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Hope you all are having a great day.
Does anyone here know if it would be possible to use iLogic or other means to build an addon that will find the bend line on a flat pattern and add two holes to it (one on each end)?
The way our CNC machine picks up our centerpunch is we add a .125" hole on the part. I spends hours opening flat patterns , creating a sketch, projecting the bend lines, adding a point usually .100" away from the edge, then using the hole feature to create the .125" hole.
Example part attached.
We would probably pay money for it if anyone knows of something existing.
Am I just dreaming here?
Thanks
Chris
Hi chrisw01a,
I think it can be done, based off a quick look at the API. I suspect we could do it with an ilogic rule, but I don't have the time to look into it at the moment.
See this link for a similar example:
You might post on the Inventor Customization forum:
http://forums.autodesk.com/t5/Autodesk-Inventor-Customization/bd-p/120
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
On second glance I don't think this will take too long, I'll try and come up with something here in a bit.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Hi @chrisw01a,
Okay here's a quick iLogic rule that creates a sketch on the top face of the flat pattern and then places holes on the ends of each bend (up and down).
I'd set this up as an external rule, although the attached 2017 file has it set up as an external rule.
I didn't test this much, so you're likely to run across some issues. If so post back.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
'[ edit these variables as needed
sSketchName = "Flat Pattern Sketch"
sHoleName = "Locator Holes"
oOffset = 0.100 in'defines offset from edge of flat pattern
oDiameter = 0.125 in 'defines hole diameter
']
' a reference to the active document.
Dim oPartDoc As PartDocument
oPartDoc = ThisApplication.ActiveDocument
'verify document type is sheet metal
If oPartDoc.ComponentDefinition.Type <> 150995200 Then
MessageBox.Show("File is not a sheet metal part.", "iLogic")
Exit Sub
End If
Dim oCompDef As SheetMetalComponentDefinition
oCompDef = oPartDoc.ComponentDefinition
' Check to make sure a flat pattern is open.
If Not TypeOf ThisApplication.ActiveEditObject Is FlatPattern Then
Try
If oCompDef.HasFlatPattern = False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Catch
MessageBox.Show("Error editting the flat pattern.", "iLogic")
End Try
End If
' a reference to the active flat pattern.
Dim oFlatPattern As FlatPattern
oFlatPattern = ThisApplication.ActiveEditObject
'clean up existing holes
Dim oHole As HoleFeature
For Each oHole In oFlatPattern.Features.HoleFeatures
oHole.Delete
Next
Dim oFace As Face
oFace = oFlatPattern.TopFace
Dim oSketch As PlanarSketch
'clean up existing sketch
For Each oSketch In oFlatPattern.Sketches
If oSketch.Name = sSketchName Then
oSketch.Delete
End If
Next
' Create a new sketch. The second argument specifies to include/not include
' the edges of the face in the sketch.
oSketch = oFlatPattern.Sketches.Add(oFace, False)
' Change the name.
oSketch.Name = sSketchName
' Create a new object collection for the hole center points.
oHoleCenters = ThisApplication.TransientObjects.CreateObjectCollection
Dim oTG As TransientGeometry
oTG = ThisApplication.TransientGeometry
Dim oPoint As Point2d
Dim oEdge As Edge
oOffset = oOffset * 2.5400013716 'converts cm to inches
' Get all Bend UP edges on top face
Dim oTopFaceBendUpEdges As Edges
oTopFaceBendUpEdges = _
oFlatPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendUpFlatPatternEdge, True)
For Each oEdge In oTopFaceBendUpEdges
oPoint = oTG.CreatePoint2d(oEdge.StartVertex.Point.x, oEdge.StartVertex.Point.Y - oOffset)
oHoleCenters.Add ( oSketch.SketchPoints.Add(oPoint, True))
oPoint = oTG.CreatePoint2d(oEdge.StopVertex.Point.x, oEdge.StopVertex.Point.Y + oOffset)
oHoleCenters.Add ( oSketch.SketchPoints.Add(oPoint, True))
Next
' Get all Bend DOWN edges on top face
Dim oTopFaceBendDownEdges As Edges
oTopFaceBendDownEdges = _
oFlatPattern.GetEdgesOfType(FlatPatternEdgeTypeEnum.kBendDownFlatPatternEdge, True)
For Each oEdge In oTopFaceBendDownEdges
oPoint = oTG.CreatePoint2d(oEdge.StartVertex.Point.x, oEdge.StartVertex.Point.Y - oOffset)
oHoleCenters.Add ( oSketch.SketchPoints.Add(oPoint, True))
oPoint = oTG.CreatePoint2d(oEdge.StopVertex.Point.x, oEdge.StopVertex.Point.Y + oOffset)
oHoleCenters.Add ( oSketch.SketchPoints.Add(oPoint, True))
Next
' Create the hole feature.
oHole = oFlatPattern.Features.HoleFeatures.AddDrilledByThroughAllExtent( _
oHoleCenters, oDiameter * 2.5400013716 , kPositiveExtentDirection)
oHole.Name = sHoleName
Hi chrisw01a & karthur1,
I caught this issue after posting yesterday, but wasn't able to determine what the issue was, so I posted a question concerning this on the Inventor Customization Forum, here:
I see a response on that thread, but haven't had time to look into it just yet. But I'll try to do so at some point today.
I'll post back to this thread when I've had a chance look at this again.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Hi chrisw01a,
I'm still not having much luck with offsetting the holes predictably, but the attached version does behave more predictably in placing them. It's just that it lays them right on the part edges.
I don't suppose adding the holes on the edges is acceptable?
In any case I'll look at this again when I can, to see if I can determine how to do the offsetting predictably.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
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