How to tell How a Body (or Component) Sits w Relation to Another Body or Component

[pittsallen]

Hello Fusion forum.

Now in about the thirtieth hour of diligently following tutorials
by running the tutorial on the iPad while the steps are followed exactly
on the PC with the F360 app running. The tutorials are repeated
over and over because the instructor says something like
'use the mouse to increase the dimension' when what is meant
is 'press down on the mouse wheel and move the mouse wheel while it
is pressed down.' So the process must be repeated until the correct
process is stumbled upon. Painstaking and tedious.

But a great deal has been learned.

However, the assumption is that by following the tutorial, that the knowledge 

needed to create a model, which is quite different from model in the tutorial,
will be happened upon or extrapolated from the method used to create the tutorial model.

So please forgive some basic questions to get me off high center and move
along.

The context is that the part that is needed is shown in the attached
drawing marked Staircase LED Fixture Double Receiver.

The socket bottom and the round body above the socket have been
sketched and extruded in F360 and is marked Socket Bottom
and Round Body.

It is hoped that it is ok to ask more than one question in a forum
post. If it is not, I will withdraw this post and separate the questions.

1. Can it be known if the Round body sits on the top plane or the bottom
plane of the Socket bottom. If so, how can this be determined?

2. Should the Socket bottom and Round body be separate Components
or separate bodies? (Most of the advanced features of F360 like
movement studies, joints, injection mold simulation and collaberation
are not needed.)
Is the method for joining Bodies different from joining Components?

3. Are Components and Bodies created and then joined or joined as they are created?
4. The next step is to add the Lens plate. Should the Lens plate be begun
as a Body or Component? Can Components be begun as a Sketch or can
only Bodies be begun as a Sketch?

5. Is there knowledge of any type of interactive class or instruction,
even if it was a talking head that would allow queries at a specific, limited time?
I have resources and am willing to patiently go through the tutorials
but quite often a tutorial is followed that has little or nothing to do
with goals that are the challenge.

Thanks.

Allen Pitts
@jhackney1972 
@laughingcreek

[davebYYPCU]

Appears that the yellow body would be made of various features.  A single component.  Following Rule 1, build your yellow component first, with all sketches and features required in the Component, and grounded.  Your file structure is not right or wrong, will just take some steps to combine all to one part when completed.

The Lens will be the second component.  Built in place, using articles from the yellow body to build it.

As many questions about this model here in this thread, is best method to get this one done.

1. Depth of Socket is determined from where you measured it from, using same items in Fusion.

2. As said both of your parts would be in component 1, and will be joined in the Extrude process to maintain one body as you proceed.

3. Components are Joint(ed) together, Bodies are joined in process.

4. Lens is second Component, is a simple extrusion of the floor outline less clearance.  Built in place will be parametric and adjust if modified.  Many ways to make it, but finish the yellow body first, the Lens will be much easier.

If it were me I would likely build the lens first, and build second component from it.

Don’t have any recommendations for tutors, but the are 6-8 of the regulars here that will keep you going. Some us can do detailed stuff by PM.

When stuck, attach the file to a message here and ask away.

Might help.....

[jhackney1972 · Accepted solution]

---

@pittsallen wrote:

1. Can it be known if the Round body sits on the top plane or the bottom
plane of the Socket bottom. If so, how can this be determined?

Without the model it is hard to tell.  I would model the tube from the face of the washer, guaranteeing they are attached.  If you check the Browser after making the tube extrusion you will not it is one body meaning the tube is attached (joined) to the plate.

2. Should the Socket bottom and Round body be separate Components
or separate bodies? (Most of the advanced features of F360 like
movement studies, joints, injection mold simulation and collaberation
are not needed.)

It would seem to me that this whole model (yellow one in your post) could be one component.  It seems to be a solid continuous entity.

Is the method for joining Bodies different from joining Components?

