Fusion Rule #0 - How to effectively learn Fusion

[Drewpan]

[Post modified by moderator to remove "360"]

Fusion Rule #0 - How to effectively learn Fusion

The Fusion Documentation has a full explanation of commands and a number of excellent
Tutorials embedded within. They can be found here:

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-1C665B4D-7BF7-4FDF-98B0-AA7EE12B5AC2

The Fusion Self Paced Learning has a series of step by step videos to get you started on
your learning journey. They can be found here:

https://help.autodesk.com/view/fusion360/ENU/courses/

The AutoDesk YouTube Channel has excellent general purpose learning tutorial videos and explanations.
They can be found here:

https://www.youtube.com/@adskFusion

Some of the Gurus lurking in the Forum also have great YouTube Channels, like this one:

https://www.youtube.com/@TheCADWhisperer

Warning: There are Cowboys on YouTube, not everyone knows what

                 they are doing. These links all DO know what they are doing.

General Tips for learning Fusion

1. Sketches should be simple and fully Constrained to prevent problems later.
2. If you can't find where the Sketch is unConstrained (no Lock icon) use the Text Command
    Sketch.ShowUnderconstrained

3. Dimension critical stuff and constrain the rest.

4. Work logically. The Browser tree is your friend not a beast to be wrestled to the ground and tamed.

5. There is more than one way to kill a cat than drowning it in butter. There are also many ways to do the

    same thing in Fusion.

6. Learn to use the Timeline early and fix issues with it WHEN THEY HAPPEN. If the timeline is yellow
    or red and you didn't fix it then that is probably causing you grief now.
7. Sketch simple and use the Tools to sculpt your models. Fancy Sketches are easily broken and sometimes
    hard to fix.

8. Refer to Rule #1 and Rule #2 OFTEN.
9. Practice a lot. Draw what interests you for fun, it makes learning much easier.
10. Challenge yourself. Give it a shot. Ask for help when needed. Follow through to the end. Look back and
      see what you have achieved. Reward yourself for the improvements.

Requirements for asking for help in the Forum.

1. If you have a problem then ask a question.
2. Attach your File and a picture or screenshot of the behaviour or what you want to achieve.
3. If your File is proprietary, create an example of the behaviour to share and upload that. Re-creating
    the behaviour may either solve your own problem or prove it may be a genuine Bug.
4. Gurus and Developers lurk in the Forum. Be nice to everyone but especially them!
5. Be humble if someone is pointing out things you have not seen or be aware of. They are NOT aiming a
    personal attack at you they are trying to help you learn.
6. Never stop learning.

[TheCADWhisperer]

---

@NNJ115679 wrote:

Please sir give me something learning information about autocad 

---

@NNJ115679 

Post your AutoCAD questions over here...   https://forums.autodesk.com/t5/autocad-forum/bd-p/706

[jacobsebasitan_98]

Thanks

[thefdownloader]

what are the pros and cons of fusion and it's best alternatives?

[TrippyLighting]

---

@thefdownloader wrote:

what are the pros and cons of fusion and it's best alternatives?

---

Please create a new thread for such questions!

[Steve_Worley]

I found this very helpful. Thank you for taking the time to post. What I am missing is how to think, and I'm having trouble knowing what to search for and where to post. If Fusion is used for "Top Down" design, it would make sense to leverage the geometry in components that have already been built for the coordinate system (origin) on the next component you are building. For instance, if I want to move the origin of component 2 to the location of the center of the top hole in the component, is there a way to just "click" on the diameter and have the origin move there? This way, each new component would be built in the assembly in the proper location, and all mating components could leverage the geometry (holes would always match up, errors would be caught during the sketching process, etc.). I know I can move the origin and save the new location, but it would be much nicer just to select something and have Fusion do the work. I guess I am saying that even if someone in this forum could tell me how to do it, do I want to do it?  I'm trying to understand the "why" of doing things right now more than the how. If I learn the "how" before the "why" I'm afraid I'll spend just as much time unlearninng things as I did learning them. Hence my comment on leaning how to think. If I have an assembly with 20 separate components, is there a best practice for origins? What are the unintended consequences of my thinking? Help pointing me in the right direction would be appreciated.

[Drewpan]

Hi,

I am a student still myself and what I aim for is to work logically to a standard that I think an engineer would/should

work to. I am still a work in progress and the Gurus on this forum critique and offer suggestions constantly. I am also

a strong believer in work smart not hard.

