Need help with iLogic Holes - Pattern
I opened the part that was originally posted. A sketch with a circular pattern of center points being used by the Hole feature. The model parameter that is being used as the quantity of the sketch pattern is the "QTY_Holes" parameter. When I suppress both local iLogic rules, then I can change that parameter's value manually, and see the quantity of holes changing in the model. However, the problem is that these parameter changes are changing the sketch pattern OK, but the hole feature is not updating its 'positions' properly. It seems a bit random, if it will update properly. And after changing the parameter's value, I am not seeing the 'update' tool highlight, which would indicate that it needs to be updated to see the changes. I also tried clicking the Manage tab > Rebuild All tool, but that does not appear to fix the hole feature's positions either. I can tell that what needs to happen is to get the hole feature and modify its HoleFeature.HoleCenterPoints, or something similar, to force it to update properly after the parameter change.
Wesley Crihfield
(Not an Autodesk Employee)
That might work out better for you in a configuration/automation type situation. However, I came up with an additional iLogic rule that seems to be working for this situation. This iLogic rule is set-up to be triggered to run when the value of that parameter changes. Then it gets the Part document. Then updates it. Then gets the sketch that the hole feature is based on. Gathers all center points within it into a collection. Then gets the hole feature, and sets the collection of center points to it, as mentioned in my earlier post. Check this out on your end and see if it will work for you. (I was testing it while I had your other two local iLogic rules suppressed.)
Again, this would be in its own local iLogic rule. Probably after the other two.
oTrigger = QTY_Holes
Dim oPDoc As PartDocument = ThisDoc.Document
oPDoc.Update
oSketch = oPDoc.ComponentDefinition.Sketches.Item("Sketch4")
Dim oCPoints As ObjectCollection = ThisApplication.TransientObjects.CreateObjectCollection
For Each oSPoint As SketchPoint In oSketch.SketchPoints
If oSPoint.HoleCenter Then
oCPoints.Add(oSPoint)
End If
Next
'MsgBox("There are now " & oCPoints.Count & " center points in the sketch.",,"")
oHoleFeat = oPDoc.ComponentDefinition.Features.HoleFeatures.Item("Hole1")
Dim oHDef As SketchHolePlacementDefinition = oHoleFeat.PlacementDefinition
oHDef.HoleCenterPoints = oCPoints
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Wesley Crihfield
(Not an Autodesk Employee)
It seems to me like it might make a slight difference in your drawing annotations, which way you produce those holes. For instance, if you use the 'Hole and Thread' tool on the 'Feature Notes' panel of the 'Annotate' tab of a drawing to call out the holes. If I'm remembering correctly, when you create all the holes in one hole feature, the quantity in that hole note will come out correct, but I can't remember if doing the holes by patterning one hole feature messes that up. Either way, if the quantity note isn't right, it's just a minor irritation which is quickly fixable.
Wesley Crihfield
(Not an Autodesk Employee)