Yes, joining a body will fuse the material together just like the video shows above.  As one body joins another, they are joining into one body.  Components are Joined together using Assembly Joints.  They attach components together with different degrees of motion.  For example a wheel component is joined to an axle component with a Revolve Joint so it will be joined to the axle, in a particular chosen location, and will freely rotate.

3. Are Components and Bodies created and then joined or joined as they are created?

Bodies can be created joined together, as shown above, or can be joined together, if and only if they have contact, using the Combine command.  Components are joined together, using assembly joints, after they are created.  There may be exceptions to this but I cannot think of one right now.

4. The next step is to add the Lens plate. Should the Lens plate be begun
as a Body or Component? Can Components be begun as a Sketch or can
only Bodies be begun as a Sketch?

You need to learn Rule #1.  I have added a hyperlink for you.  The video will show you how Rule #1 works.

5. Is there knowledge of any type of interactive class or instruction,
even if it was a talking head that would allow queries at a specific, limited time?
I have resources and am willing to patiently go through the tutorials
but quite often a tutorial is followed that has little or nothing to do
with goals that are the challenge.

I am sending you a Private Message which you can retrieve by clicking on the envelope.

[pittsallen]

Hello davebYYPCU

'Following Rule 1, build your yellow.....'
What is Rule 1?

'with all sketches and features required in the Component, and grounded. ...'
What is grounded?

Thanks.

Allen Pitts

[Bunga777]

@pittsallen 

I think Rule1 is what is mentioned in this thread.

https://forums.autodesk.com/t5/fusion-360-design-validate/fusion-360-r-u-l-e-1-and-2/td-p/6581749

[Bunga777]

I will answer one by one with my own views.

1.   Either one is fine. It depends on the intention of the producer. But whichever you choose, the desired shape can be the same.
2. We think of a body as a single piece of material, and a component as a collection of objects. Parts that have no functional behavior and can be handled as a single collection of objects in CAD are grouped into components. For example, a lot of screws attached to a part are the first parts that should be a component. If there are many of them as bodies in a single file, the design becomes complicated and slower. These parts should be components. Also, moving parts should be separate components, otherwise the joint function cannot be used.
3. Components should be made as soon as you think you need them. Ideally, it should be the first thing you do when you start making each part. Once you have made the sketch at the top, it will not move to each component even after you have converted the part to a component. This specification is very troublesome, and we feel that we want to create the component first to avoid this.
4. I would make one component and one body, since all the parts appear to be one piece from the diagram. As mentioned above, I would create the component first and start fabrication there.
5. There are many people on this forum who can give you guidance if you indicate what kind of part you would like to end up making. If you have any questions, just write down the diagram, the data, what you don't understand, and what you want to do, and someone will get back to you as soon as possible.
   If you want to make a part like the one in this example, I would suggest that you focus on the solids first, and then learn additional surface features. With solids as a base, additional knowledge of surface operations will be a powerful weapon when designing parts.

[TrippyLighting]

This is Fusion 360 R.U.L.E #1 &2

It would help if you understood the difference in purpose between components and a bodies.

A body is a contiguous piece of geometry. A component can have more than one body, but in most mechanical designs there is only one body in each component.

A component is a collection, or container of all those objects that are used to create that body (or multiple bodies). It also contains (explicit) joint origins that can help to assemble these components into a functional assembly/

For mor components with complex geometry it is not unusual to have multiple bodies during the design process that might get combined into one body at the end.

Generally you can think of a component as one discrete functional part. 

[davebYYPCU]

Grounded / Grounding, is applied to each new component, unless it is replaced by a Joint.

Right Click on the Component name in the Browser, Select Ground at top of Menu.

All Fusion New Components are free to click drag move by intention or accident.  Best to Ground both of your components as step 1 in each.  You model would not have any motion in the static position.

Others have already pointed to Rule 1, and I have not watched John’s video.

Might help.....

