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# System prepended metadata

title: 'NOPE001: FreeCAD Shell case with PD Loft + Thickness'

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# NOPE001: FreeCAD Shell case with PD Pad + Thickness

Non-Obvious Practical Examples 001:

Probing the ways to make what would look like a vacuum-formed cover over a template. PartDesign Thickness or bust!
So, mostly bust, and eventually some result in the form of a working block and tackle:

![image](https://hackmd.io/_uploads/S1fvlSv6T.png)

The design is intended to lift up objects while the rope is pulled from above (think well shaft, second level in a building).

To facilitate the setup, a sleeve is shoved over the pulleys, preventing the rope from slipping off. The sleeve in turn is held in place by a carbine.


## Starting Material

FreeCad Version: 0.21.1

Snackblock pulley with 608 bearing (for inspiration and the pulley model): https://www.printables.com/model/613342-snatchblock-prime-pulley-608-bearing

5:1 pulley system, allowing two pulleys to be arranged on opposite sides of a central plate:
![image](https://hackmd.io/_uploads/ryRJXBDpa.png)
(source: https://issuu.com/tlins/docs/pulleysystems)

## Basic idea
- 3 sketches padded symmetrically to different heights
- sketches share a lower edge
- single face selected, PartDesign_Thickness to hollow it out / create outward thickness
- cut hole
- add extra ribbing / geometry to assist 3D printing

![image](https://hackmd.io/_uploads/r1dwErwTa.png)


## Failed Approaches

### Thickness on refined face

![image](https://hackmd.io/_uploads/rJzBBSDa6.png)

### Thickness on unrefined face

Selecting all pieces of the future opening also fails.

![image](https://hackmd.io/_uploads/SJVOBSPT6.png)

Reducing the problem to only one edge and attempting to create thickness based on only one face shows that something is very much not right with what OCC does behind the scenes:

![image](https://hackmd.io/_uploads/ByuaBSwp6.png)

## Best-Effort Solution

Apparently, a step pyramid shape with a simple rectagular starting face and step depth greater than the targeted thickness produces a result:

![image](https://hackmd.io/_uploads/S1c98SDTa.png)

- sketch another rectangle with a horizontal edge a set distance away from center
- pad symmetrically
- boolean subtraction of the overlap

![image](https://hackmd.io/_uploads/BkLKvrDpa.png)


### printability mishaps and fix

![image](https://hackmd.io/_uploads/S1fCPBwaT.png)

- initial idea to print with the wide opening down abolished
- goblet-shaped orientation problematic regarding overhangs when no support is used (slicers currently don't produce nice code for horizontal overhangs)
- fillets remain a big problem:
![image](https://hackmd.io/_uploads/HkiL_rP6T.png)


Final mitigation steps:
- extended dimenions
- chamfers with dissimilar edge lengths
- thickness
- fillets to clean up internal edges
- square base for printing plus some reinforcement and integral support

![image](https://hackmd.io/_uploads/rk0tFBD6T.png)

I would have preferred to pad the stepped features at an obligue angle instead of just adding a chamfer (which then cannot be extended all the way down, because OCC can't handle merging edges for "some reason").

Symmetrical pads with a non-normal direction vector however don't produce a mirrored result, but an oblique prism, which is not useful. One therefore has to model one half, create a mirrored copy and only subsequently apply PD Thickness and the boolean operation to truncate the result back into shape:

![image](https://hackmd.io/_uploads/S1fIuiwpa.png)



