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You probably did not create a drawing but a model in Fusion 360. To assemble such a device you'd use joints.
I did read your question. You can ask yourself now why an Autodesk Expert Elite with almost 30 years of experience in CAD, 3D modeling, engineering and building very complex machinery recommends to use joints.
Of course you can design this stuff in place and don't need to use joints. But just because that can be done yes not mean it is a good idea to do so! In fact, in a design that uses multiple instance of the same components that is an outright terrible idea!
I've looked at the design you linked to.
It looks to me this design was not designed in Fusion 360 but exported from a different application and then imported into Fusion 360.
The timeline is disabled, which is the default for imported geometry.
There are almost no sketches in that design, which is something that does not convert over to Fusion 360 from other applications.
If you do want to design something like this in Fusion 360 you would have to delete the timeline after designing it. Delete all the joints and all the sketches.
Or if you don't use joints you'd have to use the align and point-to-point move command. Again I'd strongly advise aginst not using joints.
That build-in-place top down methodology indeed works fairly nicely in Fusion 360. However, particularly when designing machinery you will need many identical components to build that machine and in CAD software instead of designing that identical piece a second time from scratch, as you know, you'd create an instance of that part. That instance has to be placed somewhere and in Fusion 360 you can do this in mainly two ways.
- You move it into place using either the align function or the point-to-point move tool, but then you'll have to use a position capture feature to capture the position of that part. That has a few distinct disadvantages, e.g. the position capture feature does not show up in the browser..
- Use joints.
There is actually a third way, but I am not sure I'd recommend that either so I'll keep it to myself 😉
No, offense taken!
I've only done this with smaller stuff, but I believe if you export an assembly as a .step file from Solid Works the assembly structure is maintained, but all the application specific information such as sketches, feature tree (roughly comparable to the timeline in Fusion 360) are stripped.
When you import that into Fusion 360 it attempts to recreate the structure and by default for imported geometry the timeline is turned off ( for a good reason!)..
What was previously an instanced object is not an unliked copy and "dumb" geometry.
To interchange Cad data I would strongly advise against the use of. stl files unless there is really no other way. .stl files are triangulate meshes that lack accuracy.
While you can use linked components for an original design there is no need to first create a component in it's own file and insert it. You can create instances of components in a single file without using any external files, by simply copy/pasting a component. The copy will update when the original is updated.
Well ... that also is not easy to answer 😉
It sort of depends what your goal is. If you want to really learn how to use joints you might approach this differently then if you just want to get on with assembling this.
Biut I can tell you how I would do this. Consider that this is an imported assembly and all the components are already in their intended location and orientation. Somewhat similar to a top down design where everything was designed in place.
All stationary components would go into an as build rigid group for stationary components.
The main moving components in the X, Y Z axis would go into rigid groups for that axis.
The few remain components that need to move independent for example the components on the extruder for advancing the filament I would use as-buil;d rigid, revolute etc, joints for.
the key in this assembly is that everything tis already ion place and you cause the as-built joints very effectively.
If this design would be designed from scratch the process would be very different. Say, for example you start with designing the frame Meade from Aluminum profiles. You might create components for the 1st frame profile extrusion, active it, create a sketch for the first profile in the desired assembled location and then extrude it.
Bit that profile is already needed 4 times. You would obviously not want to create that profile 4 times from scratch. You'd copy/paste an instance of it into the design. Fuiosn 360 will allow you to move it to a desired location and the first move when tasing and instance is free in the sense that it does not create a feature in the timeline. Then you would want to usee a joint to assemble that profile into the correct location and orientation.
Have you watched any of the introductory tutorials in the Support and Learning section of the Forum ?
These basic steps are covered there.
Please don't take this as an offense. I obviously don't mind answering your questions, but I don't want to start with Adam and Eve!
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