Importing and Exporting Files

Introduction

The purpose of this section is to explain how to import external file formats into CadQuery, and export files from it as well. While the external file formats can be used to interchange CAD model data with other software, CadQuery does not support any formats that carry parametric data with them at this time. The only format that is fully parametric is CadQuery’s own Python format. Below are lists of the import and export file formats that CadQuery supports.

Import Formats

DXF
STEP

Export Formats

DXF
SVG
STEP
STL
AMF
TJS
VRML
VTP
3MF
glTF

Notes on the Formats

DXF is useful for importing complex 2D profiles that would be tedious to create using CadQuery’s 2D operations. An example is that the 2D profiles of aluminum extrusion are often provided in DXF format. These can be imported and extruded to create the length of extrusion that is needed in a design.
STEP files are useful for interchanging model data with other CAD and analysis systems, such as FreeCAD. Many parts such as screws have STEP files available, which can be imported and used in CadQuery assemblies.
STL, AMF and 3MF files are mesh-based formats which are typically used in additive manufacturing (i.e. 3D printing). AMF and 3MF files support more features, but are not as universally supported as STL files.
TJS is short for ThreeJS, and is a JSON mesh format that is useful for displaying 3D models in web browsers. The TJS format is used to display embedded 3D examples within the CadQuery documentation.
VRML is a mesh-based format for representing interactive 3D objects in a web browser.
VTP is a mesh-based format used by the VTK library.
glTF is a mesh-based format useful for viewing models on the web. Whether the resulting glTF file is binary (.glb) or text (.gltf) is set by the file extension.

Importing DXF

DXF files can be imported using the importers.importDXF() method.

importers.importDXF(tol: float = 1e-06, exclude: List[str] = [], include: List[str] = []) → Workplane

Loads a DXF file into a Workplane.

All layers are imported by default. Provide a layer include or exclude list to select layers. Layer names are handled as case-insensitive.

Parameters

filename (str) – The path and name of the DXF file to be imported
tol (float) – The tolerance used for merging edges into wires
exclude (List[str]) – a list of layer names not to import
include (List[str]) – a list of layer names to import

Return type

Workplane

Importing a DXF profile with default settings and using it within a CadQuery script is shown in the following code.

import cadquery as cq

result = (
    cq.importers.importDXF("/path/to/dxf/circle.dxf").wires().toPending().extrude(10)
)

Note the use of the Workplane.wires() and Workplane.toPending() methods to make the DXF profile ready for use during subsequent operations. Calling toPending() tells CadQuery to make the edges/wires available to the next modelling operation that is called in the chain.

Importing STEP

STEP files can be imported using the importers.importStep() method (note the capitalization of “Step”). There are no parameters for this method other than the file path to import.

import cadquery as cq

result = cq.importers.importStep("/path/to/step/block.stp")

Exporting STEP

This section covers exporting CadQuery Workplane objects to STEP. For exporting assemblies to STEP, see the next section.

Default

The exporters module handles exporting Workplane objects to STEP. It is not necessary to set the export type explicitly since it will be determined from the file extension. Below is an example.

# Create a simple object
box = cq.Workplane().box(10, 10, 10)

# Export the box
cq.exporters.export(box, "/path/to/step/box.step")

Non-Default File Extensions

If there is a requirement to export the STEP file using an “stp” extension, CadQuery will throw an error saying that it does not recognize the file extension. In that case the export type has to be specified.

# Create a simple object
box = cq.Workplane().box(10, 10, 10)

# Export the box
cq.exporters.export(box, "/path/to/step/box.stp", cq.exporters.ExportTypes.STEP)

# The export type may also be specified as a literal
cq.exporters.export(box, "/path/to/step/box2.stp", "STEP")

Setting Extra Options

There are additional options that can be set when exporting an object to a STEP file. For an explanation of the options available, see the documentation of the Shape.exportStep() method or the Assembly.exportAssembly`() method.

# Create a simple object
box = cq.Workplane().box(10, 10, 10)

# Export the box, provide additional options with the opt dict
cq.exporters.export(box, "/path/to/step/box.step", opt={"write_pcurves": False})

# or equivalently when exporting a lower level Shape object
box.val().exportStep("/path/to/step/box2.step", write_pcurves=False)

Exporting Assemblies to STEP

It is possible to export CadQuery assemblies directly to STEP. The STEP exporter has multiple options which change the way exported STEP files will appear and operate when opened in other CAD programs. All assembly export methods shown here will preserve the color information from the assembly.