I have found that the documentation has great tutorials and the self paced learning is great too. As I have said, the best way to learn is pick something that interests you and model it. Ask questions when you get stuck and be humble.

There are many different ways to design things, top down and bottom up are two of them. I try to design as if I was in

a design team and I have been given a component or assembly as part of a team. How would a real engineer do this?

I am far from perfect but I improve constantly and that is the main thing.

There are two main methods of design: design in place and use In-built Joints; and design at the Origin and use it and

the associated planes then use a normal Joint to put it where it goes. Both methods are valid and have their place. Try

to think how an engineer would do it.

TheCADWhisperer is a Guru on these forums and has a great YouTube site. Just be careful who you learn from as there

are a lot of self-taught amateurs who DON'T think like engineers.

Keep going and good luck. Remember that RULE #1 and #2 are also there to help you.

Cheers

Andrew

[thatotherfellasbrother]

Yes, I have tried to keep my learning to the recommended contributors. There are many ways to approach a design, and I'm very new myself. I completely understand your interest in learning the right way instead of trying to unlearn bad techniques.

I found this tutorial about the BORN technique from the CADWhisperer very interesting https://www.youtube.com/watch?v=YyQHEKrT8bo. On the other hand, there are several commands under the Construct menu that I have found very useful, e.g., for starting a new sketch on a plane that uses an existing feature as a new origin.

[Fully_Defined]

---

@thatotherfellasbrother wrote:

Yes, I have tried to keep my learning to the recommended contributors. There are many ways to approach a design, and I'm very new myself. I completely understand your interest in learning the right way instead of trying to unlearn bad techniques.

I found this tutorial about the BORN technique from the CADWhisperer very interesting https://www.youtube.com/watch?v=YyQHEKrT8bo. On the other hand, there are several commands under the Construct menu that I have found very useful, e.g., for starting a new sketch on a plane that uses an existing feature as a new origin.

---

I remember seeing that video a few years ago, and it’s a good reference.

A word of advice: if you follow the conventional wisdom dispensed on this forum by the usual suspects, you might develop some bad habits that will be hard to unlearn. You have probably already run into rules 1 & 2, both of which are pointless, unless you really like Russian dolls and constantly renaming things.

[Drewpan]

Hi,

Just remember that the "usual suspects" collectively have hundreds of years of practical real world experience. Also that

many of them have been with Fusion since the beginning and learned things the hard way. That being said, I want to be

a successful engineer so I am looking at learning best practice that works.

Rule #0 says "there are many ways to kill a cat than drowning it in butter". It comes down to learning different

techniques, but also learning when is the right time and the wrong time to use them.

I recently posted about the Born technique and only had a single reply. It is a valid technique, it isn't the only

technique. The two main ways to model are design in place and born modeling. Each have advantages and

disadvantages. I have used both and will continue to do so, I am still learning about exactly when it is and isn't

the best way.

Cheers

Andrew

[laughingcreek]

---

@Drewpan wrote:...The two main ways to model are design in place and born modeling....

---

for the record, these are not mutually exclusive techniques.   The smaller assemblies typical of my current work are all both built "in place" and use born techniques.

[Steve_Worley]

Thank you for your response and all the others that were kind enough to respond. I watched the video on the BORN technique, and it made sense. It also gave me a much better understanding of the CAD Whisperer. Specifically, that he had worked on a drawing board and in manufacturing. I used to work in a job shop when computers were first starting to be used for design/detailing. I always found it a pleasure to work behind someone who was good at drafting on a board. It seemed like everything was well thought out, the views were understandable, and there was enough information to manufacture the part without dimensioning things that didn’t really need to be dimensioned (think assumed constraints). If it looks symmetrical and it’s not dimensioned, we manufacture it symmetrical.

Whenever we would have a new part, the first thing we would look for would be the datum structure and the most convenient place to program from. Hopefully, it was from the datum structure. Even if the print was in car body coordinates (usually centerline of the axel or bumper, or something like that). We would simply pick up the fixture origin with an indicator, then move the origin 100 inches or whatever was necessary. It didn’t matter where the origin was as long as what we were machining was on the table.