[pittsallen]

Hello @davebYYPCU, @jhackney1972, @TrippyLighting, @Anonymous and the Fusion forum,

Sorry guys. Forgot to attach the file. I suffer from ADD (Attachment Deficit Disorder).

davebYYPCU
Thanks for the tip about measuring as a method to discover if Round Body sits on the top plane or
the bottom plane of the Socket Bottom. Not sure why I did no think of it. By measuring
the Round Body sketch it is found that the the depth of the Round Body is 38 mm
and the depth of the Socket Bottom is 1.8 mm. So if the Round Body is joined to the Socket Bottom
at the lowest plane of the Socket Bottom the two parts joined together would be 38 mm.
If the Round Body was joined to the Socket Bottom at the higher plane of the Socket Bottom
the dimension of the two parts joined would be the sum of those two dimensions or 39.8 mm.
The key was finding out that the Measure tool is in the Inspect tab and then fiddling with the
Measure tool until predictable results could be achieved

jhackney1972
The short video on the post marked "Message 3 of 8' is spot on.
Things pointed out in the video that were previously unknown
1. The part w title 'Staircase LED Fixture Double Receiver' in Message 1 of 8
can be one Component.
2. The cylinder marked 'Round Body' the part w title 'Staircase LED Fixture Double Receiver'
in Message 1 of 8 can be extruded by using the Offset tool to create the cylinder wall
as opposed to the way it was done in the attached file which used the Thin Extrude
feature of the Extrude tool. This seems to be an example of many instances in F360 where the exact
same result can be achieved using different methods.
3. When extruding one part from another the Extrude Operation Join is available to make sure the
the cylinder (Round Body) created on top of the disc (Socket Bottom) is joined to the disc.
Experimentation with the two methods, extruding using Thin Extrude and extruding using Offset
from a circle reveals that the Thin Extrude method creates a part whose height 38 mm where the
Offset circle method creates a part which is the sum of the height of the disc and the height
of the cylinder or 39.8 mm.
4. Counting the number of bodies in the Browser confirms that the disc and the cylinder
are joined because if the disc and the cylinder were not joined there would be two bodies instead
of one.

"Components are Joined together using Assembly Joints....." If this true, since the three parts
required for the Staircase System have no moving parts and autonomous, each of the three
would be a file with on Component and a number of Bodies.

I am amazed that in the dozens of hours of tutorials viewed in the Self Paced Learning section at
https://help.autodesk.com/view/fusion360/ENU/courses/
that Rule 1 & 2 were never mentioned.

It seems that Components can contain Bodies, Sketches, Origins, Planes (called 'Construction' in the Browser).

TrippyLighting
I am amazed that in the dozens of hours of tutorials viewed in the Self Paced Learning section at
https://help.autodesk.com/view/fusion360/ENU/courses/
that Rule 1 & 2 were never mentioned.
It seems that a Component can have multiple Bodies. And if this statement is true
"...A component is a collection, or container of all those objects that are used to create that body
(or multiple bodies). ..."
then Bodies can have multiple Components.
The most prominent feature of Components, it is surmised, is that Components can be used in Assemblies
where as Bodies cannot be used in Assemblies.
The video titled "Components" was very helpful.

davebYYPCU
The Grounding concept would seem to be an important element for the Staircase System in that there are no
moving parts and knowing where the elements of the Component are is needed.

Bunga
"make one component and one body, since all the parts appear to be one piece from the diagram."

The realization is the F360 will do all kinds of things like injection mold simulation, movement
analysis and CAM related processes that are not needed on the relatively simple Staircase System (residential
architecural LED lighting). And so the idea forming is that the challenge in learning F360 is isolating,
out all the incredible number of features in F360, those features that are required to design and
3D print relatively small and precise static objects.

Thanks for your time and courtesy

Allen Pitts

[etfrench]

Note that the Measure tool is only accurate to the precision level set in Preferences. This can cause problems with near coincidence when positioning bodies.  It's better to use components and joints or when extruding use To Object.