This are some the models:
Hi Matt, it´s true, i add some pictures for represent better the question,
In my opinion is a good model, but keep recording (cut list, BOM) is most dificult, what is your opinion?
From the models you posted I would follow in the footsteps of John Stoltzfus. - Fine Handcrafted Furniture | Keystone Collections
If you search SSP you will find many posts on his technique.
I have had some resistance to adopting his methods because most of my work is 'one off' in nature and I believe it's more work up front. However after continuing frustration we are looking to move in that direction where we can.
I was about to post exactly the same sentiment as Rob Edwards. You are doing very similar work as John Stoltzfus. I have a simple walk-thru in my pdf at Skeleton Sketch Part Method for Large Assemblies that shows some of the methods John taught me. It is definitely hard to get used to and you have to be disciplined in how you create parts and assemblies. But, the pay off is there. If you've finished an assembly and the boss comes by and says "What would that look like if it were 3foot tall instead of 4foot?", all you have to do is go into the top level SSP, and make the change...BAM! Everything updates and nothing is broken.
yep that is the way to move. not sure if I used SSP or not but I had created a file that we were able to do a pack and go of the template and then change a few top level dimensions and all the parts and drawings updated. A little cleaning on the drawings moving the views around of fixing up a few places for the details, and move a few dims and it was ready to go.
I use a method like skeleton, but planes are the driving force. The size cube for sheet metal box's and the gauges of the sheet metal are what need to vary in my case. I start by offsetting the 3 base planes and then create all my sheet metal on or related to those assembly planes. Move a plane or change a gauge.....boom everything updates. The sequence of events is key. My first two parts tically interact with each other, then the rest interact with the thickness of the first two parts.
Do you have some example?
See John Stoltzfus' first post to this thread, https://forum.solidworks.com/message/708077#comment-708077. You have to un-hide the sketch at the top of the Cabinet-9000.SLDASM file and make some changes and see how all the parts in the subassemblies update. Try for instance changing the "Total HT" to 55 inches and see what happens. Then change the OutsideBottomOfCabinet to 15 inches.
Matt Peneguy - Rob Edwards
Thanks for the kudos....
I don't use weldments, maybe I should. There is still a lot to be developed in the SSP process thanks for many people trying it in their work flow. A SSP component can be planes as mentioned by Scott Leacox or the SSP can be a combination of Solids, Surfaces, Axis or Sketches.
The SSP conceptual model is more of a methodical way of setting up your models so...
A. They are "Designed For Change"
B. Easier to diagnose any issues with your models
C. A quicker method to achieve Robust Models "Every Time"
E. Easier to change out components, so there are no "Forest Fires" in your feature tree (Anytime anyone sends me a model I do two things, 1. Randomly delete a part in the feature tree 2. Modify sketches - Robust models will not break apart when you do this.
F. If I were to go back to Machinery Design or rather any 3D modeling using SW, I would use the same method and principles
Like Matt mentioned it can be a challenge to learn, however once you grasp the idea and method your overall design time will dramatically drop, primarily because you only need to draw the shape one time, use either Derived Sketches or Convert to Entity. Another huge plus is the ability to work in different zones, preferably smaller Sub-Assemblies independently, while at the same time achieving a smarter Model.
Don't get confused with Master Part, Design Part or Skeleton Sketch Part, they are basically the same in one regard, they drive your entire or a portion of your model, whatever you desire.
Weldments work great till you change out profiles for new sizes.
Retrieving data ...