I think a lot of my past is bleeding over into the present. My impulse is to move the component origin to wherever it is attached to the mating part and then capture the position. When that component is finished, I do the same for the next component. This means I would have several “capture positions” in my timeline. This doesn’t seem to be a problem, but now I’m concerned about the unintended consequences. I know the capture button is put there for a reason, but is how I’m using it the reason it was added? If I have 20 capture positions in my timeline will it matter? I understand I still need to use joints. But again, should I use these as I build, or build and then add them? Each answered question leads to another.

Are there unintended consequences for having multiple capture positions in your timeline (the larger the assembly the more there would be)?
Are joints best added at the end or as you go, or does it matter. Any unintended consequences with either method?

[TrippyLighting]

---

@Steve_Worley wrote:
... This means I would have several “capture positions” in my timeline. This doesn’t seem to be a problem...

---

Not yet, but it will get there!

The capture position feature captures the position of all components that have been moved  since the last capture position feature in the timeline. As your design grows, the number of components grows and the the amount of data needed to capture the position(s), grows.

That will substantially increase the computational burden on a model. For example the time it takes to re-compute the timeline if you edit a feature will become much longer.

Most mechanical designs should not have a capture position feature. The purpose of the capture position feature is to be able to use different component orientations/locations for modeling. I personally could live completely without the capture position feature and capturing joints in the timeline at all! 

[Steve_Worley]

Thank you! These are the unintended consequences that I was wondering about. If I am understanding this correctly, joints would use less computing power than muliiple capture positions. Thank you for the enightenment. This would only show up after the models got much larger than what they are now (after I had already made it a “habit” of capturing positions).

[davidpbest]

There should be a section called "Requirements for offering help and suggestions in the Forum."

1. Don't lecture, or bully the OP.  You are not here to show off your brilliance. 

2. Assume the OP could be smarter than they appear in their post, or could be smarter than you are.

3. If you want to offer help, take the time to be thorough in your suggestions.  If you just want to complicate the treasure hunt map with "clues", resist the temptation to post a cryptic reply, and let someone else handle the response.  

[Fully_Defined]

---

@davidpbest wrote:

There should be a section called "Requirements for offering help and suggestions in the Forum."

1. Don't lecture, or bully the OP.  You are not here to show off your brilliance. 

2. Assume the OP could be smarter than they appear in their post, or could be smarter than you are.

3. If you want to offer help, take the time to be thorough in your suggestions.  If you just want to complicate the treasure hunt map with "clues", resist the temptation to post a cryptic reply, and let someone else handle the response.  

---

My experience with fora in general has been that the frequency people post suggestions and help has no relationship to their relative breadth of experience or understanding of the topic. Unfortunately, the concentration of relatively few advice-givers does have a direct relationship to the mythological canon of Fusion 360, and it means most English-speaking beginners develop bad habits by trusting random strangers on the internet, right here. If I take Rule #0 at face value, it exists explicitly because of that.

[Steve_Worley]

Thanks to all who have been patient enough to try to answer my questions.

I’m still having trouble learning how to think, so I’ll answer my own post a few months later in the hopes that it will help someone else. The first thing I’d like to say is that the rules listed are good, and the more you use them, the better off you are and the more you understand why you use them. Fully constrained drawings are a must. If I would add a rule, it would be that components are one of your best friends. Grasping how they work is a beautiful thing.

I’ve noticed that most Fusion CAD users come from other CAD backgrounds, so it’s nice to get their overall experience. However, I still have not found anyone from AutoDesk who says, “Fusion was designed to work this way, although it can be used in many other ways.” I’ve been using model steam engines (and a radial aircraft engine model) for my practice of assemblies and joints. This is my best guess at how Fusion was designed to be used, although there are many, many, many, many other ways to accomplish something.

It’s designed for top-down work, and it easily allows you to leverage everything in the assembly you have created for each new component you create. Think in a way that you are designing parts where they go, not designing individual parts and placing them where they go (more on that in a moment).

I was hung up on coordinate systems. Don’t be. You’ve got dimensions. Create your first component. DO NOT USE THE TOP-LEVEL COMPONENT (THE ONE WITH THE FILENAME) TO DESIGN ANYTHING! After you finish with your first component’s design, create your second component. Pick a plane from your first component (or construct one if necessary) and project geometry from the first component to your new sketch plane. Now you can tie all the geometry back to the projected geometry. Once you have your projected geometry, isolate the component you are working on to eliminate the “noise” of all the other components. Unisolate it when you're finished. You’re not moving any coordinate systems, and if the projected geometry changes, so does your sketch. If you don’t want this you can always unlink the projected geometry. This will make your sketch not fully constrained, but all you have to do is use dimensions to tie it back to the origin. Since all the geometry is exactly where it belongs (nothing moves when you break the link) this is a snap. The sketch is now fully constrained and you are ready to move on to the next component.