Default

CadQuery assemblies have a Assembly.save() method which can write an assembly to a STEP file. An example assembly export with all defaults is shown below.

import cadquery as cq

# Create a sample assembly
assy = cq.Assembly()
body = cq.Workplane().box(10, 10, 10)
assy.add(body, color=cq.Color(1, 0, 0), name="body")
pin = cq.Workplane().center(2, 2).cylinder(radius=2, height=20)
assy.add(pin, color=cq.Color(0, 1, 0), name="pin")

# Save the assembly to STEP
assy.save("out.step")

This will produce a STEP file that is nested with auto-generated object names. The colors of each assembly object will be preserved, but the names that were set for each will not.

Fused

The following will attempt to create a single, fused shape while preserving the name and color information of each assembly object. The process of fusing the solid may cause performance issues in some cases, and is likely to alter the faces of the fused solids.

import cadquery as cq

# Create a sample assembly
assy = cq.Assembly()
body = cq.Workplane().box(10, 10, 10)
assy.add(body, color=cq.Color(1, 0, 0), name="body")
pin = cq.Workplane().center(2, 2).cylinder(radius=2, height=20)
assy.add(pin, color=cq.Color(0, 1, 0), name="pin")

# Save the assembly to STEP
assy.save("out.stp", "STEP", mode="fused")

# Specify additional options such as glue as keyword arguments
assy.save("out_glue.step", mode="fused", glue=True, write_pcurves=False)

Naming

It is also possible to set the name of the top level assembly object in the STEP file with either the DEFAULT or FUSED methods. This is done by setting the name property of the assembly before calling Assembly.save().

assy = Assembly(name="my_assembly")
assy.save(
    "out.stp",
    cq.exporters.ExportTypes.STEP,
    mode=cq.exporters.assembly.ExportModes.FUSED,
)

If an assembly name is not specified, a UUID will be used to avoid name conflicts.

Exporting SVG

The SVG exporter has several options which can be useful for achieving the desired final output. Those options are as follows.

width - Width of the resulting image (None to fit based on height).
height - Height of the resulting image (None to fit based on width).
marginLeft - Inset margin from the left side of the document.
marginTop - Inset margin from the top side of the document.
projectionDir - Direction the camera will view the shape from.
showAxes - Whether or not to show the axes indicator, which will only be visible when the projectionDir is also at the default.
strokeWidth - Width of the line that visible edges are drawn with.
strokeColor - Color of the line that visible edges are drawn with.
hiddenColor - Color of the line that hidden edges are drawn with.
showHidden - Whether or not to show hidden lines.
focus - If specified, creates a perspective SVG with the projector at the distance specified.

The options are passed to the exporter in a dictionary, and can be left out to force the SVG to be created with default options. Below are examples with and without options set.

Without options:

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(result, "/path/to/file/box.svg")

Results in:

Note that the exporters API figured out the format type from the file extension. The format type can be set explicitly by using exporters.ExportTypes.

The following is an example of using options to alter the resulting SVG output by passing in the opt parameter.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(
    result,
    "/path/to/file/box_custom_options.svg",
    opt={
        "width": 300,
        "height": 300,
        "marginLeft": 10,
        "marginTop": 10,
        "showAxes": False,
        "projectionDir": (0.5, 0.5, 0.5),
        "strokeWidth": 0.25,
        "strokeColor": (255, 0, 0),
        "hiddenColor": (0, 0, 255),
        "showHidden": True,
    },
)

Which results in the following image:

Exporting with the additional option "focus": 25 results in the following output SVG with perspective:

Exporting STL

The STL exporter is capable of adjusting the quality of the resulting mesh, and accepts the following parameters.

Shape.exportStl(fileName: str, tolerance: float = 0.001, angularTolerance: float = 0.1, ascii: bool = False, relative: bool = True, parallel: bool = True) → bool[source]

Exports a shape to a specified STL file.

Parameters

fileName (str) – The path and file name to write the STL output to.
tolerance (float) – A linear deflection setting which limits the distance between a curve and its tessellation. Setting this value too low will result in large meshes that can consume computing resources. Setting the value too high can result in meshes with a level of detail that is too low. Default is 1e-3, which is a good starting point for a range of cases.
angularTolerance (float) – Angular deflection setting which limits the angle between subsequent segments in a polyline. Default is 0.1.
ascii (bool) – Export the file as ASCII (True) or binary (False) STL format. Default is binary.
relative (bool) – If True, tolerance will be scaled by the size of the edge being meshed. Default is True. Setting this value to True may cause large features to become faceted, or small features dense.
parallel (bool) – If True, OCCT will use parallel processing to mesh the shape. Default is True.

Return type

bool

For more complex objects, some experimentation with tolerance and angularTolerance may be required to find the optimum values that will produce an acceptable mesh.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(result, "/path/to/file/mesh.stl")

Exporting AMF and 3MF

The AMF and 3MF exporters are capable of adjusting the quality of the resulting mesh, and accept the following parameters.

fileName - The path and file name to write the AMF output to.
tolerance - A linear deflection setting which limits the distance between a curve and its tessellation. Setting this value too low will result in large meshes that can consume computing resources. Setting the value too high can result in meshes with a level of detail that is too low. Default is 0.1, which is good starting point for a range of cases.
angularTolerance - Angular deflection setting which limits the angle between subsequent segments in a polyline. Default is 0.1.

