It is not possible to dimension all views in drawing

[bas1l]

I have constructed a truss and am now trying to create drawings of the struts. Unfortunately I can only dimension one view at a time and it is not possible with the other views. I have tried with a "named view" but without success.

At first I thought the problem was the sketch. But it is clean and rectangular. Then I tried a workaround by moving the strut to the origin. This would work but it is not practical.

I have created a simplified model which shows exactly the same effect. Maybe someone can find a practical way to create a drawing of this part.

[TimelesslyTiredYouth]

Hello again, @bas1l 

In my opinion, the best way to handle this in Fusion 360 is to create a derived component of the strut and temporarily move it to the origin or align it with a primary plane. This way, you can generate a clean drawing with all the necessary views properly aligned without messing up the original assembly. Once you’ve got your dimensions sorted, you can just delete or hide the derived component. It’s simple and doesn’t impact your main design.

Just an opinion...

kind regards

Ricky

[bas1l]

Thanks for the quick reply and the suggestion. I have tested it and yes, it would be a possibility and so far also the cleanest one. however, I don't think it is perfect yet. Ideal would be if there would be the possibility to give each component a clearly defined view or something like another origin where the drawing refers to it.

[TimelesslyTiredYouth]

Hi @bas1l (perfectionist)

So with the "named view" what do you mean it didn't work, some context would be nice with a scrrenshot or vid pls
Since "Named View" didn’t work, you could try using "Joints" or "As-built Joints" to fix the component in a specific orientation for your drawing. By creating a new component or isolating the strut and applying a joint to set its position, you can generate the drawing from that fixed view, allowing for better control over the dimensions without affecting the original assembly. This method can help you achieve the desired results without needing to move parts around manually.

just an opinion that will most likely go very wrong...

contemplating Regards

Ricky

[TimelesslyTiredYouth]

I just realised you said another origin, sorry, do you understand the concept of making new planes and axis's, e.g midplanes ect...

just something that came to mind when you said another origin as you can sort of make another one, if you put in the time and effort to make copies and move them to where you'd like it to be. If this is something you think is to your liking just give a shout and I'll upload a short vid

Apolagetic Regards

Ricky🤣

[bas1l]

Thanks for your tips. Attached a video. Sorry i'm doing this for the first time 😉 Ss you can see it works with Named Views only for one view. For the other views I can't select the lines and when I wait over the line this message comes up.

This is just an example part I posted but with the real ones it behaves exactly the same. If I insert the component into another component and move it to the origin via joints or drive it works. But this is an extra step i would like to avoid.

[TimelesslyTiredYouth]

Hi @bas1l (warning ignorer)
1. - congrats for just ranking to 5 

2. - 

The message you're seeing, "Cannot project objects in isometric projected view. Select objects in orthogonal drawing view only," typically occurs when you're trying to project an object or dimension in an isometric view in Fusion 360. Isometric views aren't standard orthogonal views, so projection tools don’t work the same way.

To resolve this, switch to a standard orthogonal view (like front, top, or side) in your drawing, and then try the projection again. Projection works best with these views because they align with the component’s axes, unlike isometric views that are angled. Once you've projected the objects in the orthogonal view, you can adjust them as needed for your isometric or other angled views.
I'm going to test this now as I can't keep giving theoretical views, as I'm out of them so I'll try some trial and error

Kind regards

Ricky

[laughingcreek]

This is clearly a bug. I'm able to reproduce it on a clean design.  when the view isn't lined up with an ortho plane, drawings seems to think you're in an iso view.  @Phil.E , see vid posted above (I'd point you to the specific post number, but this new forum layout doesn't have post numbers)

[TimelesslyTiredYouth]

Sorry for my asking questions, but how do you realise and identify that there are bugs? When I can't do something, I usually just think it's my incompetence and find a workaround.

kind regards

Ricky

[Phil.E]

Thanks for tagging me.  I logged FUS-183761 as a priority bug, the customer is essentially blocked here.

• Named views fail
• Automatic drawings fail

This is the best I could manage using automatic drawings.

However, there is a workaround for this particular part.

Align the body with the origin.

This shouldn't break the assembly as long as the part is jointed to the assembly. Every design is different, so I don't imagine this would help in every case. 

[Phil.E]

What makes this a bug is the tool (Fusion commands) are not performing consistently. In this case, the automatic drawing method and the named view method should produce a usable drawing view but do not. The error message is for a completely different situation. In software development speak, this is a "case that wasn't handled". Thousands of other cases work just fine (which is why you can produce drawings at all). This one instance needs to be investigated and sorted as to why the results are inconsistent, i.e. buggy.

[bas1l]

Thank you all for the feedback and tips. I am glad to know that it is a bug so I can deal with it and will probably build the model differently to be able to create clean drawings. I am interested to see if and how a solution will be found.

To give some knowledge about the use case. We are building a truss and have constructed the truss top down. That means without external components. So all components refer to the origin of the first component. Since it is a truss and is arranged at an angle in space, it comes to this atypical arrangement of the individual part. The solution will probably be that we build all individual components as external components and create the assembly from them so that we have clean drawings and models.

[Phil.E]

Fusion has Edit In Place for external components, and now a preference for new components to be external by default, so you might find an entirely "external" workflow for components will look and feel a lot like your current top down workflow.

More about edit in place https://help.autodesk.com/view/fusion360/ENU/?guid=ASM-EDIT-IN-PLACE

Let me know if you have questions, glad to help. I also teach Fusion and Inventor so my perspective crosses all worlds here. (top down vs bottom up assemblies)