Assembly Parts and Manufacturing Best Practice.

[kylematthew159]

I've been using F360 for years now at this point as a machinist and one thing that has always perplexed me is the figuring out the recommended workflow for assemblies and then machining individual parts.

I prefer a more top down design approach utilizing parameters to lock everything in and adjust variables when needed. To utilize these parameters You have to make all the components internal. I know you can export and import them but that is clunky in my opinion... and I don't like doing it. Furthermore as you're going along in your design and add more parameter, you have to reexport and reimport parameters for any eternal components. So its best to leave everything internal.

My frustration comes from when its time for to machine the parts, you have 2 options i think. Option 1 is machine all the parts internally to model. This gets messy fast when you have multiple setups on multiple parts... Option 2 is to "Save Copy As" the component externally but the catch is, if you fully program the part for machining and then make changes to the part, you have to reprogram the entire parts. 

Option 2 is the method I go with for now but am I missing something? Is there a better way to keep the assembly all internal so design changes and parameters can be used, shared and synced between components but also be able to separate the CAM side of parts for organization purposes, WHILE keep all the benefits of parametric modelling and part updates and revisions? Does all that make sense? Can someone help guide me on the correct way to go about this.

Thank you!

[Drewpan]

Hi,

When you are setting up Engineering Drawings and Manufacture Tooling Code

you don't have to select the entire Model. One of the reasons Fusion is set up

with Bodies and Components and Components that can be grouped into

Assemblies and Sub-assemblies is so that you CAN pick and choose. The Design

Method can be Top Down or Bottom Up, Internal or External or a Hybrid of all

of that. It makes no difference to the actual Model how you arrived at the end

result.

Most of the Post Modelling  functions in Fusion begin with the Model from the

Design area. If you simply want Engineering Drawings then you select the Model

or parts of the model, go to Drawings and press the buttons. Similar with

Animation, you only select the bits you want. If you want an exploded model that

has ALL of the bolts and screws and nuts and washers then you select all that. If

all you want is the major Components and Assemblies then you turn off the

Hardware before opening the Animation Tools.

The same functionality will quite happily work when creating the Manufacturing

CNC code. You only pick the stuff you need and then open the Tools. If you have

designed an Engine but only want to CNC the Block because the Piston Assemblies

and the Rings will be Off The Shelf then simply select the Block and go for it.

In terms of Workflow there are some things that make no difference at all and

some things that are critical and you cannot avoid. If you make major changes to

a Component then it will make little difference to Drawings and Animations because

all you need to do is simply hit the Recalculate Button and it will Automagically

update the Drawings and Animations. Programming CNC however is quite a different

function because some CNC might be able to be easily updated by pressing the

Button, but other stuff might mean radical changes to the Code. You cannot really

avoid this bit.

The new Fusion Part, Assembly and Hybrid Workflows exist because different groups

who use fusion in major Manufacturing and large scale Production have asked for

this functionality. The only real difference between an Assembly and a Hybrid is that

you are more likely to have Parts and Assemblies designed by multiple Teams and

those things are likely to be imported into a single Design. It doesn't really change

your Workflow because the only real difference is YOU didn't design that Part. It is

very similar to importing a Part from the McMaster-Carr Cattledog except you cannot

modify External Parts as easily.

Whatever method of Design you use the only really important thing is to keep it all

Logical and easy to follow. Once you find a system that works for you often that is

the system you will use all the time. If you want to Design Part by Part and do all of

the Drawings and Fabrication stuff as you go will work just as well than if you leave

it all to the end. All of this stuff is done using the Fusion Model. Fusion doesn't care

if you haven't finished a major Component or Assembly. If you select another critical

Part that you can start Fabrication and it will not be changed down the track then

Production comes down to what efficiencies and cost savings you can generate along

the way.

Only select the Components you are ready to use and take the next step with. It is

highly unusual to fabricate nuts and bolts so you just don't import them into your

Manufacture Model. Works the same for other Components within the same Model.

Cheers

Andrew

[TheCADWhisperer · Accepted solution]

Derived Components

[kylematthew159]

Hello, I understand what you're saying but if you have an assembly of 20 parts and at least 2 setups per part, that's like 40+ setup to manage in the CAM tab. Obviously I don't need to manufacture typical fasteners and stuff. Like I described, the easiest way to make an assembly is to do so internally where you add new components inside the assembly file. That way you share all the functions, parameters and you assembly stay truly parametric. But doing it this way makes the manufacturing organization a bit harder. You can make the components external but then you lose a lot of the things that make assemblies parametric... Does that make sense? 

[John_Wright]

Im with @TheCADWhisperer, "Derive" is the tool you want to use.

Make a new file & "Derive" the part (body) you want to machine into it.

If you update your original model, then the derived parts will update.

I design and make injection mould tooling. This is the workflow i use for each plate in the die-set.

[kylematthew159]

Hello, thanks for the response. This seems to be backwards from what I'm thinking unless I'm not understanding it correctly. My typical workflow is Create the assembly file, draw the skeleton model and setup some parameters. From here you have 2 options, create your part components internally or externally. I guess this decision branch is the main issue. Creating parts internally lets you easily share the functions, parameters and thing that keep the assembly parametric. The down side then you have 1 file for all CAM data. If your assembly has 20 parts with at least 2 setups per part that 40+ setups in 1 assembly file. (I'm going to keep typing but I think it just clicked by how derived components could help here.) If you create your parts and save them externally, you get the separation on the CAM Side keeping it organized but on the design and assembly side you lose a lot of parametric features that make designing intuitive. 

So I just tested some things out the and I think the command you were referencing was the "Insert Derive" command correct? This is one pretty much exactly what I was talking about. You're able to design a full assembly and keep all the part components internally. Then you just have to start a manufacturing file for each part you want to machine, "Insert Derive", select the part and then you have a separate but linked part to work with! This method works great. The only change I would make, would be making a toggle or something in the "New Component" menu that if you saved a part externally, you could select an option that would give the external part, the "Insert Derived" functionality. This way would wouldn't have do to the extra step of saving the assembly, creating the manufacturing file and then select the part component for machining. 

Thank you for your help, this works perfect for now!

[kylematthew159]

Yes I just responded to him and figured this only. If you read the bottom of my response to him, I think we could add a nice feature to the "New Component" menu that would allow us to skip and few steps. Thanks for the response! 

[John_Wright · Accepted solution]

There is a "create derive" button under the create menu. That will make a new file for you. I think that will be what you're after. It certainly works for me.

[kylematthew159]

That's dam near perfect. Thank you very much!

[kacper.suchomski]

If you don't need additional fixture models, you can easily manage setups in a single hybrid file.

You can also isolate views within the CAM module to facilitate ongoing work on a specific NC program.

[kylematthew159]

Thank you for the reply and demo.