Fusion 360 - Create drawing of angled assembly component

[ericw.wise]

I'm new Fusion 360 and have thoroughly enjoying and quickly productive. However, I have been banging my head against my keyboard for a while now with what I think should be a simple drawing option. I have created an simple assembly to interface between a 4 wheeler frame and pintle hitch. The assembly consists of two flat panels and four pieces of angles with inserts (it all bolts together). The flat panel for the pintle hitch is aligned with the default X-Y-Z axises while the flat panel to interface with the 4 wheeler is angled at 39 degrees. I created the 4 wheeler flat panel aligned with the default axises and then rotated it in the assembly. Creating the drawing of the pintle hitch panel is quick, easy, and intuitive. However, when I create the drawing for the 4 wheeler panel (which is rotate in the assembly) I cannot get a normal (perpendicular) view of the panel - all of the views have are rotated 39 degrees. This makes the drawing peculiar and complicated (and the dimensioning ugly and confusing). 

Here is the question - When a component is angled away from the default axises in an assembly is there some way to align the drawing plane (NOT sketch plane) with the component so the drawing views are normal (perpendicular) to the component ?

Thanks for any help!

[HughesTooling]

It sounds like you rotated the body, if you rotate the component it's origin rotates with it and when you create the drawing by selecting just that component it should be aligned.

If you actually create a body that is not aligned with the origin there is a workaround. You need to select a face on the body, click Look At then create a custom view. Then when you create the drawing select the custom view as the base view.

Mark

Edit, It looks like my first sentence doesn't work, I'm sure I've used that technique before though so I don't know if somethings changed. I'll have to look through some of my drawings to see if I can find one that used to work.

[HughesTooling]

Edit Didn't work how I thought so removed.

Mark

[ericw.wise · Accepted solution]

Thanks for the responses - the custom view didn't work, but it sent me down a path which did. I exported the component from the assembly (into it's own file) and rotated the base feature so it was aligned with the default axises. Then I imported the component (back) into the assembly, placed it (rotating it), and now the drawings work. So I learned how to model better (more in line with Fusion 360's requirements). It worked, thanks!

[Anonymous]

Hello, I have a similar problem when I make a assembly then make a multiple drawing from it, parts that are at a angle have views that are not perpendicular. I intended to use every part of the assembly in separate sheets hiding the others, is this the wrong way to do a technical drawing of all parts of an assembly. Or must I do something in the design before so parts are all in one multiple sheet and have the correct view?

[HughesTooling]

You have to create custom views for each component. Use Look At to align a face then create a Custom view, if the XY don't align create a Joint Origin on an edge with the correct alignment then use Look At and select the joint origin. Here's an example of a joint origin aligned with an edge and selected with Look At. Fusion really needs some tools for creating and maintaining views of components.

[Anonymous]

Thank you! 😉

[Doubletop_]

Creating custom views and then using the view to align the object correctly on the drawing works fine. Until you move a component by (say) testing motion in the assembly. Then modify any in the of the components in the assembly and update the drawing. The moved components take up their new orientation and you are back to having update the views and replace the components on the drawing.

There must be some trick buried in Fusion 360 somewhere, but I can't find it.

Any clues please?

[HughesTooling]

You can update the Named View in the design to match the new orientation. Just select the face, Look At then update.

[tedbradley314]

For those who (like me) didn't know what the "Look At" tool/feature is... works great.

https://forums.autodesk.com/t5/fusion-360-design-validate/how-do-you-look-at-sketch-face/m-p/5508032...

[legendary_marc]

this work like a charm thanks !!!