Fusion 360 help please.

[ukracer]

That is how it is done in Design Spark Mechanical and it seemed to be the most logical. I'm not getting on too well with Fusion, even a simple thing like saving an .stl to disc is eluding me. It only want to save it into Cura.

AH I can see I had the same problem. You need to export it I believe.

 

[ajlelectronics]

AH I can see I had the same problem. You need to export it I believe.

I worked it out! Select the item to print, click on the save icon, select 3D print, untick "save to application" and show it where you want to save it.

 

[ukracer]

I worked it out! Select the item to print, click on the save icon, select 3D print, untick "save to application" and show it where you want to save it.

Ah straight to cura without export then.

I am finding this thread very interesting but sadly I am.not understanding much of what's being said.
It's ideal when I am back in my quiet place at the static but we stopped going due to cold weather till March now.

Perhaps once I decipher whats being said I might understand the packages better.

 

[daedalusminos]

I worked it out! Select the item to print, click on the save icon, select 3D print, untick "save to application" and show it where you want to save it.

I usually right click on the body in the browser and select save as mesh

 

[Anguz]

I normally export as stl

 

[ukracer]

I normally export as stl

I got something right then

 

[Misterg]

Start a new assembly, bring your existing flange in as the first part, locate it at 0,0,0.
Draw the other part, save it as a part, then bring it into the assembly.
Mating conditions to stick them together.

Sort of, but by default, F360 *starts* in an assembly, and for simple things like this the parts (components in F360 speak) are best nested within the assembly in one file.

However that extrusion appeared not to be a separate part, but becomes part of the base. How should I approach that please?

Individual parts are called 'Components' in F360. Components are made of 'Bodies'.

When you do the extrude (or any similar operation) there is an option to control what happens. By default, it's usually set to 'Join' - so the piece you're creating becomes part of the parent body.

You could choose 'New Body' or 'New Component'. The "right" thing to to is to make a new component, however I don't like doing this during an operation like this as you end up with one of the sketches controlling the component inside its parent. As we're not working on a complicated assembly it doesn't really matter except that it can get confusing as you move to more complicated assemblies.

What I think you should have done is created a new component and called it 'Vent Hood' or something, selected that component and then started sketching. Everything defining that component is then under one roof.

[As an example of the sort of structure: In the screenshot above, there are 5 main components marked with green arrows (not all are visible - look at the icons next to the names). The 'Binding Guide' component is made up of 4 components (orange arrows), one of which - 'Shaft' includes another 2 instances of the same component (purple arrows).]

As above, when F360 is in Design mode, the default is that you are working in an assembly. It will happily let you start modelling, but really, the very first thing you should do is to create a new component - e.g. 'Vent Base', select that component and *then* start modelling it. (Indeed there's an argument that you should create all your major components before modelling anything.)

Note that if you're working with components, you need to join them, or they can be dragged out of position accidentally. The easiest way (without getting into Joints) is to create an 'As Built' joint between the two components - look for the icon next to the green arrow in the 'Assemble' drop down. Click that, click both components and 99% of the time you're done. I use it so often that I've put it as a tool-bar button.

As regards visualising the assembly, there's an option under 'Inspect' to 'Display Component Colours' that shows adjacent components in different colours:

There are loads of different tutorials on Youtube about the differences between bodies and components - I found this video quite good (though I find some of his other videos very laboured):

 

[ukracer]

"What I think you should have done is created a new component and called it 'Vent Hood' or something, selected that component and then started sketching. Everything defining that component is then under one roof."

Interesting. If I understand this correctly I am always doing things wrong to start with.

I really must start videoing my failed attempts at using fusion.
It might help others (as well as me) if the correct method/action were identified.
All I need to do is find the right platform (I am guessing) a forum is going to be better than youtube as it happens.

 

[Erie Fred]

Aha !
I'm driving Inventor these days.
Hence the differences.

 

[Misterg]

If I understand this correctly I am always doing things wrong to start with.

I did, for a long time after moving to F360. The 'lightbulb' moment for me was realising that what you're creating is an assembly, not a part/component. Therefore, the first thing to do is create your component(s) within that assembly before you model them.

It doesn't really break anything by not doing this, but it goes against the logic of parametric design and makes the whole thing get quite confusing quite quickly.

 

[Misterg]

'm driving Inventor these days.
Hence the differences.

I haven't used inventor, but came from Creo / ProEngineer which operated exactly as you described. It caused me some confusion when I no longer had access to this and had to move to F360 for my personal stuff.

