---
jupyter:
  description: 'Pad and Pocket in planex2d: thin wrappers around the OpenCASCADE extrusion that turn a face or a sketch
    into a solid or cut it into one, with the names of the profile on the faces of the solid.'
---

# Pad and Pocket

`px.Pad(profile, length)` extrudes a planar face, shape or sketch into an OpenCASCADE solid, and
`px.Pocket(target, profile, length)` cuts that extrusion out of a solid. Both are thin wrappers around the
OpenCASCADE extrusion, `ToOCCShape().Extrude(...)`, that take care of what is otherwise written by hand:

- the direction along the plane's normal, or against it for a pocket;
- a length on both sides of the plane;
- an end on a plane or a face instead of a length;
- the names: every side face of the solid carries the name of the profile edge it comes from, so the faces can be
  selected by name for meshing and boundary conditions.

```python
import math
import netgen.occ as occ
from ngsolve_webgpu.jupyter import Draw
import planex as px
```

```python nbsphinx="hidden"
from docs_figures import Row
```

## A clamp plate

The example is a clamp plate of 80 × 50, 12 thick, with corners rounded to a radius of 6 and four bolt holes of 6.6
on a 64 × 34 rectangle (Figure 1). The outline and the holes are one sketch, with the outline named `side` and the
holes `bolt hole`. The holes are circles, which have no vertices, so `Fillet(plate.vertices, 6)` rounds exactly the
four corners of the outline.

```python
thickness = 12.0
sketch = px.QuickSketch().RectangleC(80, 50, name="side")
for x in (-32, 32):
    for y in (-17, 17):
        sketch.Circle(x, y, 3.3, name="bolt hole")
plate = sketch.Face()
plate.Fillet(plate.vertices, 6)
plate.name = "plate"
```

```python nbsphinx="hide-input"
Row((plate, "The profile of the clamp plate"), caption="A planex2d face with rounded corners and four bolt holes")
```

`px.Pad` makes the solid. Its side faces carry the names of the edges they come from, the solid carries the name of
the face, and the two end faces have no name. The volume is the area of the profile times the thickness:

```python
solid = px.Pad(plate, thickness)
print(solid.name, sorted({f.name for f in solid.faces if f.name}))
print("volume", solid.mass, "area × thickness", plate.mass * thickness)
```

The same solid comes from the OpenCASCADE extrusion of the exported face, and the difference between both is empty:

```python
by_hand = plate.ToOCCShape().Extrude(thickness)
print("OpenCASCADE extrusion", by_hand.mass, "difference", (solid - by_hand).mass)
```

## Pockets from a sketch on the top face

The counterbores for M6 socket head screws, 11 wide and 6.5 deep, are sketched on the top face of the solid and
cut with `px.Pocket`. A pocket runs against the normal of the sketch's plane by default, into the material.
`px.QuickSketch(top)` sketches on the top face, with the global origin and x axis projected onto it, so the
coordinates in the sketch are those of the plate (Figure 2). See [The plane in 3D](plane.md) for choosing another
origin or axis.

```python
top = solid.faces.Max(occ.Z)
counterbores = px.QuickSketch(top)
for x in (-32, 32):
    for y in (-17, 17):
        counterbores.Circle(x, y, 5.5, name="counterbore")
clamp = px.Pocket(solid, counterbores, 6.5)
Draw(clamp, euler_angles=[-40, 0, 30])
```

With `until=px.last`, a pocket runs through the whole part, to the last flat face it crosses. The clamping slot,
40 long and 8 wide, is cut through the middle of the plate that way, from the same top face:

```python
slot = px.QuickSketch(top)
slot.Move((-20, 0)).Slot(40, 8, name="slot")
clamp = px.Pocket(clamp, slot, until=px.last)
Draw(clamp, euler_angles=[-40, 0, 30])
```

The volume is the plate minus four counterbore rings, 6.5 deep, and the slot through the full thickness:

```python
expected = solid.mass - 4 * math.pi * (5.5**2 - 3.3**2) * 6.5 - slot.Face().mass * thickness
print("volume", clamp.mass, "expected", expected)
print(sorted({f.name for f in clamp.faces if f.name}))
```

## Options

| Argument | Meaning |
|---|---|
| `length` | The extent along the direction, from the profile's plane |
| `length2` | The extent against the direction, so the solid reaches across the plane; 0 by default |
| `dir` | The direction of the extrusion, any direction that leaves the plane, also tilted; by default the plane's normal, for a pocket its negative |
| `reverse` | `True` turns the direction around |
| `until` | Instead of a length: a `px.Plane`, a flat OpenCASCADE face, or a planex face, shape or sketch, up to its plane; for a pocket also `px.first` or `px.last`, the first or last flat face of the target along the direction |

The solid carries the name, `maxh` and color of the profile's face. Each side face carries the properties of its
profile edge, the two end faces the color and `maxh` of the face, and the edges along the direction the properties of
the profile vertex they start at. See [Placing a sketch](../sketch/placement.md) for sketches on the faces of solids
and [OpenCASCADE](../../integrations/occ/index.md) for the export in general.