Use component name as drawing title and file name

[Murdug]

I have an assembly with multiple components, each named. I select a component, RC, "Create Drawing", and leave the "full assembly" checkbox un-selected. But the title block "Title" uses the assembly name instead of the component name? How do I get Fusion to grab the component names without manually renaming every component drawing I create?

The same question arises when saving the component drawing. The default name is the top assembly name instead of the component name?

MRD 

[mike.tessier]

Hi @Murdug,

Thanks for posting!

The reason that the title block "Title" uses the assemblies name is because that is where the component was designed (I suspect) and therefore does not have it's own "Title" characteristic associated with it (i.e. Fusion 360 just sees it as some geometry associated with the full assembly design).

To get around this, instead of selecting "Create Drawing" when you right click the component instead select "Save Copy as". This will create a new design that appears in your project of just that one component. Once the design appears in your data panel, you can create a drawing of it by clicking the workspace changer in the upper left corner of Fusion 360 and selecting "Drawing>From Design".

I hope this helps! Please let me know if that resolves the issue or if you have any questions or concerns. I look forward to hearing back from you!

Cheers,

[Murdug]

Hi Mike,

Thanks for the suggestion. It is a useful work-around, because it also solves my component orientation issues I have in the current assembly, as I can re-align the "saved-as" component with no detriment to the assembly ... However ... I lose the link to my design. So changes to my "skeleton" sketch in the assembly does not translate to the stand-alone component. Unless I'm missing some useful trick of maintaining the link to the original parent assembly?

***

And now that I've mentioned my orientation problem, let me expand a little further:

I have a bunch of components with some joints enabling a pivot action...

I activate/isolate the green component, and of course it sits at an angle to the global coordinates. I intend to create a drawing of this component, but of course not at this angle, so I use the align tool to align it to the coordinate system (I tried local and global).

On reactivating the parent assy, the green arm now assumes its new orientation ... which is not what I want. I want it locally aligned with the coordinate system, but globally to adhere to its joints. But it's not.

The revolve joint is misaligned as well.

What am I missing here?

How do I align components for creating drawings without using the manual method of move/rotate in the drawing which I find rather useless. Every time I animate the assembly the drawings go wack.

Any tips?

MRD 

[Murdug]

Oh, and of course even if you do return your assembly to the same orientation, all your drawings will tell you that they need to be updated even though none of the components actually changed. It gets quite tedious and the version number keeps climbing unnecessarily.

[WyzeOwl]

Murdug, we seem to be in the same boat. I posted this very question not 1 hour before you. I also have a problem with parts modeled in the orientation that suits the function but will not orient on a drawing so that a general machinist can use. I sure hope that the Fusion Team looks at this problem soon as I am developing a massive assembly with many non-aligned parts. My issue is explained here https://forums.autodesk.com/t5/design-validate-document/dwg-part-alignments/td-p/6958021

[Murdug]

Hi sextant08,

I'll have a look. I'm glad you posted because mine is hidden under my initial topic relating to the naming schemes. This issue really limits Fusion's usability to me currently, so I hope I'm missing some trick somewhere.

MRD

[HughesTooling]

You can use named views to setup the base view in a drawing, it will not update if you move the component though. Just use Look At to set your view then create a named view.

Mark

[mike.tessier]

Hi @Murdug,

Thanks for getting back to me and sorry for the delay in response!

Regarding the "Save as" workflow not maintaining the link to the parent design, there is a little trick here to prevent that from happening. Once you have saved the component out as it's own separate design, you are going to want to delete the component (and any joints associated with it) from the assembly design. Once it has been deleted, you should re-insert the component into the assembly and redo all of the joints. This will create an externally referenced (XRef) component within the assembly. 

Then, should any changes need to be made, you can make those changes in the design which contains only that component and force those changes out to any designs that contain that component (you will be warned the next time you open the assembly that some components are out of date and need to be updated).

I just took a peek at the other forum post mentioned here, and it looks like @HughesTooling, gave you a great work around for the issue where you were unable to get components in the desired orientation for the drawing. - Nice catch Mark!

I hope this helps! Please let me know if you have any questions or concerns.

Cheers,

[Murdug]

Hi Mike,

Thanks for the idea. Not a bad option, and at least you can align the external component as you please to facilitate drawings, and your drawing remains unaffected when animating mechanisms.

Still not a final solution for me though, because you lose your design references (eg. CREO's copy/publish geometry or Inventor's Derived part) to that component. Any changes in the assembly design (eg. a skeleton sketch from which you created the initial bodies) does not transfer to the external component. 

I still figure Fusion needs to enable the orientation of an isolated component relative to it's own coordinate system without altering its global orientation, and if creating a drawing of that component alone, it should follow the local orientation. Pretty much as standard parts in the other CAD systems function. I know Fusion is not trying to emulate "other CAD" systems, but this to me seems to be a severe shortcoming.

Any idea if something of this nature has made its way onto the idea station? I'll have a look, but I don't want to create duplicates.

Thanks,

MRD 

[mike.tessier]

Hi @Murdug,

Thanks for the reply and sorry for the delay in response!

I had a look through the IdeaStation, but I wasn't able to find anything. Although, I wasn't too sure what keywords to use to describe this workflow. You may have some better luck with searching than I had. However, if you can't find a similar post, feel free to create a new one, and if it does in fact duplicate another request, we'll move it around to make sure that it gets looked at.

I hope this helps! Please let me know if you have any questions or concerns.

Cheers,

[adam_nNQEXW]

Hi,

I'm from the future where there has seemingly been no progress on dealing with this issue. I'm coming from Solidworks to Fusion, where I was lead to believe that top-down (master part, etc) modeling was finally built into the way the program works.

If I have to export each part into it's own file, then re-import into an assembly to make the drawings label properly, then why bother even using top down design?