topic Re: fusion api sketches lines in Fusion API and Scripts Forum

fusion api sketches lines

grosfaignan — Wed, 06 Jul 2022 18:57:32 GMT

hi there, i need to create some lines in python scripts, then add them length and then add them dimension (placement) from origin, how can i do that ?

thanks

Re: fusion api sketches lines

Rushikesh.kadam — Thu, 07 Jul 2022 07:19:57 GMT

@grosfaignan here are some sample links that demonstrate creating sketch lines and adding sketch dimensions.

Here is another link explaining the sketch dimensions object https://help.autodesk.com/view/fusion360/ENU/?guid=GUID-GUID-ea0faa88-65eb-4845-b2ce-22d0640bedf4 .Under the topic Samples, there few more examples related to dimension.

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Re: fusion api sketches lines

Jorge_Jaramillo — Thu, 07 Jul 2022 16:25:46 GMT

Hi @grosfaignan ,

Here you have a fragment of python code to create sketch lines and dimension one of them with a user parameter:

app: adsk.core.Application = adsk.core.Application.get() DISTANCE_PARAMETER = 'distance' design = adsk.fusion.Design.cast(app.activeProduct) # 1) user parameter distParam = design.userParameters.itemByName(DISTANCE_PARAMETER) if not distParam: # create user parameter if not found distVal = adsk.core.ValueInput.createByString('35 mm') distParam = design.userParameters.add(DISTANCE_PARAMETER, distVal, 'mm', '') # 2) sketch rootComp = adsk.fusion.Component.cast(design.rootComponent) # Create a new sketch on the xy plane. sketches = rootComp.sketches sketch = sketches.itemByName('xySketch') sketch.areDimensionsShown = True #display dimensions on the sketch if not sketch: # create sketch if not found xyPlane = rootComp.xYConstructionPlane sketch = adsk.fusion.Sketch.cast(sketches.add(xyPlane)) sketch.name = 'xySketch' # 3) create sketch points p1 = sketch.sketchPoints.add(adsk.core.Point3D.create(1, 0, 0)) p2 = sketch.sketchPoints.add(adsk.core.Point3D.create(3, 1, 0)) # 4) create 2 lines, sharing p1 as a coincident constraint line1 = sketch.sketchCurves.sketchLines.addByTwoPoints(sketch.originPoint, p1) line2 = sketch.sketchCurves.sketchLines.addByTwoPoints(p1, p2) # 5) add dimension to line1 sld = sketch.sketchDimensions.addDistanceDimension(sketch.originPoint, p1, adsk.fusion.DimensionOrientations.AlignedDimensionOrientation, adsk.core.Point3D.create(0, 2, 0)) # 6) get model parameter from the sketch dimension and assign a user parameter to its expression modelParam = adsk.fusion.ModelParameter.cast(sld.parameter) modelParam.expression = DISTANCE_PARAMETER

This is the result:

Hope it helps.

Let me know if it works for you.

Regards,

Jorge

Re: fusion api sketches lines

Jorge_Jaramillo — Thu, 07 Jul 2022 16:30:23 GMT

Please correct in the previous code, moving this line :
sketch.areDimensionsShown = True
after
sketch.name = 'xySketch'.
Sorry!!.