Python API

Everything the UI does, a script can do. This list is generated from the application's command catalog, so it is the same list the command palette uses.

Import yonta from the Python console inside the application or from a standalone script. Every command is one undo step and is recorded by the macro recorder as the Python call shown here.

A parameter marked ? is optional. Methods on Document and Sketch are called on an object, so their document parameter is implied. The same list as JSON: commands.json.

A complete example

import yonta

doc = yonta.new_document("Bracket")
sketch = doc.new_sketch(plane="XY", name="Body")
sketch.add_circle((0, 0), 20.0)
body = doc.pad(sketch, 10.0)
doc.recompute()
doc.export("bracket.step")
doc.save("bracket.yonta")

Application

`yonta.new_document(name?, body?)`

Command: app.new_document · New document

Create a new document and make it active.

Example

doc = yonta.new_document("Bracket")

`yonta.open_document(path, name?, background?, copy?)`

Command: app.open_document · Open document

Open a .yonta file as a new document.

Example

doc = yonta.open_document("bracket.yonta")

`yonta.close_document(document?)`

Command: app.close_document · Close document

Close a document without saving.

Example

yonta.close_document(doc)

`yonta.set_active_document(document)`

Command: app.set_active_document · Switch document

Make an open document the active one.

Example

yonta.set_active_document(doc)

Document

`Document.add_object(document?, type, name?)`

Command: doc.add_object · Add object

Add an object of a registered type.

Example

sketch = doc.add_object("yonta.sketch.sketch")

`Document.remove_object(document?, object)`

Command: doc.remove_object · Remove object

Remove an object.

Example

doc.remove_object(body)

`Document.set_visible(document?, objects, visible)`

Command: doc.set_visible · Set visible

Show or hide objects in the 3D view: one undo step, saved with the document, no recompute.

Example

doc.set_visible([body], False)

`Document.set_suppressed(document?, objects, suppressed?)`

Command: doc.set_suppressed · Suppress

Suppress objects: they are not computed, each passing its base's solid through; or bring them back.

Example

doc.set_suppressed([body])

`Document.rollback(document?, object?)`

Command: doc.set_rollback · Rollback

Roll the model back to an object, or forward to the end: what follows is not computed.

Example

doc.rollback()

`Document.move_object(document?, object, before?)`

Command: doc.move_object · Move in tree

Move an object to another place in the model tree; a feature takes its new place in the solid chain.

Example

doc.move_object(body)

`Document.rename(document?, object, name)`

Command: doc.rename · Rename

Give an object another name; links to it keep working.

Example

doc.rename(body, "Base")

`Document.set_label(document?, object, label)`

Command: doc.set_label · Set label

Set the name the window shows for an object; its name in Python and the file stays.

Example

doc.set_label(body, "Base plate")

`Document.set_property(document?, object, property, value)`

Command: doc.set_property · Set property

Set a property of an object.

Example

doc.set_property(body, "Length", 10.0)

`Document.add_parameter(document?, name, expression, quantity?, group?, minimum?, maximum?, comment?, before?)`

Command: doc.add_parameter · Add parameter

Add a parameter to the document's table; the first one makes the table.

Example

doc.add_parameter("Body", expression)

`Document.set_parameter(document?, name, expression)`

Command: doc.set_parameter · Set parameter

Give a parameter another expression; what reads it follows in the same step.

Example

doc.set_parameter("Body", expression)

`Document.edit_parameter(document?, name, quantity?, group?, minimum?, maximum?, comment?)`

Command: doc.edit_parameter · Edit parameter

Change a parameter's kind, group, limits or comment.

Example

doc.edit_parameter("Body")

`Document.move_parameter(document?, name, before?)`

Command: doc.move_parameter · Move parameter

Move a parameter to another place in the table.

Example

doc.move_parameter("Body")

`Document.rename_parameter(document?, old, new)`

Command: doc.rename_parameter · Rename parameter

Give a parameter another name; every expression that uses it is written anew.

Example

doc.rename_parameter(old, new)

`Document.remove_parameter(document?, name, keep_values?)`

Command: doc.remove_parameter · Delete parameter

Remove a parameter that nothing uses, or turn what uses it into values.

