One complex part VS multiple parts in assembly

[Anonymous]

I'm designing a part that has many features and together it will be a unified unit held together with welding. How do I know if I should separate the features into individual parts if I can make the whole thing in one model?

[JDMather]

Who is going to make the physical real world weldment?

Do they need individual part numbers?

Do they need cut sheet?

Do they need individual 2D drawing documentation?

Probably a lot of other questions that should be answered.

One advantage to multi-body is that if you do end up needing assembly - it is easy to push out the assembly. (Manage>Make Components)

[Anonymous]

Thank you for following up with me.

Unfortunately those are some of the same questions I'm looking to get answered as I am in the design phase trying to have presentable files for when I find a manufacturer. (For context purposes: I am designing gym equipment and I want to mass produce the product with a Chinese factory)

I'm not familiar with what manufacturers look for and I'm hoping to find out if there is certain standards I can follow in order to prevent speedbumps ahead and I can't find any resources online. 

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"One advantage to multi-body is that if you do end up needing assembly - it is easy to push out the assembly. (Manage>Make Components)" 

I feel like you answered my question here but I don't exactly understand what you said.

What do you mean by "push out the assembly"?

Also does "(Manage>Make Components)" mean that its easier to manage components but harder to make components?

[johnsonshiue]

Hi! In Inventor, there are primarily two ways to design an assembly. 1) Create individual atomic parts and then assemble them in an assembly. You can reuse some of the parts.

2) Design the assembly within a part using multiple solid bodies. Each body represents a part. Once you are done with the geometric definition within the part, you can use Make Components command to push the individual bodies into parts within an assembly.

Please share an example so that experts can comment further on specifics.

Many thanks!

[Anonymous]

Great answers, unfortunatly I still don't know how simple or complex a part has to be in order for it to be presentable to a manufacturer. I'd love to share my files but a nondisclosure agreement wouldn't work in this setting.

[Anonymous]

Great answers, unfortunately I still don't know how simple or complex a part has to be in order for it to be presentable to a manufacturer. I'd love to share my files but a nondisclosure agreement wouldn't work in this setting.

[A.Acheson]

@Anonymous 

It really depends how much of a role you want to play in controlling the design. If these designs are just at concept stage and your looking for the factory to take on the rest of the designing/engineering /drawing creation then showing detail isn’t a priority. If you want to control the design more then you need to provide more detail.

Details cost , expertise cost, time costs.

A Multibody solid part might be much better in concept stage as you don’t concern yourself too much with real world sizes until your shape and approximate sizes are defined but you still have the ability to go back afterwards and change the solid body colours and separate the features into different solids (parts) to represent different materials like plastic, steel, glass, foam etc. These parts solids can then be made into an assembly of parts at the touch of a button.

Assembly environment

If you want to control more of the design and specify sizes using industry standards and you know you are  welding the frame etc you could use standard content such as tube,box, round bar, nuts,bolts, available in the content Center library to actually build a real world example in the assembly environment  will be more complete and easier to cost and visualize to the manufacturer.

This approach can be tricky as you will get stuck in the details and dimension of each part and the relationships get interconnected all too quickly.

A combination of both multibody to define the concept shape then apply the details in the assembly environment afterwards could work. 

Hope this  helps. 

[cadman777]

I NEVER use multi-body parts, b/c of the added work down-stream.

If you're going to manufacture these machines, then if I was doing this job, I'd make sure every single part in the machine is a separate FILE (.ipt). I'd segregate the plate/sheets as 'Sheetmetal' ipt's, and the rest of the parts as Standard ipt's.

I'd also 'atomize' all weldments as individual sub-assemblies. Same with all assemblies (such as a weldment with padding or plastic snap-in parts).

Fasteners can all be added per sub-assembly, based on the components that connect together from the most basic, working up to the top-level assembly. I separate into an individual assembly all the parts that mechanically belong together as an assembly. That's also how structural steel programs work. They GROUP all parts that are welded or bolted together (unless tell the program to do otherwise).

