Fusion 360 2.0.3803 Drawing Views

[Anonymous]

I am currently experiencing difficulty in trying to place a drawing view of a component in an assembly that is not aligned with any of the origin planes within the document.

This results in me being unable to place a logically orientated drawing view and therefore unable to correctly dimension.  I cannot simply re-orientate the component in the assembly or the assembly will be broken.

[ryan.bales]

I would:

1. use the Look At feature to select say the top face.
2. Then create a new Named View under named views in the Browser.
3. Save your model
4. Then in your drawing you can create a new Base View that uses that named view.

[Anonymous]

Hi Ryan,

In a way this does work for me, thank you.  However, when I use the look at button, it only makes the view flat and doesn't 'square' the view up.  I then have to use the rotate tool in the drawing to square the view.

Would you say this is the correct workflow?

Thanks,

Matt

[ryan.bales]

I'm not sure what you mean.

Look At squares the view to the face. Then named view creates a view of exactly what is on screen.

The only other way i'd do that is by setting the current view as via right clicking on the Cube after using Look At.

This applies to the whole model and will make other views skew as a result. The first option circumvents that by only creating a view of a specific object or set of objects based on where the camera or view was at that time.

[ryan.bales · Accepted solution]

Oh i just got what you meant.

Yeah i would use look at, then set as front then create a named view and then reset the front. You may still have to rotate using constrained orbit to get it aligned.

[ryan.bales]

Also, if you do create the view and its angled, orbit within the drawing allows for a reference angle. So drawing a line along the angled side will use that as the 0 degree reference and it should rotate around to be square.