Example

doc.remove_parameter("Body")

`Document.set_expression(document?, object, property, expression)`

Command: doc.set_expression · Set expression

Give a numeric property of an object an expression.

Example

doc.set_expression(body, "Length", expression)

`Document.clear_expression(document?, object, property)`

Command: doc.clear_expression · Clear expression

Take a property's expression away; its last value stays.

Example

doc.clear_expression(body, "Length")

`Document.recompute(document?, background?)`

Command: doc.recompute · Recompute

Recompute a document.

Example

doc.recompute()

`Document.undo(document?)`

Command: doc.undo · Undo

Undo the last change of a document.

Example

doc.undo()

`Document.redo(document?)`

Command: doc.redo · Redo

Redo the last undone change of a document.

Example

doc.redo()

`Document.save(document?, path?, rename?, force?)`

Command: doc.save · Save

Save a document to a .yonta file.

Example

doc.save("bracket.yonta")

`Document.export(document?, path, objects?, schema?, stl_format?, unit?, resolution?, y_up?)`

Command: doc.export · Export

Export solids to STEP or STL.

Example

doc.export("bracket.step")

`Document.import_step(document?, path, name?)`

Command: doc.import_step · Import STEP

Import a STEP file: one solid object per root or leaf instance.

Example

imported = doc.import_step("housing.step")

`Document.copy_sketch(document?, sketch, plane?, source?, name?)`

Command: doc.copy_sketch · Copy sketch

Copy a sketch, with every constraint, onto a base plane, from this document or another.

Example

doc.copy_sketch(sketch)

Part

`Document.new_sketch(document?, plane?, support?, face?, name?)`

Command: part.new_sketch · New sketch

Add a sketch on a base plane or a planar face.

Example

sketch = doc.new_sketch(plane="XY", name="Body")

`Document.pad(document?, profile?, length?, name?, through_all?, reversed?, symmetric?, side?, second_length?, extent?, up_to?, up_to_element?, offset?, profile_edge?, new_body?, support?, face?, thin?)`

Command: part.pad · Pad

Extrude a closed sketch into a solid, joined to the tip solid.

Example

body = doc.pad(sketch, 10.0)

`Document.pocket(document?, profile?, length?, name?, through_all?, reversed?, symmetric?, side?, second_length?, extent?, up_to?, up_to_element?, offset?, profile_edge?, support?, face?)`

Command: part.pocket · Pocket

Cut a closed sketch into the tip solid.

Example

body = doc.pocket(sketch, 5.0)

`Document.revolve(document?, profile, angle?, axis?, name?, new_body?)`

Command: part.revolve · Revolve

Revolve a closed sketch about an axis, joined to the tip solid.

Example

body = doc.revolve(sketch, 2 * math.pi)

`Document.groove(document?, profile, angle?, axis?, name?)`

Command: part.groove · Groove

Revolve a closed sketch about an axis and cut it from the tip solid.

Example

body = doc.groove(sketch, math.pi / 2)

`Document.fillet(document?, edges, radius?, base?, name?, sizes?, chains?)`

Command: part.fillet · Fillet

Round edges of the tip solid with a radius.

Example

body = doc.fillet([edge], 1.0)

`Document.chamfer(document?, edges, size?, base?, name?, sizes?, chains?)`

Command: part.chamfer · Chamfer

Bevel edges of the tip solid by a distance.

Example

body = doc.chamfer([edge], 0.5)

`Document.shell(document?, faces, thickness?, outward?, join?, base?, name?)`

Command: part.shell · Shell

Hollow the tip solid to a wall, open at the chosen faces.

Example

doc.shell([face], thickness=4.0)

`Document.draft(document?, faces, angle?, neutral, neutral_element?, pull?, pull_element?, reversed?, base?, name?)`

Command: part.draft · Draft

Tilt faces of the tip solid about a neutral plane, as a moulded part needs.

Example

body = doc.draft([face], math.radians(2.0), neutral=(body, bottom))

`Document.primitive(document?, kind, length?, width?, height?, radius?, radius2?, plane?, support?, face?, origin?, new_body?, name?)`

Command: part.primitive · Primitive

Add a box, cylinder, sphere or cone as a solid.