I make all my models as a hierarchy of parts and sub-assemblies from the most basic units, working up to the top-level assembly. That makes for easy data management, as well as drawing production. It may seem like a lotta work at first, but the pay-off at the end is much greater than having to chase around a myriad of tid-bits of this, that and the other thing. That will WEAR YOU OUT! Also, if something needs changing, it will only affect that immediate assembly and those things connected to it, not the whole model.

I NEVER use Inventor 'weldments' b/c they have too much overhead. If you have to show welds, then I do it on the drawing w/weld symbols. Same with weld preps, unless it's part of job prep, in which case the weld prep are features in the individual parts.

Below are a couple screens shots of a Smoker Grill I did. These show how I segmented this design. Look at the BOM to see the individual Weldments. Look at the Model Tree to see the same thing, with one of the Weldments expanded so you can see all the individual parts. When modeling, I always think this way: HOW will this be built IN REAL LIFE? So that's how I design it. Sometimes I have to change my approach mid-stream, b/c of changes in design (by the customer) or other factors (like computing overhead grows to excessive limits).

[cadman777]

Incidentally, on separate drawing sheets, every single part is detailed for cutting, weld-prep, flatpatterns for the burn table, etc. Also, all weldments are detailed with ISO-views/BOM + dimensioned ortho-views. I give the fab shop everything they need to build from scratch. All BOM's show materia, length, width, thickness, height, diameter, wall thickness, weight, and special notes. There's NO EQUIVOCATION when you look at my drawings. I've never had anybody come back to me over the years b/c of a bad build due confusing drawings. That's the key. Draw it so they can buy materials, cut it, prep it, fit it, weld it, fasten it, and totally build it.

[cadman777]

@A.Acheson - "A Multibody solid part might be much better in concept stage..."

Man, I've tried this a number of times, even tried it using the FrameGenerator.

And you know what?

It ALWAYS bits me in the butt at the end.

So I try to NEVER use MBP's, esp. when doing prototypes.

Same w/the FG.

Core Inventor never failed me yet!

[Anonymous]

Thank you Alan and Cadman for the different approaches. Both of your insight is extremely valuable to me and have answered many other questions that I didn't even know I had yet. And thank you so much cadman for sharing an example and going so in-depth for me.

Regarding my original question I think I can make it clearer using Cadman777's example:
There is a chimney vent on the side of the smoker that I would assume is two parts welded together. If I wanted to get that made for me, would it need to be two separate parts even though together-as-a-whole it is a chimney vent?

Is it simple enough to be presented as one whole part or does it need to be separate because it was joined by a weld? 

I attached a screenshot of the chimney vent anotated for clarity.

[swalton]

I design brand new machines.  I take them from concept to production.  I have worked with US-based, China-based and Tawian-based contract manufactures and vendors.

I work similar to @cadman777 .  I start with a paper sketch, or a concept model, or some other way to communicate the initial design and concept between the client and myself.  Once I have a clear understanding of the design goals, I start planning how to build the 3d models.

I then model each part and constrain them in an assembly to build the machine.  I make individual drawing files for each part and assembly so I control the shape, materials, finishes, tolerances, and special manufacturing notes.  That way the outside vendor or inside factory team can use the drawings as detailed instructions to manufacture every component.  Also, that level of detail gives me the ability to bid the work to several outside vendors.  I can get a better price, and have options if the relationship with any vendor fails.

It's hard to argue with a vendor about quality, material choices, or other issues if you don't give clear specifications and instructions.

Don't forget packaging, artwork, shipping layout, warehousing, customs....

I can't really answer your question about what is enough without reviewing the entire design.  

[Frederick_Law]

You need to know how it'll be manufacture.

Or your manufacturer is able to help you with design.

How the machine need to be split up depends on what you want and what the manufacturer could do.

Of course most can be machine from a solid block of steel but its not cost effective.

[cadman777 · Accepted solution]

The chimney vent would be part of the whole main weldment.

The 2 separate parts that make the chimney would be detailed separately on another DETAILS sheet.

I use basic drafting and design skills from the days when we did this on a board using pencils and vellum, only now it's easier to manage in 3d electrons!