topic Re: InternalValidationError when creating construction plane in Fusion API and Scripts Forum

InternalValidationError when creating construction plane

Tim.Overbye — Fri, 04 Feb 2022 03:02:24 GMT

Howdy,

I have a script to generate a half sphere and place holes in its surface randomly. It works fine for the first 10-20 holes then throws an error.

Failed: Traceback (most recent call last): File "C:/Users/Tim/AppData/Roaming/Autodesk/Autodesk Fusion 360/API/Scripts/Star_form/Star_form.py", line 111, in run workplane = rootComp.constructionPlanes.add(workplaneinput) File "C:/Users/Tim/AppData/Local/Autodesk/webdeploy/production/6783e6b71d33852e05099c507cf8d926394ea32c/Api/Python/packages\adsk\fusion.py", line 12795, in add return _fusion.ConstructionPlanes_add(self, input) RuntimeError: 2 : InternalValidationError : data_->execute(&obj, apiName) && obj

I'd appreciate any help, the full code is below.

#Author- #Description- from tkinter.messagebox import NO import adsk.core, adsk.fusion, adsk.cam, traceback import math import random id = 300*0.1 wall_thickness = 2 * 0.1 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 arcs. arc = sketch.sketchCurves.sketchArcs arc1 = arc.addByCenterStartSweep(adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(id/2, 0, 0),math.pi) arc2 = arc.addByCenterStartSweep(adsk.core.Point3D.create(0, 0, 0), adsk.core.Point3D.create(id/2 + wall_thickness, 0, 0),math.pi) # Draw lines to close arcs. lines = sketch.sketchCurves.sketchLines line_1 = lines.addByTwoPoints(adsk.core.Point3D.create(id/2, 0, 0), adsk.core.Point3D.create(id/2 + wall_thickness, 0, 0)) line_2 = lines.addByTwoPoints(adsk.core.Point3D.create(-id/2, 0, 0), adsk.core.Point3D.create(-id/2 - wall_thickness, 0, 0)) # Draw center line to use as the axis of revolution. lines = sketch.sketchCurves.sketchLines axisLine = lines.addByTwoPoints(adsk.core.Point3D.create(-1, 0, 0), adsk.core.Point3D.create(1, 0, 0)) # Get the profile defined by the circle. prof = sketch.profiles.item(0) # Create an revolution input to be able to define the input needed for a revolution # while specifying the profile and that a new body is to be created revolves = rootComp.features.revolveFeatures revInput = revolves.createInput(prof, axisLine, adsk.fusion.FeatureOperations.NewBodyFeatureOperation) # Define that the extent is an angle of pi to get half of a sphere. angle = adsk.core.ValueInput.createByReal(math.pi) revInput.setAngleExtent(False, angle) # Create the extrusion. ext = revolves.add(revInput) body = ext.bodies[0] target_face = None # Create hole on body basesketch = rootComp.sketches.add(rootComp.xYConstructionPlane) basesketch.isVisible = False r = id/2 + wall_thickness # randomply place pt on half sphere for i in range(100): # Get face for face in body.faces: surface = adsk.core.Sphere.cast(face.geometry) if (surface and math.fabs(surface.radius - (id/2 + wall_thickness)) < 1.0e-6 ): target_face = face phi = random.random() * math.pi * 2.0 theta = random.random() * math.pi*0.5 x = r * math.sin(theta) * math.cos(phi) y = r * math.sin(theta) * math.sin(phi) z = r * math.cos(theta) # Create hole based on a point pt = adsk.core.Point3D.create(x, y, z) basesketchpoint = basesketch.sketchPoints.add(pt) if(target_face): # Create plane tangent to sphere workplaneinput = rootComp.constructionPlanes.createInput() workplaneinput.setByTangentAtPoint(target_face, basesketchpoint) workplane = rootComp.constructionPlanes.add(workplaneinput) # Create hole holeinput = rootComp.features.holeFeatures.createSimpleInput(adsk.core.ValueInput.createByString('1 cm')) holeinput.setPositionByPoint(workplane, pt) holeinput.setDistanceExtent(adsk.core.ValueInput.createByReal(10)) rootComp.features.holeFeatures.add(holeinput) # Hide workplane workplane.isLightBulbOn = False except: if ui: ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

Re: InternalValidationError when creating construction plane

kandennti — Fri, 04 Feb 2022 10:05:11 GMT

Hi @Tim.Overbye .

I haven't checked the reason in detail, but it seems that sometimes the sketch point is not on the surface.

I'm sure there are better ways to do this, but you might want to make sure they are on the surface.

・・・ if(target_face): # Check if the point is on the surface. if not isPointOnSurface(target_face, basesketchpoint): continue # Create plane tangent to sphere workplaneinput = rootComp.constructionPlanes.createInput() workplaneinput.setByTangentAtPoint(target_face, basesketchpoint) ・・・ def isPointOnSurface( target_face: adsk.fusion.BRepFace, basesketchpoint: adsk.fusion.SketchPoin, tolerance: float = 0.0001) -> bool: try: app: adsk.core.Application = adsk.core.Application.get() measMgr: adsk.core.MeasureManager = app.measureManager res: adsk.core.MeasureResults = measMgr.measureMinimumDistance( target_face, basesketchpoint ) if res.value > tolerance: return False return True except: return False

Re: InternalValidationError when creating construction plane

Tim.Overbye — Fri, 04 Feb 2022 16:40:51 GMT

Thanks, I tried what you suggested but it didn't solve the problem.

I'm still not sure what the problem was but I got it working by creating all the construction planes in a single batch and then doing all the holes in a separate batch. I think the problem was related to using the object's surface after modifying it.

Re: InternalValidationError when creating construction plane

BrianEkins — Fri, 04 Feb 2022 16:56:30 GMT

I looked into this a bit and believe it is some kind of bug with Fusion. I captured the XYZ coordinates from a failed run and then used those to test with. It consistently failed on the last point, but I can interactively create a construction plane using that point. What's especially weird is if I reordered the last point that failed to any other location in the point set, it was successful.

I would recommend another approach to do what you're doing that should be much faster to process and I think simpler too. You can use the functionality supported by the TemporaryBRep Object. I presented a class on this at Autodesk University a few years ago and that material is available here.

Re: InternalValidationError when creating construction plane

Tim.Overbye — Sat, 05 Feb 2022 04:48:01 GMT

Thanks, I switched to the TemporaryBRep Object approach and everything's working now and significantly faster.