understanding the "translate()" functionality

[jbernalr]

I have here a minimal code:

import cadquery as cq
from cadquery import exporters

filename = './rack.stl'
l_rack = 30 # mm [lenght of the rack]
base_x = 10  # mm [base width]
base_y = 10  # mm [base height]

r_x = 0.6
r_y = 0.6 

rack = cq.Workplane("XY").box(base_x, base_y, l_rack).\
    faces(">Z").workplane().rect(r_x*base_x, r_y*base_y).cutThruAll().\
    workplane().translate((0,50,10)).rect(r_x*base_x, r_y*base_x).extrude(10)

which produces the figure depicted at the bottom.
however, I cannot translate my extrusion from the center.

I tried the following variations without success:

workplane().translate((0,50,10)).rect(r_x*base_x, r_y*base_x).extrude(10)
faces(">Z").workplane().translate((0,50,10)).rect(r_x*base_x, r_y*base_x).extrude(10)
workplane().rect(r_x*base_x, r_y*base_x).translate((0,50,10)).extrude(10)
workplane().rect(r_x*base_x, r_y*base_x).extrude(10).translate((0,50,10)).

I read the docs and saw examples where the translation happens at the trailing part of the object.
Is this behaviour as expected? can anyone spot the error?

[lorenzncode]

workplane() was called immediately before translate((0, 50, 10)). This is a problem.

translate "Returns a copy of all of the items on the stack moved by ..."

By calling workplane() you create an empty workplane so there are no items on the stack to move.

Here is an example where the box is moved:

rack = (
    cq.Workplane("XY")
    .box(base_x, base_y, l_rack)
    .translate((0, 50, 10))
)

[jbernalr]

@lorenzncode thanks. Just let say you are r building (as in my case) on top of this initial box of you and pick one of the faces to create a square you want to extrude. Where should the translate be located? I can reproduce your example, but I cannot use translate on a face of an existing body.

[lorenzncode]

The origin depends on centerOption when creating a workplane on a face. One way to change the origin is to specify it (requires "ProjectedOrigin" centerOption which is the default).

result = (
    cq.Workplane()
    .box(10, 10, 30)
    .faces(">Z")
    .workplane(origin=(0, 2, 0))
    .rect(6, 6)
    .extrude(-10, combine="s")
)

Or call center:

result = (
    cq.Workplane()
    .box(10, 10, 30)
    .faces(">Z")
    .workplane()
    .center(0, 2)
    .rect(6, 6)
    .extrude(-10, combine="s")
)

Another way to locate a workplane is covered in the docs example "Locating a Workplane on a vertex". Here locating on an edge:

result = (
    cq.Workplane()
    .box(10, 10, 30)
    .faces(">Z")
    .edges(">Y")
    .workplane(centerOption="CenterOfMass")
    .center(0, -3)
    .rect(6, 6)
    .extrude(-10, combine="s")
)

You might have moved the shape in a sketch:

s = cq.Sketch().push([(0, 2)]).rect(6, 6)

result = (
    cq.Workplane()
    .box(10, 10, 30)
    .faces(">Z")
    .workplane()
    .placeSketch(s)
    .extrude(-10, combine="s")
)

(Note that Sketch and extrude with combine="s" is not available in version 2.1.)

[jbernalr]

@lorenzncode that's it. thanks!
would be correct to say that translate only works on solids created from the cadquery primitives?
I may do a PR with a few sentences in the documentation

[lorenzncode]

We can create the same shape as before using translate (probably not the most straightforward way):

result = (
    cq.Workplane()
    .box(10, 10, 30)
    .faces(">Z")
    .translate((0, 2, 0))
    .wires()
    .toPending()
    .offset2D(-2)
    .extrude(-10, combine="s")
)

translate works with any type of shape - a face in this example.