Component orientation in a drawing

[lemelman]

I confess that I find the 2D  drawing part of F360 to be totally non-intuitive.

I'm creating a model comprised of a number of components - all created in their own co-ordinate systems.

I've used joints to assemble them as shown in the screenshot, and want to create 2D drawings of them. The first one I've chosen illustrates my problem. It's orientation is determined by the recesses in the main block as shown, but when I switch to the drawing environment it is displayed at the orientation in the model. I want to display and dimension it in it's own co-ordinate system - so it can be machined as normal. But I can't find a way to orient it.

What am I missing please?

[jameshorne0503]

Hi!

So I don't think this is the most efficient solution but you could use custom Named Views. These can be used in base views then you can project from there.

It'd be nice if the Fusion360 had custom drawing orientations like Inventor so this could be done directly in the drawing, no in the model.

Hope this helps!

[lemelman]

Thanks James,

Your suggestion looked promising - I defined a named view in the model but cannot find a way to choose that named view in the drawing. The only views available are the normal ones: base, projected etc.

What am I missing?

[jameshorne0503 · Accepted solution]

Make sure you’ve saved the model and it should come up as an option when choosing a base view.

Edit: Like so

 Hope this helps!

[lemelman]

Thanks James,

That did the job.

I'm really far from impressed with the F360 drawing environment. It is, by far, the worst bit of an amazingly good product.

A great deal of effort has clearly gone into the rest of the product but 2D drawing still presents very much as an afterthought. It should be possible to separately insert multiple individual components, each with specified named views, into any part of a drawing sheet.

[jameshorne0503]

I also find the drawing options in F360 somewhat lacking (especially compared to a pure CAD package like Inventor) but fortunately the roadmap for fusion does include significant drawing improvements.

Another workflow that might work for you would be modelling each part individually then inserting them into an assembly file. You could then reference the part file in your drawing. It makes your folders a bit messier but could save some time compared to making a bunch of names views.

[lemelman]

This is a composite picture of a typical sub-assembly in my model, and illustrates my problem. It contains  4 separate components and my model has 6 of them.  They are all rather small and it seems ridiculous to have to assign a single drawing sheet to each, especially when, if they were all on the same sheet, it would be easier to show how they fitted together.

2D drawings should impart information, not obfuscate it, and separate sheets will do just that.

[laughingcreek]

agreed, drawings workspace is lacking.

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@lemelman wrote:

...it seems ridiculous to have to assign a single drawing sheet to each...

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Don't understand that statement.  You can put as many separate components on a single sheet as you wish.

[lemelman]

In the case that I illustrated, how do I put each of those 4 components on the same sheet, each with it's own projections and dimensions? I've not managed to do it.

[HughesTooling]

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@lemelman wrote:

In the case that I illustrated, how do I put each of those 4 components on the same sheet, each with it's own projections and dimensions? I've not managed to do it.

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For it to work reliably have the design and the 2d drawing open. In the design right click the component you want to add and from the menu select Create Drawing. On the dialog you should have the options to add to the existing drawing and any sheets.

Mark

[laughingcreek]

for each "base view" you add to a sheet, you can control what objects are visible for that base view from the browser.

[lemelman]

I tried your method Mark, with mixed success.  I chose to add one of the components that was already in the 2D drawing.

Attempt1. I selected the component, chose Create drawing, selected sheet1 of the existing drawing, and pressed enter. The component appeared in the drawing, but not oriented as per the named view.

Attemp2. Went through the same steps but, although the component was already displayed via the named view, chose the named view again, then  selected sheet1 of the existing drawing as before, but Fusion fell over with a message requesting more details of what I'd done.

Attempt3. Restarted Fusion, opened the design, chose the named view, opened the drawing, repeated Attemp1 and got he same result.

Attempt4. Repeated Attemp2. Fusion fell over with no error message or request for more information. It just disappeared.

I then wrote this reply.

[andrew.de.leon]

Hi @lemelman,

@HughesTooling‘s workflow is definitely one option but it requires you to go back and forth between the model and drawing. The workflow I typically use after creating a drawing is, create another base view. The new base view will default to the entire assembly, but once you’ve placed it in the same sheet as your existing views, select the component(s) you want the new base view to show with the browser, right-mouse click and select Suppress All Except Selected. This will suppress all components except the select component(s); the same result as @HughesTooling’s workflow with the back and forth. You can then repeat this as many times as you need within the same sheet.

See Olivia’s tip from a few weeks back for more details - https://forums.autodesk.com/t5/fusion-360-design-validate/drawings-tip-of-the-week-2-suppress-all-ex... 

Regarding named views, since named views are stored within the model; your assembly in this case, its available for use by all components in the assembly. Just make sure to select the named view with the DRAWING VIEW dialog as @jameshorne0503 suggested. BTW, you can edit an existing base view and change its orientation if needed.

Hope this helps, and let me know if your still having problems with it.

Cheers, Andrew

[HughesTooling]

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@lemelman wrote:

I tried your method Mark, with mixed success.  I chose to add one of the components that was already in the 2D drawing.

Attempt1. I selected the component, chose Create drawing, selected sheet1 of the existing drawing, and pressed enter. The component appeared in the drawing, but not oriented as per the named view.

@lemelman  At this point did you try double clicking the view and change the orientation to the named view?

Mark

[lemelman]

No, I haven't tried that. I've been doing the 'long' way, but then hit another problem which took a couple of days to resolve - if interested see this thread for more details.

[othiele_kh-berlin]

Hi James! I stumbled over this thread about to post the same problem. I have gotten this far but when I use named views in drawings I get a message that I cannot dimension isometric projected views which would make it useless.
In general, I think it would be a much better solution if one could opt between the component origin or the assembly origin when setting the base view.

[HughesTooling]

@othiele_kh-berlin Not sure why you're unable to dimension a custom view in your drawings. I just made up a sample file with a rotated component, created an aligned view. Then create a 2d drawing and selected the custom view for the orientation and all the dimensions tool work fine.

The small views bottom right are the document orientation and the larger views with dimensions are using the custom view. As you can see I can create a PCD from the holes and even a hole callout for the threads. The smart dimension tool as well as the simple dimension tools all work as expected. 

Don't know what's different about what you're doing. Can you export and share the design as an f3d file?