Complex Angle Faces: How to dimension in drawing?

[tonySWCR2]

Hello All, 

Attached is a simple sheet metal part that has non-perpendicular bends. This causes the face to be angled in all three main planes. In the example there are 2 holes on this face. How do I dimension them in a F360 drawing? I know how I would do it in other packages but Im lacking tools in F360. Can it be done?

Lets ignore that its sheet metal and you could flat pattern it, imagine its a solid part so making a flat component view isn't an option. 

Cheers, 

Tony

[jhackney1972 · Accepted solution]

It starts with a Named View in the model and then you create a modified Section View in the drawing.  I created a blog article and video on this process which you can view here.  I am sharing the drawing as a public link.  I have never done this before so I do not know how it will work.  You may have to use direct dimensioning instead of the dynamic dimensions for example I used the Diameter dimension command on the hole diameter instead of the dynamic dimension tool.  You will not get automated centerlines to work either, you could sketch they yourself.

Edit:   Look down further is forum question for a point that @laughingcreek made about how I went a little too far with my methods.  I got so involved thinking this was a great opportunity to show my method of Auxiliary Views I lost sight of the simple method of doing this.  Sorry, I hope you will take a look at my Blog article anyway.

[laughingcreek · Accepted solution]

@jhackney1972 -why the section view?  if you "look at" that face and name a view in the model, using that in the drawing produces a view that you can use center marks on, and avoids having to create a section view.

[jhackney1972]

Good Point!  I got so wrapped up in the fact that this was an example of the method I used in my blog article on Auxiliary Views I guess I missed the obvious.  I can't see the forest for the trees!  I will edit my post, thanks.

[tonySWCR2]

~deleted~

[tonySWCR2]

I had kind of half muddled my way to the point of using section views as aux views but its so hard to get them to line up. Found a video you made on youtube which helped, using the green boxes and dragging across the dotted line to keep the view parallel. Where I was going wrong (by which I mean, where fusion fails me) was trying to use the smart dim tool, I just tried with the linear dimension tool and it works! Unfortunately, still no centre marks. 

Cheers for you help.

[jhackney1972]

As @laughingcreek pointed out, using a Named View takes care of everything, including the Center Marks.

[chrisplyler]

Unless there is some reason that this isn't acceptable...I would just dimension them on the Flat Pattern view.

[tonySWCR2]

So it does. 

My real life problem has the face obscured by another feature in the component so I had to use your method, therefor loosing the CM's. 

[tonySWCR2]

@chrisplyler there is always one

"Lets ignore that its sheet metal and you could flat pattern it, imagine its a solid part so making a flat component view isn't an option. "

[laughingcreek]

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@tonySWCR2 wrote:

...My real life problem has the face obscured by another feature in the component so I had to use your method, therefor loosing the CM's. 

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if you start looking straight on b/c you used a named view, the cross-section is much easier to draw.  you can have your obscured view and also have your center marks-

[chrisplyler]

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@tonySWCR2 wrote:

@chrisplyler there is always one

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Sometimes I am the one. It happens.