---
jupyter:
  description: 'A C-clamp frame step by step: five parameters drive a planex2d sketch drawn with the pen, and
    OpenCASCADE extrudes, drills and pads it into a solid that keeps its face names.'
---

# A C-clamp, step by step

Five numbers drive the frame of a C-clamp: the throat depth of 60, the jaw gap of 40, the wall thickness t = 12, the
fillet radius r = 6 and the frame thickness b = 16. The profile is drawn with the pen, with every side a length along
it and every corner a turn or an arc. All of them are computed from the five numbers, so changing a number changes the
whole part. The profile is then extruded into the frame, drilled for the screw and given an anvil pad, with
OpenCASCADE doing the 3D operations.

```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, Vertices
```

## The profile

The sketch lies in the xz plane, with h along x and v along z, so its normal points along −y. W = t + depth is the
width of the profile and H = gap + 2t its height. The pen starts at the end of the lower bend, heading
along x, and runs once around counterclockwise. It draws the bottom, the lower tip, the lower jaw, the inner fillet of
radius `r` into the throat and out of it, the upper jaw and tip, the top, and the outer bends of radius `r + t` around
the same centers, so that the wall keeps its thickness around the bend. `Turn(90)` turns the pen left for a square
corner, and `Arc(r, -90)` is a fillet that turns it right, into the mouth. Every edge carries a `name`, which the faces
of the solid take over below (Figure 1).

```python
depth, gap, t, r, b = 60, 40, 12, 6, 16
W, H = t + depth, gap + 2 * t

side = px.QuickSketch(px.Plane(normal=(0, -1, 0), axis=(1, 0, 0)))
side.Move((r + t, 0), dir=(1, 0))
side.Line(W - r - t, name="bottom").Turn(90).Line(t, name="lower tip").Turn(90)
side.Line(W - t - r, name="lower jaw").Arc(r, -90, name="lower fillet")
side.Line(gap - 2 * r, name="throat").Arc(r, -90, name="upper fillet")
side.Line(W - t - r, name="upper jaw").Turn(90).Line(t, name="upper tip").Turn(90)
side.Line(W - r - t, name="top").Arc(r + t, 90, name="upper bend")
side.Line(H - 2 * (r + t), name="rear").Arc(r + t, 90, name="lower bend")
face = side.Face()
print("the pen ends at", side.pen.position, "where it started")
```

```python nbsphinx="hide-input"
shift = {"rear": -9, "throat": 10}
names = [(e.name, (e.PointAt(0.5).h + shift.get(e.name, 0), e.PointAt(0.5).v)) for e in face.edges
         if "tip" not in e.name]
Row((side, "The profile drawn with the pen", {"fill": False, "marks": Vertices(face)}),
    (face, "The face, its edges named", {"labels": names}), caption="The C-clamp profile")
```

## Check

The area is that of the outer rectangle with two rounded corners minus the mouth with two rounded corners:

```python
k = 2 * (1 - math.pi / 4)
area = W * H - k * (r + t) ** 2 - (depth * gap - k * r**2)
print("area", face.mass, "exact", area)
```

## The frame

`px.Pad` extrudes the profile along its normal by b into an OpenCASCADE solid:

```python
frame = px.Pad(face, b)
Draw(frame)
```

## The screw hole

The screw hole, of diameter 10, is sketched on the top face of the frame, 20 from its tip. `px.QuickSketch(face)` puts
the sketch on the face's plane with its outward normal and projects the origin and the x axis onto it, so here h = x
and v = y. `px.Pocket` cuts the hole from there down through the upper jaw.

```python
top = px.QuickSketch(frame.faces.Max(occ.Z))
frame = px.Pocket(frame, top.Circle(W - 20, -b / 2, 5), 2 * t)
Draw(frame)
```

## The anvil pad

The anvil pad, of diameter 14 and 3 high, is sketched on the face of the lower jaw, which is the face nearest to the
screw axis at jaw height. `px.Pad` extrudes it out of that face, and the union adds it to the frame.

```python
jaw = px.QuickSketch(frame.faces.Nearest(occ.Pnt(W - 20, -b / 2, t)))
frame = frame + px.Pad(jaw.Circle(W - 20, -b / 2, 7), 3)
Draw(frame)
```

## Check the volume

The volume is the profile times b, minus the hole through the upper jaw, plus the pad:

```python
print("volume", frame.mass, "exact", area * b - math.pi * 5**2 * t + math.pi * 7**2 * 3)
```

## Mesh and export

The edge names of the profile become the names of the faces of the solid, so netgen's mesh knows them as boundaries.
The mesh is curved to third order, and the solid is written as a STEP file.

```python
print(sorted({f.name for f in frame.faces if f.name}))
```

```python
mesh = occ.OCCGeometry(frame).GenerateMesh(maxh=4)
mesh.Curve(3)
Draw(mesh)
frame.WriteStep("clamp.step")
```