Rotating objects created by polarArray()

[gridstop]

I can't figure out how to rotate things created on the points of a polarArray(). Specifically something like:
cq.Workplane("XY").polarArray(100,0,360,6).cylinder(10,20,angle=180)
Creates a ring of six cylinder objects, each one is a half cylinder because of the angle=180, and the start angle for each is pointed inwards to the center of the polarArray. OK so far. But if I want to rotate each of those cylinders by 90 so the start isn't directly inward, but instead is to the side, this seems to be impossible, or much more complicated.
You can't rotate the points created by polarArray() before doing the cylinder, and after calling cylinder(), attempting to rotate rotates the entire combined object, not each individual cylinder. Adding combine=False to the cylinder() call does nothing either. Possibly each individual object is being rotated, but is being rotated around the center of the polarArray rather than each objects center, and I can't figure out how to make that rotate local. rotate() doesn't take any parameters that would seem to modify where the center of rotation is, only the orientation of the axis.

If anyone has any advice I'd appreciate it.

[lorenzncode]

Is this what you are looking for - control of angle a1 as in this example?:

import cadquery as cq

a1 = -90
shape1 = (
    cq.Workplane().cylinder(10, 20, angle=180).rotate((0, 0, 0), (0, 0, 1), a1).val()
)
res = cq.Workplane("XY").polarArray(100, 0, 360, 6).eachpoint(shape1)

You might also try with Sketch:

import cadquery as cq

a1 = -90
sk1 = cq.Sketch().parray(100, 0, 360, 6).arc((0, 0), 20, a1, 180).close().assemble()
res = cq.Workplane().placeSketch(sk1).extrude(10)

Another way to create the half circle is with free function API:

from cadquery.func import *
from math import pi

c1 = circle(20).trim(0, pi)
s1 = segment((-20, 0, 0), (20, 0, 0))
f1 = face(wire(c1, s1))

[gridstop]

Thanks! The construction of a shape, using val() and eachpoint() was the trick to do it right. I think if I struggle with anything in cadquery the most it's knowing how and when to construct temporary objects rather than just building on the stack, and how to join them back in to an object correctly.

[lorenzncode]

val was not strictly necessary here because eachpoint accepts Workplane objects too.

If we do call val, there is an easy way to rotate around z now with move:

shape1 = (
    cq.Workplane()
    .cylinder(10, 20, angle=180)
    .val()
    .move(rz=a1)
)

[adam-urbanczyk]

Thanks! The construction of a shape, using val() and eachpoint() was the trick to do it right. I think if I struggle with anything in cadquery the most it's knowing how and when to construct temporary objects rather than just building on the stack, and how to join them back in to an object correctly.

TBH eachpoint is not very well documented, val() is mentioned explicitly: https://cadquery.readthedocs.io/en/latest/primer.html#fluent-api-direct-api. I'd say always split, when things get too complicated. Or simply stop using Workplane if your designs are too complex.