When you are finished, all of your components will be right where they need to be, with no “capture position” used. The bonus is that you can easily drag and drop components to get them out of the way when you want to look at something more closely and use the revert button to put them back when you're done. At this point, you can use as-built joints for most of the components (quick and easy) and focus on the joints for movement last. 

This appears to work well with small assemblies (10-30 components). Please feel free to blast holes in my logic (nicely). Again, I’m interested in learning how the software was designed to be used. Things went more smoothly this time using the methods above than in previous tries. I am curious if I am on the right track or if something is going to derail me.

[William_Dec_45]

I would respectfully add that forum gurus should check their preacher hat at the door. Sure, the question the poster is asking, all questions for that matter, can be answered by reading the reams of documentation and/or keeping after it for hours until you crack it yourself. Forums provide expediency for those of us who have worked hard but still overlook the obvious. We do stupid things like not establishing a relation ship with the point-of-origin. Simply asking the gurus instead of putting out the effort will certainly be abusive and lazy. But rather than pointing them to the book, let someone else answer the question, someone more tolerant. Otherwise, there's really no need for a forum. I know my face has been reddened many times by coming here, but, contrary to what some gurus might think, I have learned a lot from them and I sincerely appreciate it.

[Fully_Defined]

---

@Steve_Worley wrote:

Please feel free to blast holes in my logic (nicely).

---

I agree with very little of the advice you gave, which if followed would create a tangle of circular and dangling references. Depending on the complexity of the design, that might not matter to you personally.

A far more robust method is to use parameters; have each component draw from the same data rather than relying on projected geometry. You can include some fairly complex equations and logic in parameters, and with the new configurations features it is a no-brainer to leverage smart parameters over dumb projections. It's not ALWAYS possible though, and sometimes projections make more sense or are the only way; it's important to know when to use each tool appropriately.

It's also important to know when a design should be an assembly and when it should just be a collection of bodies with a common origin. Both are possible in Fusion 360, but there is a vocal faction here on the internet (that's the one with email) that thinks 100% of all designs are assemblies, 100% of the time. Ironically, these folks don't tend to give equal weight to joints, which are literally the entire reason to choose an assembly structure over a collection of bodies, when there is a choice.

In other words, it is entirely appropriate to work in the top level of a design without first adding a blank component. I have seen - with my own eyes - MANY beginners start with a blank component inserted into an otherwise blank assembly with the ultimate intention of designing a single body, and then they don't even bother to joint that component to the origin. Facepalm!

I propose a different tack. Rather than reflexively inserting new components into new assemblies, try creating the first part as its own component at its own top level, and then inserting it into a new assembly, taking advantage of the new "ground to parent" feature. It's pretty easy to unlink the component if you change your mind, but working your way backwards through a minefield of projected geometry and interdependent components all living solely inside an assembly is not something I would recommend.

[Steve_Worley]

“A far more robust method is to use parameters; have each component draw from the same data rather than relying on projected geometry”

This makes a lot more sense than projecting everything. For what I had been doing, it was not a problem. However, it sets a bad precedent. In a complex assembly, it would be difficult at best to go back and find every instance to fix things. Using parameters, it's literally “one and done.”  Thank you for your insight.

“It's also important to know when a design should be an assembly and when it should just be a collection of bodies with a common origin.”

I was under the impression that it was always good practice to create assemblies. What I’m hearing you say is why make something more complicated than it has to be. If I heard you correctly, if I don’t need a joint, why would I need an assembly? This might be an obvious point, but I certainly missed it. 

“try creating the first part as its own component at its own top level, and then inserting it into a new assembly, taking advantage of the new "ground to parent" feature.”

I will try this and your other observations. Thank you for taking the time to correct some of my thinking. The laws of unintended consequences can be brutal. It sounds as if you have had a few “facepalm” moments in your career, and I appreciate you letting me (and others) learn from your experience.

[TrippyLighting]

---

@Steve_Worley wrote:

I was under the impression that it was always good practice to create assemblies.

---

What gave you that impression?