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In PlanarSketch, I wish to create a fillet between two touching sketch lines. Errors out!!!
Code is:
Dim startWorkPoint As WorkPoint = m_compDef.WorkPoints.AddFixed(newStartPoint, True)
Dim pathSketch As PlanarSketch = pathSketchCurve.Parent
Dim pathSketchLine As SketchLine = pathSketchCurve
Dim skpt1 As SketchPoint = pathSketch.AddByProjectingEntity(startWorkPoint)
Dim addedSketchLine As SketchLine = pathSketch.SketchLines.AddByTwoPoints(skpt1, pathSketchLine.StartSketchPoint)
Dim skarc As SketchArc = pathSketch.SketchArcs.AddByFillet(addedSketchLine, pathSketchLine, m_bendradius, addedSketchLine.EndSketchPoint.Geometry, pathSketchLine.StartSketchPoint.Geometry)
Dim path As Inventor.Path = m_compDef.Features.CreatePath(addedSketchLine)
Dim profile As Profile = profileSketch.Profiles.AddForSolid
CreateNewSweep(profile, path, PartFeatureOperationEnum.kJoinOperation)In interactive mode, 'pathSketchLine' is somehow not selectable, although its part of the same sketch.
Attached is the full file.
Any clue?
Solved! Go to Solution.
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Hi Yogesh,
Can you please share the sample file for me to understand the model ?
If you cannot select the path for fillet in Inventor UI, it is unlikely that the API can use it too.
But i would like to try it with your sample file.
Regards,
Balaji
Balaji
Developer Technical Services
Autodesk Developer Network
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I have kept project zip at https://drive.google.com/file/d/0B9ZSXyeZHd37dm56bm1wQ2ZTdHM/view?usp=sharing (password is your first name)
In this project I am trying to create Extrude/Sweep features equivalanet to given Sheet Metal features like FACE and CONTOUR FLANGE.
Please execute the project, open "My Project/FaceWithaFlange.ipt" and set break point in "ConvertContourFlangeToSweepOfEdgeWidthExtent()". Here I am trying to build two sketches, one for profile and one for path.
In case of Path I am not able to create arc between two sketch lines. Please uncomment the following line in code to see the error.
'Dim skarc As SketchArc = pathSketch.SketchArcs.AddByFillet(addedSketchLine, pathSketchLine, m_bendradius, addedSketchLine.EndSketchPoint.Geometry, pathSketchLine.StartSketchPoint.Geometry)
I wish to have arcs at every corners to achieve Bend like shape.
Not sure whats going wrong.
(Note: Please preserve this project, as I have quite a few queries on the same. Thanks)
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I tried convertting path sketch to sketch3d and use AddAsBend, but that did not work either. Attached is the file.
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Hi Yogesh,
I have downloaded the sample project and looking into it.
It is quite interesting to see the sheet metal features getting recreated ![]()
I am working on this and will get back to you soon.
Regards,
Balaji
Balaji
Developer Technical Services
Autodesk Developer Network
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Hi Yogesh,
Can you please try this change ?
Dim skarc As SketchArc = pathSketch.SketchArcs.AddByFillet(addedSketchLine, pathSketchLine, m_bendradius, addedSketchLine.StartSketchPoint.Geometry, pathSketchLine.EndSketchPoint.Geometry)
Regards,
Balaji
Balaji
Developer Technical Services
Autodesk Developer Network
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That worked fine!!...Thanks a lot.
After creating this arc, it was erroring out in Sweep creation. I guess it did not have sufficient space to create the arc. So moved back the profile little more as below:
Private Sub ConvertContourFlangeToSweepOfEdgeWidthExtent(ByRef fcd As MyFaceData, ByRef pathSketchCurve As SketchEntity)
Dim profileSketch As PlanarSketch = Nothing
' Need to shift m_boundaryPoints along -ve normal then create sketch out of it
Dim normal As Vector = fcd.m_normal
normal.ScaleBy(-2 * m_bendradius)
Then Sweep got created fine.
One more query in the aspect. Actually, I want a separate body for this feature, so wish to give kNewBodyOperation, but errors out. So I am forced to use kJoinOperation. Any clues?
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Glad you have got it working.
The sweep creation had also worked ok in Inventor 2016 without having to scale down the normal.
About using the "kNewBodyOperation", this is a behavior for which we have a request logged with our engineering team.
This was specific to a sheet metal document and unfortunately I do not have workaround for it.
Sorry about that.
The internal case notes from that request suggests that our QA have confirmed the behavior and is likely to get fixed in a future version of Inventor.
Regards,
Balaji
Balaji
Developer Technical Services
Autodesk Developer Network
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