For more complex objects, some experimentation with tolerance and angularTolerance may be required to find the optimum values that will produce an acceptable mesh. Note that parameters for color and material are absent.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(result, "/path/to/file/mesh.amf", tolerance=0.01, angularTolerance=0.1)

Exporting TJS

The TJS (ThreeJS) exporter produces a file in JSON format that describes a scene for the ThreeJS WebGL renderer. The objects in the first argument are converted into a mesh and then form the ThreeJS geometry for the scene. The mesh can be adjusted with the following parameters.

fileName - The path and file name to write the ThreeJS output to.
tolerance - A linear deflection setting which limits the distance between a curve and its tessellation. Setting this value too low will result in large meshes that can consume computing resources. Setting the value too high can result in meshes with a level of detail that is too low. Default is 0.1, which is good starting point for a range of cases.
angularTolerance - Angular deflection setting which limits the angle between subsequent segments in a polyline. Default is 0.1.

For more complex objects, some experimentation with tolerance and angularTolerance may be required to find the optimum values that will produce an acceptable mesh.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(
    result,
    "/path/to/file/mesh.json",
    tolerance=0.01,
    angularTolerance=0.1,
    exportType=exporters.ExportTypes.TJS,
)

Note that the export type was explicitly specified as TJS because the extension that was used for the file name was .json. If the extension .tjs had been used, CadQuery would have understood to use the TJS export format.

Exporting VRML

The VRML exporter is capable of adjusting the quality of the resulting mesh, and accepts the following parameters.

fileName - The path and file name to write the VRML output to.
tolerance - A linear deflection setting which limits the distance between a curve and its tessellation. Setting this value too low will result in large meshes that can consume computing resources. Setting the value too high can result in meshes with a level of detail that is too low. Default is 0.1, which is good starting point for a range of cases.
angularTolerance - Angular deflection setting which limits the angle between subsequent segments in a polyline. Default is 0.1.

For more complex objects, some experimentation with tolerance and angularTolerance may be required to find the optimum values that will produce an acceptable mesh.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(
    result, "/path/to/file/mesh.vrml", tolerance=0.01, angularTolerance=0.1
)

Exporting DXF

Options

approx

Approximation strategy for converting cadquery.Workplane objects to DXF entities:

None
no approximation applied

"spline"
all splines approximated as cubic splines

"arc"
all curves approximated as arcs and straight segments

tolerance

Approximation tolerance for converting cadquery.Workplane objects to DXF entities. See Approximation strategy.

doc_units

Ezdxf document/modelspace units. See Units.

DXF document without options.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.exportDXF(result, "/path/to/file/object.dxf")
# or
exporters.export(result, "/path/to/file/object.dxf")

Units

The default DXF document units are mm (doc_units = 4).

doc_units	Unit
0	Unitless
1	Inches
2	Feet
3	Miles
4	Millimeters
5	Centimeters
6	Meters

Document units can be set to any unit supported by ezdxf.

DXF document with units set to meters.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.exportDXF(
    result,
    "/path/to/file/object.dxf",
    doc_units=6,  # set DXF document units to meters
)

# or

exporters.export(
    result,
    "/path/to/file/object.dxf",
    opt={"doc_units": 6},  # set DXF document units to meters
)

Approximation strategy

By default, the DXF exporter will output splines exactly as they are represented by the OpenCascade kernel. Unfortunately some software cannot handle higher-order splines resulting in missing curves after DXF import. To resolve this, specify an approximation strategy controlled by the following options:

approx - None, "spline" or "arc". "spline" results in all splines approximated with cubic splines. "arc" results in all curves approximated with arcs and line segments.
tolerance: Acceptable error of the approximation, in document/modelspace units. Defaults to 0.001 (1 thou for inch-scale drawings, 1 µm for mm-scale drawings).

DXF document with curves approximated with cubic splines.

cq.exporters.exportDXF(result, "/path/to/file/object.dxf", approx="spline")

Exporting Other Formats

The remaining export formats do not accept any additional parameters other than file name, and can be exported using the following structure.

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(result, "/path/to/file/object.[file_extension]")

Be sure to use the correct file extension so that CadQuery can determine the export format. If in doubt, fall back to setting the type explicitly by using exporters.ExportTypes.

For example:

import cadquery as cq
from cadquery import exporters

result = cq.Workplane().box(10, 10, 10)

exporters.export(result, "/path/to/file/object.dxf", exporters.ExportTypes.DXF)