You *can* use F360 that way, and for complicated, multi user projects it would be a 'no brainer'. There are restrictions in the "free" / personal use version that make this more awkward than it needs to be, and a restriction on the number of editable files that tends to work against it, also. (But there really is no need for anything less than something with the complexity of (say) a car engine.)

 

[daedalusminos]

Interesting. If I understand this correctly I am always doing things wrong to start with.

Not really wrong, just not as good as they could be. To be honest I would get used to modelling with F360 first - because you can't do anything until you grasp that. Forget components and assemblies of components for now it's only when you get to the point of wanting to reuse parts of your design or move individual parts about that you'll get the real benefit of components - for this vent consisting of flap, shroud and duct 3 bodies and a few sketches is fine.

Incidentally, don't get stuck in having to copy the original exactly - for this I would think it just needs to be form, fit and function to the original (which was probably designed for high volume injection moulding). You could consider a living hinge for the flap and try and print all in one (or two).

 

[ajlelectronics]

Whilst appreciating that this is running before learning to walk, I would like to design a smart watch charging stand. This is for 'indoors who can't ever get the magnetic connector to engage. My idea was to photograph it, clean up the outline and then somehow mould a casing around its contours. I gather that Fusion can do that?

 

[daedalusminos]

I would create a model of the watch back in F360 and then subtract this model from your basic charging stand model.

To create the watch model you can take a photo, insert it in F360 as a canvas, calibrate (scale) it and use that as a guide for your sketch outline, then extrude that sketch. If you need to capture more detail on the back then create a tool to cut the profile as they would when manufacturing the case

 

[ajlelectronics]

I would create a model of the watch back in F360 and then subtract this model from your basic charging stand model.

To create the watch model you can take a photo, insert it in F360 as a canvas, calibrate (scale) it and use that as a guide for your sketch outline, then extrude that sketch. If you need to capture more detail on the back then create a tool to cut the profile as they would when manufacturing the case

So what you are saying is that the photo needs to be traced as a sketch?

 

[daedalusminos]

Sketch of outline (you'd trace round a photo):

Sketch of half profile tool to 'cut' the case back

Extrude case, revolve tool to creat ebodies and cut one from the other:

 

[ajlelectronics]

You make it sound so easy.

 

[bricol]

I do it this way, after years, many years of work, of having to always make changes midstream.
Damn customers.

Also, I have found out the hard way, that the longer method i described is better when you need to re-visit the files a year later for changes.
You can clearly see the parts, the mating, the links, etc.

Having to call up some one else's work when done the "tricky slick" way, and make changes, things go sideways real fast.

the amount of time I've wasted trying to work out how the flippin' 'eck some f**kwit has manged to create something in some excessively complicated, over-the-top, time consuming way! I swear one of our recently retired contractors, when sat working from home during Covid was working out ways to make things as incomprehensible and slow to work with as possible for the next poor sod to work with it! Features constrained to planes, positioned with dimensions, when a simple dimensioned sketch worked better.

Last week, I could not work out how another colleague who started, and left, during Covid (so I never met him) had modelled something - just incomprehensible and I've been using NX for well over a decade! Another respected colleague couldn't figure it out either. But then again, the ex-colleague has masters and CEng . . (not yet met one who could actually do anything sensible practical, including a life-long mate of mine!), so what do I know ?

We won't mention flipping dimensions like 22.9mm, when for what he was doing 23, or 22, or even better 20 or 25, would have worked fine (I personally like to stick to sensible whole numbers if I know it will be made by a person with a rule, centre-punch and a hand drill - just quicker/easier to mark off). I often find the "real" dimension in the model is 22.8789876543210001112999 because the clown used the synchronous function to drag stuff around approximately, rather than nailing down with a proper, sensible dimension, rounding off in the drafting side of things to get semi-sensible numbers.

And use the "hole" function if has one - then the poor sod editing it later can quickly and easily edit, rather then mucking around with the extruded circles, especially buried in some other extruded sketch - and in most CAD systems, the hole command allows assembly patterns to be used to throw fasteners in quick and easily, patterns that then respond to changes in dimensions.

I still don't really get this 3D printing thing - spend hours modelling, hours printing, using a good few quid of material and power . . . for a two quid part that will be better, last longer and fit . . . but then I have full multi-million quid machine shop at my disposal (sort of ), and people who know how to operate it

 

[ajlelectronics]

I still don't really get this 3D printing thing - spend hours modelling, hours printing, using a good few quid of material and power . . . for a two quid part that will be better, last longer and fit . . . but then I have full multi-million quid machine shop at my disposal (sort of ), and people who know how to operate it

Small scale / home prototyping and generating parts that are impossible to buy.

 

[ukracer]

You make it sound so easy.

It's frustrating isn't it. Lol