Finding the parent sketches and features of bodies.
yes, this can be a challenge. It helps if you use components to contain your bodies. Then you can turn on Component Color Swatches, which will indicate which features are owned by which components, because of the colors:
Also, if you use Rule #1: fusion-360-r-u-l-e-1-and-2 , then your sketches will be owned by the component that owns the body. That will help, as well.
And, some features support "edit profile sketch" which will take you from the feature to its sketch:
Jeff Strater
Engineering Director
There are numerous ways to identify those.
Are you familiar with Fusion 360'a R.U.L.E #1 and how to organize your designs into components ?
You can right-click on geometry in the viewport and then select "edit feature" or "edit profile sketch", which convers a a lot of the use cases.
After the right click, further down at the bottom of the pop-up menu you can also select "find in timeline" or "find in Browser".
It depends on the designer, you can remove Capture Design History on any F3D or F3Z (linked assembly) file but I would not recommend this. With an imported file such as a SAT or STEP file, you can have a timeline but it only shows a Direct Model component. Some designers feel that designing without a timeline is easier and creates a more responsive model, I am not one of them.
If you receive a file without a timeline, you can start a timeline from that point on but unfortunately it will not pick up any previous features and operations in the timeline.
The answer to your question is No, just because you import a F3D file it does not turn off the timeline.
John Hackney, Retired
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@larsboelman wrote:
Thanks Jeff, Günther and Peter for the prompt replies. Impressive to get this good feedback this fast.
I am familiar with the functionality mentioned, as well as Rules 1&2. My problem is less with my own models than with the stuff I receive from a colleague who seems to ignore the two fundamental rules and prefers quick 'claying'. My challenge is to engineer something that will work out of a design/styling proposal. I am trying to find his original sketches in the file I received, to figure out his design intent and hopefully reuse some of his geometry. It is frustrating getting nowhere with the 'find in timeline/browser' and 'edit feature/profile sketch' functionality. There's about 80 sketches loaded with projections in a file I am currently using as reference, which contain information that could easily be in less than 10 simple sketches. I was hoping there would be a strategy within Fusion to find the dependencies between the (>95% unconstrained) sketches and features, so it would be easier to find what I need as well as to clean up the mess. Redoing it all so far has proven to be the quicker option than trying to find with the strategies described above.
Thanks for your suggestions! Much appreciated.
This sounds to me that your colleague requires a good amount of coaching and/or mentoring.
Have you had a conversation with your colleague abut the difficulties you are encountering with his work ?
Aside from pure software tools, much can be gained from understanding each others workflows and difficulties.
@davebYYPCU wrote:
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How do you Extrude by vector other than Fusions method of normal to the profile plane?
Sweep will do it, needs you to identify the vector to Fusion.
In other CAD systems you can define alternative coordinate systems often called frames. Then you can pick an axis of that frame when you want to define the direction of the extrusion. The process in Fusion 360 is different, but the end result isn’t.
@larsboelman wrote:
@TrippyLighting The colleague responded when asking about why he didn't just edit one sketch in one of my files, but instead added a full screen of direct modelling actions to the timeline, that he wasn't aware of this possibility. I suppose this also has to do with my initial question: it is unclear (at least to me) how to access the hierarchy/relationship between the features is in the current interface. Even doing a 'replay' of the timeline will not clarify this; merely an understanding of what was done when but not how to quickly find which sketch is used where and which feature is the parent or child of another feature. The suggestions and explanations from yourself and others have made the options for improving this more clear, but the current interface is still lacking in my opinion.
Unfortunately I can not share the file due to confidentiality of the project.
The browser shows objects that are created by features in the timeline in the sequence it they were created.
A sketch, for example appears as an item in the bowser, but also as a feature in the timeline. To edit a sketch you can select it in the bowser or timeline, right-click on it and select "edit Sketch" from the pop-up menu.
When visible in the viewport, you can also select a sketch object, right-click and select edit sketch.
You can also select a face from 3D geometry in the viewport and right-click and select "Edit feature". That will allow you to conduct changes very quickly, without having to track down those features in the timeline.
If a feature was created by a sketch, after selecting it in the view port you can also right-click and select "edit profile sketch"
The first paragraph in Fusion 360 R.U.L.E #1 & #2 outlines a more component centric approach and outlines some benefits of it. This includes component activation to filter the timeline for items that only belong to that component etc.
Naming "stuff" is one of the most overlooked aspects of proper design organization. I don't name everything, but if I find myself going back to a sketch more than 2 times I'll give it a descriptive name. I'll definitely name components and sometimes bodies.
That, however only addresses direct "connections". If you project an edge form a body or an object form another sketch into a new sketch, later it is difficult to see what the originating sketch was. As designs get more complex it can get very difficult to untangle these connections.
A feature I have asked for many times is a dependency graph that helps to visualize dependencies, but I don't see that happening any time soon.
Having said that, this is clearly a feature for advanced users. From your comments it is clear to me that both, you and your colleague need more seat time with Fusion 360. If you colleague did not know how to find, or even edit existing sketches and what the effects of that would be, then my first action would be to try to bring him up to your level.
