topic Re: Create centerpoint rectangles from sketch centers in Fusion API and Scripts Forum

Create centerpoint rectangles from sketch centers

Anonymous — Fri, 22 Jan 2021 20:19:28 GMT

Hey there -

New to Fusion scripting, and I am 90% sure I am getting tangled up in object types, but thought this would be a good place to start.

I wrote a script already that imports a pile of DXF files separately. Now, what I would like to do is create a rectangle of fixed size around the *individual sketch* origin, not the origin of the entire project.

I am having 2 issues:

1) I can't create another point translated from the first for some reason

2) Trying to retrieve the origin of the sketch is proving to be difficult - I keep getting the global origin, *not* the origin on the sketch. I have a demo file attached, and code is below. Thanks for the help!

import traceback import adsk.core import adsk.fusion def run(context): ui = None try: app = adsk.core.Application.get() ui = app.userInterface design = app.activeProduct cornerTrans = adsk.core.Vector3D.create(24, 24, 0) # Get the sketch out of the root component of the active design. rootComp = design.rootComponent sketches = rootComp.sketches; sketch = sketches[0] wO = sketch.origin xzPlane = rootComp.xZConstructionPlane sketchNew = sketches.add(xzPlane) sketchPoints = sketchNew.sketchPoints lines = sketchNew.sketchCurves.sketchLines; workOrigin = sketchPoints.add(wO) rC = wO.translateBy(cornerTrans) recCorner = sketchPoints.add(rC) recLines = lines.addCenterPointRectangle(workOrigin, recCorner) except: if ui: ui.messageBox('Failed:\n{}'.format(traceback.format_exc()))

Re: Create centerpoint rectangles from sketch centers

kandennti — Sat, 23 Jan 2021 13:48:48 GMT

Hi @Anonymous .

It is possible that I am not understanding what you want.

The translateBy method of the Point3D object is a destructive method that changes the calling instance itself.

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-29830e60-05c0-4c88-8ef7-2bfe7af6bcc1

The first parameter of the addCenterPointRectangle method is the Point3D object.

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-cdc75402-9c1c-4134-bd01-e95eb9c9b8ee

So if you do it this way, the error will no longer

・・・ sketchPoints = sketchNew.sketchPoints lines = sketchNew.sketchCurves.sketchLines; workOrigin = sketchPoints.add(wO) # rC = wO.translateBy(cornerTrans) rC = wO.copy() rC.translateBy(cornerTrans) recCorner = sketchPoints.add(rC) # recLines = lines.addCenterPointRectangle(workOrigin, recCorner) recLines = lines.addCenterPointRectangle(workOrigin.geometry, recCorner) ・・・

Re: Create centerpoint rectangles from sketch centers

Anonymous — Sun, 24 Jan 2021 02:24:17 GMT

Thank you for this help! I will check it out on Monday and report back. I think at the least this will solve one of the issues.

Re: Create centerpoint rectangles from sketch centers

Anonymous — Mon, 25 Jan 2021 17:54:22 GMT

This definitely got a step closer, but is not quite what I am looking for. Here is the goal that I am aiming for:

If I select an imported DXF sketch in Fusion that is off the part origin:

...and then hit "Create sketch"...

I am given a sketch plane where its local origin corresponds to the center of the previously selected sketch. If I draw from that point, I can create fully defined sketches:

...the long goal here being I am trying to automate a very repetitive CAM process by importing a bunch of DXFs from a folder, create a center rectangle representing the stock, and then automatically create CAM profile data and export a pile of NC code.

Does that make a bit more sense?

Re: Create centerpoint rectangles from sketch centers

kandennti — Tue, 26 Jan 2021 01:32:34 GMT

@Anonymous .

In this case, if you don't have this problem, I think it is easy to use BoundingBox3D.

https://modthemachine.typepad.com/my_weblog/2017/06/getting-the-overall-size-of-parts.html

https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-9ce5053e-72b6-4a47-8172-e4223fb4caff

Although there is not enough processing, we have created such a sample.

