import adsk.core, adsk.fusion, traceback
def run(context):
ui = None
try:
app = adsk.core.Application.get()
ui = app.userInterface
doc = app.documents.add(adsk.core.DocumentTypes.FusionDesignDocumentType)
design = app.activeProduct
# Get the root component of the active design.
rootComp = design.rootComponent
# Create a new sketch on the xy plane.
sketches = rootComp.sketches;
xyPlane = rootComp.xYConstructionPlane
sketch = sketches.add(xyPlane)
# Draw two connected lines.
lines = sketch.sketchCurves.sketchLines;
line1 = lines.addByTwoPoints(adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(3, 1, 0))
line2 = lines.addByTwoPoints(line1.endSketchPoint, adsk.core.Point3D.create(1, 4, 0))
# Draw a rectangle by two points.
recLines = lines.addTwoPointRectangle(adsk.core.Point3D.create(4, 0, 0), adsk.core.Point3D.create(7, 2, 0))
# Use the returned lines to add some constraints.
sketch.geometricConstraints.addHorizontal(recLines.item(0))
sketch.geometricConstraints.addHorizontal(recLines.item(2))
sketch.geometricConstraints.addVertical(recLines.item(1))
sketch.geometricConstraints.addVertical(recLines.item(3))
sketch.sketchDimensions.addDistanceDimension(recLines.item(0).startSketchPoint, recLines.item(0).endSketchPoint,
adsk.fusion.DimensionOrientations.HorizontalDimensionOrientation,
adsk.core.Point3D.create(5.5, -1, 0));
# Draw a rectangle by three points.
recLines = lines.addThreePointRectangle(adsk.core.Point3D.create(8, 0, 0), adsk.core.Point3D.create(11, 1, 0), adsk.core.Point3D.create(9, 3, 0))
# Draw a rectangle by a center point.
recLines = lines.addCenterPointRectangle(adsk.core.Point3D.create(14, 3, 0), adsk.core.Point3D.create(16, 4, 0))
except:
if ui:
ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))
#include <Core/CoreAll.h>
#include <Fusion/FusionAll.h>
using namespace adsk::core;
using namespace adsk::fusion;
Ptr<Application> app;
extern "C" XI_EXPORT bool run(const char* context)
{
app = Application::get();
if (!app)
return false;
Ptr<Documents> documents = app->documents();
if (!documents)
return false;
Ptr<Document> doc = documents->add(DocumentTypes::FusionDesignDocumentType);
if (!doc)
return false;
Ptr<Product> product = app->activeProduct();
if (!product)
return false;
Ptr<Design> design = product;
if (!design)
return false;
// Get the root component of the active design
Ptr<Component> rootComp = design->rootComponent();
if (!rootComp)
return false;
// Create a new sketch on the xy plane.
Ptr<Sketches> sketches = rootComp->sketches();
if (!sketches)
return false;
Ptr<ConstructionPlane> xyPlane = rootComp->xYConstructionPlane();
if (!xyPlane)
return false;
Ptr<Sketch> sketch = sketches->add(xyPlane);
if (!sketch)
return false;
// Draw two connected lines.
Ptr<SketchCurves> sketchCurves = sketch->sketchCurves();
if (!sketchCurves)
return false;
Ptr<SketchLines> sketchLines = sketchCurves->sketchLines();
if (!sketchLines)
return false;
Ptr<SketchLine> line1 = sketchLines->addByTwoPoints(Point3D::create(0, 0, 0), Point3D::create(3, 1, 0));
if (!line1)
return false;
Ptr<SketchLine> line2 = sketchLines->addByTwoPoints(line1->endSketchPoint(), Point3D::create(1, 4, 0));
if (!line2)
return false;
// Draw a rectangle by two points.
Ptr<SketchLineList> recLines =
sketchLines->addTwoPointRectangle(Point3D::create(4, 0, 0), Point3D::create(7, 2, 0));
if (!recLines)
return false;
// Use the returned lines to add some constraints.
Ptr<GeometricConstraints> constraints = sketch->geometricConstraints();
if (!constraints)
return false;
Ptr<HorizontalConstraint> HConstraint = constraints->addHorizontal(recLines->item(0));
if (!HConstraint)
return false;
HConstraint = constraints->addHorizontal(recLines->item(2));
if (!HConstraint)
return false;
Ptr<VerticalConstraint> VConstraint = constraints->addVertical(recLines->item(1));
if (!VConstraint)
return false;
VConstraint = constraints->addVertical(recLines->item(3));
if (!VConstraint)
return false;
Ptr<SketchDimensions> sketchDimensions = sketch->sketchDimensions();
if (!sketchDimensions)
return false;
Ptr<SketchDimension> sketchDimension = sketchDimensions->addDistanceDimension(
recLines->item(0)->startSketchPoint(),
recLines->item(0)->endSketchPoint(),
HorizontalDimensionOrientation,
Point3D::create(5.5, -1, 0));
if (!sketchDimension)
return false;
// Draw a rectangle by three points.
recLines = sketchLines->addThreePointRectangle(
Point3D::create(8, 0, 0), Point3D::create(11, 1, 0), Point3D::create(9, 3, 0));
if (!recLines)
return false;
// Draw a rectangle by a center point.
recLines = sketchLines->addCenterPointRectangle(Point3D::create(14, 3, 0), Point3D::create(16, 4, 0));
if (!recLines)
return false;
return true;
}
/**
* API Sample that demonstrates creating sketch lines in various ways.
* Demonstrates several ways to create sketch lines, including as the result of creating a rectangle.