Example

box = doc.primitive("box", length=40.0, width=20.0, height=10.0)

`Document.loft(document?, profiles, profile_edges?, ruled?, closed?, new_body?, name?)`

Command: part.loft · Loft

Build a solid through profiles in order.

Example

doc.loft([sketch, upper])

`Document.sweep(document?, profile, path, path_edges?, frame?, transition?, profile_edge?, new_body?, name?)`

Command: part.sweep · Sweep

Sweep a profile along a path into a solid.

Example

body = doc.sweep(profile, path)

`Document.mirror(document?, plane?, support?, face?, base?, name?, features?, new_body?)`

Command: part.mirror · Mirror

Join the tip solid with its reflection in a plane or a planar face.

Example

body = doc.mirror(plane="YZ")

`Document.pattern_linear(document?, features, direction?, count?, spacing?, direction2?, count2?, spacing2?, length?, offset?, end_offset?, symmetric?, reversed?, skip?, base?, name?)`

Command: part.pattern_linear · Linear pattern

Copy features' tools along a direction: the count includes the original.

Example

row = doc.pattern_linear([hole], direction="X", count=4, spacing=15.0)

`Document.pattern_circular(document?, features, axis?, count?, angle?, offset?, end_offset?, symmetric?, reversed?, skip?, base?, name?)`

Command: part.pattern_circular · Polar pattern

Copy features' tools round an axis: the count includes the original.

Example

ring = doc.pattern_circular([hole], axis="Z", count=6, angle=math.radians(60.0))

`Document.body(document?, name?)`

Command: part.body · New body

Add an empty body: the next feature with no base joins it.

Example

doc.body()

`Document.set_material(document?, objects, material?, density?)`

Command: part.set_material · Material

Set the material of a body's solid (a feature's is its body's): a table material or a custom density; its mass follows.

Example

doc.set_material([body])

`Document.section_plane(document?, plane?, support?, face?, flip?, offset?, name?)`

Command: part.section_plane · Section plane

Add the document's section plane on XY, XZ or YZ or on a planar face: the side its normal points to is cut away in the view; no solid changes.

Example

doc.section_plane()

`Document.boolean(document?, tools, operation?, base?, name?)`

Command: part.boolean · Boolean

Fuse, cut or intersect other bodies into a body.

Example

doc.boolean("Body001")

`Document.hole(document?, profile, diameter?, depth?, through_all?, reversed?, base?, name?, type?, standard?, size?, fit?, series?, thread_length?, left_hand?, counterbore?, countersink?, tip?, tip_angle?, depth_to?, end?, support?, up_to_face?, offset?, far_counterbore?)`

Command: part.hole · Hole

Drill plain holes at a sketch's points and circle centres into the tip solid.

Example

body = doc.hole(sketch, 3.0, 5.0)

`Document.datum_plane(document?, plane?, support?, face?, offset?, name?, method?, references?, angle?)`

Command: part.datum_plane · Datum plane

A reference plane on a base plane or a planar face, moved by an offset.

Example

plane = doc.datum_plane(plane="XY", offset=10.0)

`Document.datum_axis(document?, axis?, support?, edge?, offset?, name?)`

Command: part.datum_axis · Datum axis

A reference axis along X, Y or Z, or on a straight edge, moved by an offset.

Example

doc.datum_axis()

`Document.datum_point(document?, support?, vertex?, offset?, name?)`

Command: part.datum_point · Datum point

A reference point at the origin or a vertex, moved by an offset.

Example

doc.datum_point()

Sketch

`Sketch.add_line(document?, sketch, kind, coords, construction?)`

Command: sketch.add_geometry · Add sketch element

Add a point, line, circle or arc to a sketch.

Example

line = sketch.add_line((0, 0), (10, 0))

`Sketch.copy(document?, sketch, geometry, offset?, angle?, center?)`

Command: sketch.copy_geometry · Copy sketch elements

Copy sketch elements moved by an offset or turned about a point, with the constraints among them.