#Fusion360API Python script import traceback import adsk.core import adsk.fusion _app = adsk.core.Application.cast(None) _ui = adsk.core.UserInterface.cast(None) def run(context): try: global _app, _ui _app = adsk.core.Application.get() _ui = _app.userInterface des :adsk.fusion.Design = _app.activeProduct root :adsk.fusion.Component = des.rootComponent # create Bounding BoxSketch # Default modeling orientation "Y up" only createBoundingBoxSketch(root.sketches[0],root.xZConstructionPlane) except: if _ui: _ui.messageBox('Failed:\n{}'.format(traceback.format_exc())) def createBoundingBoxSketch( targetSkt :adsk.fusion.Sketch, supportPlane :adsk.core.Base = None ) -> adsk.fusion.Sketch: # check profile if targetSkt.profiles.count < 1: return None # create new sketch comp :adsk.fusion.Component = targetSkt.parentComponent skt = adsk.fusion.Sketch.cast(None) if supportPlane: skt = comp.sketches.add(supportPlane) else: skt = comp.sketches.add(targetSkt.referencePlane) # get boundingBox prof :adsk.fusion.Profile bound :adsk.core.BoundingBox3D = targetSkt.profiles[0].boundingBox for prof in targetSkt.profiles: bound.combine(prof.boundingBox) # get min/max point minPnt :adsk.core.Point3D = bound.minPoint maxPnt :adsk.core.Point3D = bound.maxPoint # get mid point midPnt :adsk.core.Point3D = adsk.core.Point3D.create( (maxPnt.x + minPnt.x) * 0.5, (maxPnt.y + minPnt.y) * 0.5, (maxPnt.z + minPnt.z) * 0.5) # create boundingBox lines = skt.sketchCurves.sketchLines lines.addCenterPointRectangle(midPnt, maxPnt) skt.name = f'BoundingBox of {targetSkt.name}' return skt

~~However, you need to set "Y up" in the Fusion360 preferences to get the correct result.~~

Isn't the attached f3d file created with "Y up"?

Re: Create centerpoint rectangles from sketch centers

Anonymous — Tue, 26 Jan 2021 18:58:19 GMT

This is great! Yes, this was the enabling bit to get my code to work. Posting here for a little more help in case anyone else needs this. Essentially, I have updated this to iterate through all available sketches, create a fixed size bounding box, and place a point at the lower left bounding box corner to help automate CAM setup creation.

Thank you!!

#Author-S. Cusack #Description-CORE: Create Setup CAM Boundaries #Units are in *CM*, thus the weird scale factors import traceback import adsk.core import adsk.fusion _app = adsk.core.Application.cast(None) _ui = adsk.core.UserInterface.cast(None) def run(context): try: global _app, _ui _app = adsk.core.Application.get() _ui = _app.userInterface des :adsk.fusion.Design = _app.activeProduct root :adsk.fusion.Component = des.rootComponent # Get number of existing sketches sketchLen = root.sketches.count i = 0 # create Bounding BoxSketch # Default modeling orientation "Y up" only while i < sketchLen: createBoundingBoxSketch(root.sketches[i],root.xZConstructionPlane) i += 1 except: if _ui: _ui.messageBox('Failed:\n{}'.format(traceback.format_exc())) def createBoundingBoxSketch( targetSkt :adsk.fusion.Sketch, supportPlane :adsk.core.Base = None ) -> adsk.fusion.Sketch: # check profile if targetSkt.profiles.count < 1: return None # create new sketch comp :adsk.fusion.Component = targetSkt.parentComponent skt = adsk.fusion.Sketch.cast(None) if supportPlane: skt = comp.sketches.add(supportPlane) else: skt = comp.sketches.add(targetSkt.referencePlane) # create sizing vector cornerTrans = adsk.core.Vector3D.create(60.96, 60.96, 0) cT2 = cornerTrans.copy() cT2.scaleBy(-2) # get boundingBox prof :adsk.fusion.Profile bound :adsk.core.BoundingBox3D = targetSkt.profiles[0].boundingBox for prof in targetSkt.profiles: bound.combine(prof.boundingBox) # get min/max point minPnt :adsk.core.Point3D = bound.minPoint maxPnt :adsk.core.Point3D = bound.maxPoint # get mid point midPnt :adsk.core.Point3D = adsk.core.Point3D.create( (maxPnt.x + minPnt.x) * 0.5, (maxPnt.y + minPnt.y) * 0.5, (maxPnt.z + minPnt.z) * 0.5) # translate midpoint to exterior corner rC = midPnt.copy() rC.translateBy(cornerTrans) # create boundingBox lines = skt.sketchCurves.sketchLines lines.addCenterPointRectangle(midPnt, rC) # create boundary corner rC.translateBy(cT2) sketchPoints = skt.sketchPoints sketchPoints.add(rC) skt.name = f'Boundary for {targetSkt.name}' return skt