*/
import { adsk } from '@adsk/fusion';
// Params
// {
// "useCurrentDocument": false,
// "saveAsNewDocument": false,
// "message": "",
// "hubId": "wip1fqaautodesk4298",
// "fileURN": "urn:adsk.wipqa:dm.lineage:WlSCDh7RQN6zD2btrrO4SA"
// }
function run() {
// Read the parameters passed with the script
const scriptParameters = JSON.parse(adsk.parameters);
if (!scriptParameters) throw Error("Invalid parameters provided.");
// Get the Fusion API's application object
const app = adsk.core.Application.get();
if (!app) throw Error("No adsk.core.Application.");
// Create a new empty document
const doc = getDocument(
app,
scriptParameters.useCurrentDocument,
scriptParameters.hubId,
scriptParameters.fileURN,
);
if (!doc) throw Error("Invalid document.");
// Ensure we are in the Design environment.
const design = app.activeProduct as adsk.fusion.Design;
//Get the root component of the active design.
const rootComp = design.rootComponent
// Create a new sketch on the xy plane.
const sketches = rootComp.sketches
const xyPlane = rootComp.xYConstructionPlane
const sketch = sketches.add(xyPlane)
//Draw two connected lines.
const lines = sketch.sketchCurves.sketchLines;
const line1 = lines.addByTwoPoints(adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(3, 1, 0))
const line2 = lines.addByTwoPoints(line1.endSketchPoint, adsk.core.Point3D.create(1, 4, 0))
// Draw a rectangle by two points.
const recLinesTwoPoints = lines.addTwoPointRectangle(adsk.core.Point3D.create(4, 0, 0), adsk.core.Point3D.create(7, 2, 0))
// Use the returned lines to add some constraints.
sketch.geometricConstraints.addHorizontal(recLinesTwoPoints.item(0))
sketch.geometricConstraints.addHorizontal(recLinesTwoPoints.item(2))
sketch.geometricConstraints.addVertical(recLinesTwoPoints.item(1))
sketch.geometricConstraints.addVertical(recLinesTwoPoints.item(3))
sketch.sketchDimensions.addDistanceDimension(recLinesTwoPoints.item(0).startSketchPoint, recLinesTwoPoints.item(0).endSketchPoint,
adsk.fusion.DimensionOrientations.HorizontalDimensionOrientation,
adsk.core.Point3D.create(5.5, -1, 0))
// Draw a rectangle by three points.
const recLinesThreePoints = lines.addThreePointRectangle(adsk.core.Point3D.create(8, 0, 0), adsk.core.Point3D.create(11, 1, 0), adsk.core.Point3D.create(9, 3, 0))
// Draw a rectangle by a center point.
const recLinesCenterPoint = lines.addCenterPointRectangle(adsk.core.Point3D.create(14, 3, 0), adsk.core.Point3D.create(16, 4, 0))
saveDocument(
doc,
scriptParameters.saveAsNewDocument,
scriptParameters.message,
doc.dataFile.parentFolder,
);
while (app.hasActiveJobs) {
wait(2000);
}
}
function wait(ms: number) {
const start = new Date().getTime();
while (new Date().getTime() - start < ms) adsk.doEvents();
}
function getDocument(
app: adsk.core.Application,
useCurrentDocument: boolean,
hubId: string,
fileURN: string,
): adsk.core.Document {
if (useCurrentDocument === true) {
adsk.log(`Using currently open document: ${app.activeDocument.name}.`);
return app.activeDocument;
}
if (hubId) {
// Possible hubId formats: base64 encoded string, or business:<id>,
// or personal:<id> (deprecated)
const hub =
app.data.dataHubs.itemById(hubId) ||
app.data.dataHubs.itemById(`a.${adsk.btoa(`business:${hubId}`, true)}`) ||
app.data.dataHubs.itemById(`a.${adsk.btoa(`personal:${hubId}`, true)}`);
if (!hub) throw Error(`Hub with id ${hubId} not found.`);
adsk.log(`Setting hub: ${hub.name}.`);
app.data.activeHub = hub;
}
const file = app.data.findFileById(fileURN);
if (!file) throw Error(`File not found ${fileURN}.`);
adsk.log(`Opening ${file.name}`);
const document = app.documents.open(file, true);
if (!document) throw Error(`Cannot open file ${file.name}.`);
return document;
}
function saveDocument(
doc: adsk.core.Document,
saveAsNewDocument: boolean,
message: string,
destinationFolder: adsk.core.DataFolder,
): boolean {
if (saveAsNewDocument) {
adsk.log("Saving as new document.");
try {
destinationFolder.parentProject;
} catch (e) {
adsk.log(
"Destination folder is not in a project, setting folder to Fusion Automation Service project.",
);
destinationFolder = defaultFolder(
doc.parent,
"Fusion Automation Service",
);
}
if (
doc.saveAs(doc.name + " Additive Ready", destinationFolder, message, "")
) {
adsk.log("Document saved successfully.");
return true;
} else {
adsk.log("Document failed to save.");
return false;
}
}
if (!doc.isModified) {
adsk.log("Document not modified, not saving.");
return true;
}
adsk.log(`Saving with message: "${message}".`);
if (doc.save(message)) {
adsk.log("Document saved successfully.");
return true;
} else {
adsk.log("Document failed to save.");
return false;
}
}
function defaultFolder(app: adsk.core.Application, defaultProjectName: string) {
const projects = app.data.activeHub.dataProjects;
if (!projects) throw Error("Unable to get active hub's projects.");
for (let i = 0; i < projects.count; ++i) {
const project = projects.item(i)!;
if (project.name === defaultProjectName) {
return project.rootFolder;
}
}
adsk.log(`Creating new project: ${defaultProjectName}`);
const project = projects.add(defaultProjectName);
if (!project) throw Error("Unable to create new project.");
return project.rootFolder;
}
run();