Example

copies = sketch.copy([line], offset=(10.0, 0.0))

`Sketch.add_external(document?, sketch, object, edge?, edges?)`

Command: sketch.add_external · Add external geometry

Project an edge of another object into the sketch as fixed construction geometry that follows it.

Example

external = sketch.add_external(body, edge)

`Sketch.add_constraint(document?, sketch, type, first, second?, value?, value2?, third?, inner?, driving?, expression?)`

Command: sketch.add_constraint · Constraint

Add a sketch constraint.

Example

sketch.add_constraint("coincident", (line, "end"), (other, "start"))

`Sketch.set_value(document?, sketch, constraint, value)`

Command: sketch.set_value · Change dimension

Change a sketch dimension.

Example

sketch.set_value(constraint, 10.0)

`Sketch.set_label(document?, sketch, constraint, offset?)`

Command: sketch.set_label · Move dimension label

Place a dimension's label away from its default place; dragging a label does this.

Example

sketch.set_label(constraint)

`Sketch.set_expression(document?, sketch, constraint, expression)`

Command: sketch.set_expression · Set dimension expression

Give a driving dimension an expression.

Example

sketch.set_expression(constraint, expression)

`Sketch.clear_expression(document?, sketch, constraint)`

Command: sketch.clear_expression · Clear dimension expression

Take a dimension's expression away; its last value stays.

Example

sketch.clear_expression(constraint)

`Sketch.set_driving(document?, sketch, constraint, driving)`

Command: sketch.set_driving · Reference dimension

Make a dimension a reference dimension, which measures and is never solved for, or a driving one again.

Example

sketch.set_driving(constraint, False)

`Sketch.move(document?, sketch, ref, to, grab?)`

Command: sketch.move · Drag

Drag a point or an element within its constraints; no constraint is added or removed.

Example

sketch.move((line, "end"), (25.0, 5.0))

`Sketch.set_construction(document?, sketch, geometry, on)`

Command: sketch.set_construction · Construction geometry

Make elements construction geometry, which guides and constrains but is never part of a profile, or normal geometry again.

Example

sketch.set_construction([line], True)

`Sketch.trim(document?, sketch, geometry, at)`

Command: sketch.trim · Trim

Remove the piece of a line, arc or circle between the curves that cut it.

Example

sketch.trim(line, (16.0, 0.0))

`Sketch.extend(document?, sketch, geometry, end)`

Command: sketch.extend · Extend

Lengthen a line or an arc from one end to the next curve ahead.

Example

sketch.extend(line, "end")

`Sketch.offset(document?, sketch, geometry, distance, constraints?)`

Command: sketch.offset · Offset

Copy elements a distance away, joined where they meet and tied to their sources.

Example

sketch.offset([line], 2.0)

`Sketch.fillet(document?, sketch, corner?, geometry?, radius, constraints?)`

Command: sketch.fillet · Sketch fillet

Round a sketch corner with a tangent arc; the corner's dimensions are kept.

Example

sketch.fillet((line, "end"), 3.0)

`Sketch.transform(document?, sketch, geometry, offset?, angle?, center?)`

Command: sketch.transform · Move sketch elements

Move or turn sketch elements themselves, keeping their constraints.

Example

sketch.transform([line], angle=math.radians(90.0))

`Sketch.mirror(document?, sketch, geometry, axis, constraints?)`

Command: sketch.mirror · Mirror sketch elements

Copy sketch elements mirrored in a line, with their constraints.

Example

sketch.mirror([line], other.id)

`Sketch.set_polygon_sides(document?, sketch, geometry, sides)`

Command: sketch.set_polygon_sides · Polygon sides

Give a polygon another number of sides; its circle and its first side's constraints stay.

Example

sketch.set_polygon_sides(circle, 5)

`Sketch.remove_geometry(document?, sketch, geometry)`

Command: sketch.remove_geometry · Remove sketch element

Remove a sketch element and its constraints.

Example

sketch.remove_geometry(line)

`Sketch.remove_constraint(document?, sketch, constraint)`

Command: sketch.remove_constraint · Remove constraint

Remove a sketch constraint.

Example

sketch.remove_constraint(constraint)