Trying to split a body but...

[Anonymous]

Hi Fusioners!

I am trying to cut this body along the zig-zag line. The line runs over different faces and I am uncapable of getting Fusion 360 to cut the whole thing making two halves through the line.

Please give it a look  🙂

[Anonymous]

@Anonymous

You may do that by these steps :

draw continuous sketch and extrude it in ( patch ) and create two component one for extruded sketch and the other for body after that split it (split body ), I attach a screenshot as  simple example 

[etfrench]

There are several reasons why this is failing for you:

1. Lines and splines are located in several different sketches.  They must be in one sketch.
2. There are overlapping lines and splines.

Here are the steps I did to correct the problems:

1. Move the main body to a component.  This should actually be the first thing you do when creating a new model.  See Rule #1.
2. Create a new offset plane that is outside the body.  This isn't necessary, but it makes it easier to see what you're working on.
3. Create a new sketch on the plane.
4. Project the zig-zag line geometry from multiple sketches to the new sketch.
5. Break the links on the new geometry.
6. Draw a connecting line between the left and right sides.
7. Delete the left side geometry as I wasn't able to correct the overlapping spline.
8. Trim overlapping geometry on the right side.
9. Delete line segments which are continuations of other lines.
10. Extend those other lines to meet their neighbors. Test whether or not you can select the entire right side geometry as a splitting tool. 
11. Once you can select the entire right side geometry, mirror it to the left side.
12. At this point you should be able to split the body.

Notes:

You're using way too many sketches.  You also have symmetrical geometry which can be created easier using the Mirror tool.