Fusion 360 - Combine two complex bodies. Creating gradual step down filleted sections.

[hamzanabi123456]

Hi,

I have two problems with my design. 

Firstly, i'm trying to combine a body with a side section. However, it doesn't let me combine them together.

Secondly, can someone guide me on how to create gradual step down fillets from the existing edges of a body. The effect i'm trying to achieve is gradual filleted sections offset from the edges of the body (see pic 2).

I've attached pics to show this and also attached the fusion design file. Help would be greatly appreciated.

[ The subject line of this post has been edited to include the product name, and for clarity. by @CGBenner ]

[hamzanabi123456]

I've also attached the other component below.

[sutherland-]

Hi @hamzanabi123456 

I believe that you are not able to combine the bodies due to the fact that they are not "overlapping". I tried moving the smaller component towards the bigger component for 0.1 mm, then the "Combine" feature worked just fine.

[hamzanabi123456]

Thanks. Yes, i tried this and it works but does that mean that to combine bodies they have to be overlapping?. I wasn't aware of this i thought as long as the bodies were adjacent to each other the combine feature would work?. Seems abit strange for bodies to be required to overlap.

Also, is there a better way of creating something like this where gradual step down sections can be created at the edges of a body?

[sutherland-]

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@hamzanabi123456 wrote:

Also, is there a better way of creating something like this where gradual step down sections can be created at the edges of a body?

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Do you mean something like this?

[hamzanabi123456]

Thanks for all the replies. @sutherland- Yes something like that but closely reflecting what i've originally done e.g. at the edge of the body.

Can anyone recreate what i've done (that small body next to the main body swooping down the edge) but with a more elegant solution, i'm sure there is one. My way of doing it seems iffy. I would greatly appreciate it. 

@Bunga777 Thanks. I will check your method out. 

[TheCADWhisperer]

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@hamzanabi123456 wrote:

My way of doing it seems iffy.

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@hamzanabi123456 

Do you have Capture Design History enabled?

Are all of your sketches fully defined?

Are you willing to start over from scratch?

[hamzanabi123456]

@TheCADWhisperer  Yes, design history is enabled. My sketches are reasonably well defined, the thing is because i'm working with alot of curves and splines, i can't fully define the sketch but this hasn't been an issue.

It's mainly trying to figure out how to incorporate complex feature designs into the model. 

I want to share my design with timeline as that would be ideal but i kind of want to keep it private as its an internal design. Is there a way of sharing design on fusion with just a select few members on the forum?

[TrippyLighting]

Please share the complete design with the timeline enabled!

[sutherland-]

@hamzanabi123456 

No it is not a requirement that bodies need to overlap, but seems like in your case it works out that way.

[sutherland-]

You could also try to follow those steps to overcome this error.

[Bunga777]

I went so far as to composite and fillet from the file you attached.

First, offset one part so that the parts overlap completely.

Combine the two parts.

Fillets are attached.

However, in the fillet at the end, the configuration of the surface is not clean, so it may be an area that needs a lot of work.

[Bunga777]

You can send private messages privately, and it is a good idea to share data only with trusted users to solve problems.

[davebYYPCU]

It’s way more complicated than that.

Private messages do not accept files, just pictures.

You password protect the shared file and post in the forum the file,

and 

you create the private Message, and share the password to your audience.

PITA for some.

Might help....

[hamzanabi123456]

@davebYYPCUThanks. for the method. I've shared a link along with a message to some of you guys.

However, i can't send more links because there's a limit on how many private messages i can send so i will send the link to the others which i've missed by tomorrow. 

Also, if someone has turned their private messages off, naturally i can't send the link this way.

Can you guys check your messages and reply if you can help further. Thanks as always.

[TrippyLighting]

I am looking at your design and I would start this again from scratch!

Lets start right with the first sketch.

1. Your sketch is not fully defined. If you need to use splines, use control point splines with the least number of control points. That is then much easier to dimension and constrain. 
2. I would not use conic curves. If you want a smooth curvature transition, then use control point splines.
3. Do you even need to use splines? What is the reason you are using splines vs. arcs? (Just to be clear, there are good reasons to do so, but if you don't know those reasons, there is no reason for you to use them!!!)
4. Do not mirror an entre sketch! Sketch half, create geometry and then mirror the geometry!

Whoever designed that reference housing also wasn't exactly a modeling wizard 😉

5. You use to many spline control points as can be seen by he wavy curvature comb. Start with a 3-degree control point spline with 4 control points. If that does not give you the shape you're looking for, use 5 degree control point spline with 6 CVs.

[TrippyLighting]

Also - I should have asked this at the beginning - how is this going to be made? 3D printing ?

[hamzanabi123456]

@TrippyLighting Thank you for the feedback. Yes, this is my first model which i'm creating in fusion so i'm definetly learning. I've already learnt quite alot from the really helpful people such as yourself on the forums here.

The idea is to create an enclosure like this and then have it manufactured (injection moulded) as a series production. However, that is the long term goal, for now i think the first prototype will be 3D printed i guess. 

I really appreciate your feedback. I would be grateful if you could correct some of the things on the sketch based on the things you outlined in your post, maybe trying to fully define my first sketch as i can't seem to define the spline points (if you have some free time, the more fixes the better 😁) and send the updated file back privately. You are correct about the splines because i couldn't define the spline geometries on the sketch. 

Also, what disadvantage am i likely to have or difficulties will i face if i use an undefined sketch in the design?. I know the main reason defining a sketch is so that it allows easy changes to the geometry of the design as everything is referenced.

However, is there another reason why fully defining a sketch is essential e.g does this cause problems later on during design modelling?. 

[TrippyLighting]

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@hamzanabi123456 wrote:

The idea is to create an enclosure like this and then have it manufactured (injection moulded) as a series production. However, that is the long term goal, for now i think the first prototype will be 3D printed i guess. 

If it will be injection molded, everything needs at least 1 degree or more of draft, so it can be pulled/released from the mold halves. You should consider draft and split line for the mold halves right from the start.

[hamzanabi123456]

@TrippyLighting I udnerstand what you mean about the degree of tolerances in the design required for injection moulding.

Ideally, if it's not too much to ask, can you make a few edits to my design which will be saved in the timeline and pm me back, after which i can analyse and work from those edits, it would be even better if you could provide a summary of the reasons for the changes you implemented into the design.

Many thanks as usual for the continued support, much appreciated 🙂.

[TheCADWhisperer]

Can any of the splines be replaced with more primitive (basic geometric math) arcs that would still be well within any possible manufacturing tolerance without violating your true Design Intent?  (In my opinion any new user should have at least 6 months of instructor led training before attempting spline based geometry.  Full disclosure - I made my living teaching CAD, so I might be considered biased. And before that I worked out on the shop floor where I appreciated geometry that could be made with standard tooling/techniques.)