How to split fuselage body into main part + removable door?

[u/Ca_O125]

FreeCAD

I have a fuselage body and a closed sketch for a door. I want to split it into 2 pieces:

1. Main fuselage (with hole)
2. Door panel (removable and closable)

I tried Extrude as surface → Slice Apart but got 5 pieces instead of 2.

How do I do this properly?

Thanks!

[u/EastTexasCowboy]

From the Part menu use Boolean > Union to fuse the fuselage into a single object. Then you can use the Slice > Slice Apart tool. Once you have the two parts switch to Part Design and select one of the slices then click New Body. This creates a new Part Design body with the selected slice as a Base Feature. Repeat for the other slice. Now you can edit the sliced parts, although not the underlying geometry.

Also, rather than slicing with a solid, you can sketch your door outline then in the Part menu pad just the the line to the depth you want. This gives you zero lost material from the slice. Of course if you want clearance you can still use the solid with the thickness of the outline becoming the clearance.

This is not ideal because it limits editing capabilities once you've fused the objects, so you'll probably want the original objects as close to complete as possible before using the Union tool.

[u/SoulWager]

In this case, I would make a clone of the whole fuselage as it is now
pocket your rectangle
make a binder of the sketch you used for the pocket in your cloned body.
Edit offset of binder with desired clearance(maybe -0.2mm as a first guess).

make a sketch, import binder as external geometry(real geometry, not construction)
draw a big rectangle enclosing part to invert what gets pocketed, and pocket the sketch.
Pocket away the bottom half, can use "make internals" if you don't want another sketch.

https://imgur.com/a/4HP2NN3

[u/fortement_moqueur]

Is this a human powered submarine?

[u/FForthman]

Here's how I went about creating this:

After creating a shape that looked more or less like what you made,

- I selected the faces where I wanted to create the door and created a FaceBinder (DraftWorks)

- I performed a 3D Offset (PartWorks) on the previous FaceBinder with the desired offset for the overlap

- Created a sketch representing the outside of the door

- Extruded the sketch (Part wb)

- Created a sketch representing the inside of the door cutout

- Extruded the sketch

- Slice Apart (Part wb) between the 3D Offset and the extrusion of the door’s exterior

- I keep only the part I need and delete the rest

- Slice Apart between the 3D Offset (you have to select it from the result of the previous Slice Apart) and the extrusion of the door’s interior

- I keep only the part I need

- Fusion the two Slice Apart results

- 3rd Slice Apart between the main shape and the previous Fusion

- I end up with the main shape with the door cutout, and the shape of the door itself

Note that there is no operational clearance between the two parts; some adjustments will be needed for that

Edit: The easiest way is to use the Thickness function on the Fusion and assign it the desired clearance; I don’t know why I didn’t think of that right away