---
jupyter:
  description: 'Parameters shared by planex2d sketches: px.Parameters holds named values, sk.Use lets a sketch''s
    expressions name them, and one Update changes every sketch that uses them. A flange and its gasket that keep their
    bolt holes in line.'
---

# Parameters shared by sketches

Parts that fit together share dimensions. A flange and its gasket have the same bolt circle, and when the bolt circle
changes, both have to change with it. `px.Parameters` holds such values by name. A sketch that uses the set with
`sk.Use(p)` can name the values in its expressions, and `p.Update(...)` sets new values in every sketch that uses
them, in one step.

```python
import math

import planex as px
```

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

## A flange and its gasket

The example is a round flange with an outer diameter of 120, four bolt holes of 9 on a bolt circle of 90 and a bore of
50, and its gasket, which has the same outline and holes but an opening of 70. The three shared values are parameters:

```python
p = px.Parameters(od=120, pcd=90, bolt=9)
print(p)
```

Both parts are drawn by one function. Each sketch dimensions its outline, its bore and one bolt hole, and three
expressions tie the shared dimensions to the parameters. A circular pattern then repeats the hole four times:

```python
def part(bore):
    sk = px.Sketch().Use(p)
    sk.Circle((0, 0), 58, id="outer")
    sk.Constrain("outer.center", px.Fix)
    sk.Constrain("outer", px.Diameter, 116, id="outer_d")
    sk.Circle((0, 0), bore / 2, id="bore")
    sk.Constrain("bore", "outer", px.Concentric)
    sk.Constrain("bore", px.Diameter, bore, id="bore_d")
    sk.Circle((44, 0), 4, id="hole")
    sk.Constrain("hole", px.Diameter, 8, id="hole_d")
    sk.Constrain("hole.center", "outer.center", px.Distance, 44, id="hole_r")
    sk.Constrain("hole.center", "outer.center", px.Horizontal)
    sk.Expression("outer_d = od").Expression("hole_r = pcd / 2").Expression("hole_d = bolt")
    sk.CircularPattern("hole", "outer.center", 4)
    return sk


flange, gasket = part(50), part(70)
print("flange", flange.status, "gasket", gasket.status)
```

The outline and the hole were drawn at rough sizes. The expressions bring them to the parameters' values, so both parts
are fully constrained with an outer diameter of 120 and their holes on the bolt circle of 90 (Figure 1). Their areas
are the disc less the bore and the four holes:

```python
for name, sk, bore in (("flange", flange, 50), ("gasket", gasket, 70)):
    print(name, "area", sk.Face().mass, "exact", math.pi / 4 * (120**2 - bore**2 - 4 * 9**2))
```

```python nbsphinx="hide-input"
Row((flange.Face(), "The flange"), (gasket.Face(), "The gasket"),
    caption="A flange and its gasket from one parameter set")
```

## One update for both

A larger flange, with an outer diameter of 130, a bolt circle of 100 and bolts of 11, is one call. `p.Update` sets the
three values and solves both sketches again:

```python
p.Update(pcd=100, od=130, bolt=11)
for name, sk, bore in (("flange", flange, 50), ("gasket", gasket, 70)):
    print(name, "area", sk.Face().mass, "exact", math.pi / 4 * (130**2 - bore**2 - 4 * 11**2))
```

The bolt holes of the two parts stay in line, each of them at the same place in both:

```python
def holes(sk):
    centers = [sk.Measure(ref)["center"][:2] for ref in sk.elements["Circle"] if ref not in ("outer", "bore")]
    return sorted((round(x, 9), round(y, 9)) for x, y in centers)


print(holes(flange))
print(holes(flange) == holes(gasket))
```

## The rules

- A parameter is set only by `p.Update`. Setting it in a sketch, as `flange["pcd"] = 110`, raises an error, as do
  driving it and removing it there.
- Inside a sketch, its dimensions stay its own, with their own ids. No dimension or element of a sketch may have the
  name of a parameter, and `h`, `v` and `t` are no parameter names, since curve formulas use them.
- `p.Update` changes all sketches or none. If one of them has no solution for the new values, it raises an error that
  names that sketch and leaves every sketch as it was.
- Curve formulas may name parameters too. See [Parametric curves](../sketch/parametric-curves.md) for curves.

```python
try:
    flange["pcd"] = 110
except ValueError as err:
    print(err)
```