How to create windows into a non-square surface

[controll21]

Here is a model that I am re-creating from drawings and need to understand how to model the window openings in the nose of the submarine.  I have tried the techniques described on the net for mapping sketches and solids onto the cylinder but non apply to creating these openings onto the slanted surface of the object that is created for the nose.  Help is appreciated.  I have been at this for several days and no luck.  See the image for ideas.Left Side View

Left 3/4 View

Head on View

Top View

Full Model

Windows

[TrippyLighting]

Can you share your model (public link to it from the data panel ) ?

[etfrench]

This thread may help.

[controll21]

How do you create the lines for this type of action in the image...this would work great!

https://forums.autodesk.com/t5/fusion-360-design-validate/creating-square-panels-on-a-dome-surface-r...

Thanks,  Rick

[controll21]

I successfully got the sketches onto the surface with your suggested links help...now I need to figure out how to keep the lines straight instead of how they turned out in the picture...also, I cannot push-pull the red areas after finishing the projection steps....lost again.  Thanks

See images for details

[Johnc911]

Use that sketch you make and extrude surfaces back thru the submarine. Then split the submarine hull with the surfaces. 

[Johnc911]

[etfrench]

Try creating your sketch on the bottom instead of the side.  This image using @laughingcreek's file shows how to he was able to keep the sides straight when using the split face command.

[controll21]

I will try this.  Thanks for the help.

[controll21]

This final area of this model/design messed with my head, and thanks to all the suggestions on here and some thinking on my part, I came up with the solution that eventually worked....thanks to all.

The steps to the success are as follows

1.)     Copied the nose cone as a separate body

2.)     Created a offset plane at the rear section of the nose cone (to act as the pivot area for the following steps)

3.)     Created bodies at the pivot plane to act as cutters into the nose (see pictures)

4.)     Eyeballed the degree of angle to achieve the windows I envisioned

5.)     Cut the nose cone at the top and bottom to achieve the desired window height

6.)     Scaled the angled body cutters so as the whole height of the nose cone would be encompassed

7.)     Removed the non-essential bodies that would not be windows

8.)    Cut the nose cone with the remaining window bodies

9.)    Removed the original nose cone and replaced it with the cut nose cone

10.)   Enjoyed the fruits of your and my labors, Thanks to all!Created bodies around nose coneCut top and bottom of nose cone to size of desired windowsScaled bodies larger than height of nose coneCut nose cone with bodiesAfter cutRemoved unwanted bodiesCut nose cone with window bodies and placed nose cone back in place

[etfrench]

Looks good.  You could simplify your workflow a bit by using a sketch with a continuous line (zigzag) as the splitting tool instead of creating individual bodies.

[controll21]

Thanks,  I have spent around a week designing this (copying it really) and am happy with the results....now since I made the model in Fusion 360 actual size, I need to figure out how to scale it down to manageable within Simplify 3D for printing....I can scale it within the S3D program but would like a model scaled in Fusion for others who might want to print it.  Any ideas?

[etfrench]

Scale command?  (Make a new copy first)

[controll21]

I tried this scaling in Fusion 360 but because of all the parts I used the select rectangle only gets the parts that are surface ones the internal parts are not copied....I will try selecting all along the body list and scale that way to see if it works...thanks.

[etfrench]

Window select the entire model, then verify in the Browser.  You'll need to expand each component and add any unselected bodies and sketches to the selected list.