Hi Hastyark.misc,
1. You can try converting your bodies into components by expanding the Bodies drop-down in the designs workspace's browser (Not in Drawings). Then you can right click on each body you created and then "Create Component from bodies" (I usually give them a name at this point), once the bodies are components, you can select create a drawing and in the dialog un-check full assembly, now you can select your single or multiple components you specifically want.
2. The browser tree will represent all the components that exist in the assembly regardless of selecting a subset of components when creating the drawing. So even on placement of the single component into the drawing, if the assembly has more components then the drawing browser will have all the other components listed in the browser as turned off. One way I can think of to to get your desired behavior would be to: go back into the design work-space, right click on the component you want to make a drawing of, choose Save copy as, and save the component to its own design file. Now if you open the newly saved design, you can create a drawing from just this component, and the Drawing browser will only have that single component listed in it.
It should be noted that if you break your design into multiple components in their own separate files from a parent design file, then changes to these new designs in the parent file will not have any impact on the new files and vice versa. These are basically newly created designs copied from your existing design files.
I think the ideal workflow might have been too create your design by making each component individually or together in one design after save them all out separately. Then create a new empty design and drag in all the existing individual components to form your assembly. This way if you update any existing individual components design any assemblies that include it will automatically update to include design changes, this also gives you the option to create a drawing of each individual component, and you still have the option to create a drawing from the entire assembly design as well.
3. If you want multiple views of the single component with different projection angles you can place your initial base-view, then use the Projected View tool (In toolbar) click onto the existing base view and drag your mouse around to create more views projected from the base view. If you want to include multiple base-views in the drawing, you can just keep using the Base-view tool (in toolbar) and place several new base-views. You can also double-click any existing views and edit them, you can turn on and off hidden lines, Shading and other common view settings. Copy pasting of views is not available in Fusion Drawings. Adding more base views will add more stuff to the drawing browser as well. (This video is a bit outdated but it shows some examples of how to place some drawing views, Base, Projected, Detail etc. https://www.youtube.com/watch?v=jKZBLM0l6lw )
Hope this helps!
Best Regards,
Justin
