Suppress a feature in Model in Drawing

[tmathieson]

Hello All,

hope everyone is doing alright.  i am working on a ilogic rule for creating a drawing package, and it is coming along quite well.  i am having one issue where i want to suppress some features in the view model based on certain criteria.  my issue is i can't figure out how to get the feature suppress. i can update parameters OK, but this is giving me issues. i keep getting an error on the  'hole_suppress.Add' line...

"Error on Line 186 : Argument not specified for parameter 'Index' of 'Public ReadOnly Default Property Item(Index As Object) As Inventor.PartFeature'. "

			
			Dim oPartDef_FORM As PartComponentDefinition
			oPartDef_FORM = oModel_formed.ComponentDefinition
			oBaseView_FORMED = NewSheet.DrawingViews.AddBaseView(oModel_formed, oPoint3, 1 / 30, ktopViewOrientation, kHiddenLineRemovedDrawingViewStyle, , , oBaseViewOptions)
			oBaseView_FORMED.RotateByAngle(PI)
			'
			' NOW PASS PARAMETERS TO FORMED PART
			'
			oPart_F = oBaseView_FORMED.ReferencedDocumentDescriptor.ReferencedDocument
			propSet = oPart_F.PropertySets.Item("Inventor User Defined Properties")
			oPartDef_FORM.Parameters.Item("CROWN_RADIUS").Value = c_rad_1
			oPartDef_FORM.Parameters.Item("INSIDE_RADIUS").Value = H_RAD_1 
			oPartDef_FORM.Parameters.Item("PITCH").Value=PITCH_V 
			oPartDef_FORM.Parameters.Item("NUMB_S_HAUNCH").Value=H_RAD_H 
			oPartDef_FORM.Parameters.Item("NUMB_S").Value=TOT_S 
			oPartDef_FORM.Parameters.Item("DEPTH").Value=DEPTH_V 
			oPartDef_FORM.Parameters.Item("CIRC_HOLE_SP").Value=CIR_HOLE_SP_V
			oPartDef_FORM.Parameters.Item("FLAT_SPOT").Value=FLAT_SPOT_V
			oPartDef_FORM.Parameters.Item("LEG_S").Value=LEG_S_V 
			oPartDef_FORM.Parameters.Item("LEG").Value = LEG_LENGTH_V
			oPartDef_FORM.Parameters.Item("THICKNESS").Value = THICKNESS_V
			Dim hole_suppress As ObjectCollection
			hole_suppress.Add oPartDef_FORM.Features.Item.Name("HAUNCH_SIDE_HOLES")
			If LEG_S_V <= 1 Then
			    oPartDef_FORM.SuppressFeatures(hole_suppress)
			End If

 as always, any help/insight is greatly appreciated!

[Andrii_Humeniuk · Accepted solution]

Hi @tmathieson . Please check if it works as you wanted.

Dim oPartDef_FORM As PartComponentDefinition
oPartDef_FORM = oModel_formed.ComponentDefinition
oBaseView_FORMED = NewSheet.DrawingViews.AddBaseView(oModel_formed, oPoint3, 1 / 30, ktopViewOrientation, kHiddenLineRemovedDrawingViewStyle, , , oBaseViewOptions)
oBaseView_FORMED.RotateByAngle(PI)
'
' NOW PASS PARAMETERS TO FORMED PART
'
oPart_F = oBaseView_FORMED.ReferencedDocumentDescriptor.ReferencedDocument
propSet = oPart_F.PropertySets.Item("Inventor User Defined Properties")
oPartDef_FORM.Parameters.Item("CROWN_RADIUS").Value = c_rad_1
oPartDef_FORM.Parameters.Item("INSIDE_RADIUS").Value = H_RAD_1 
oPartDef_FORM.Parameters.Item("PITCH").Value=PITCH_V 
oPartDef_FORM.Parameters.Item("NUMB_S_HAUNCH").Value=H_RAD_H 
oPartDef_FORM.Parameters.Item("NUMB_S").Value=TOT_S 
oPartDef_FORM.Parameters.Item("DEPTH").Value=DEPTH_V 
oPartDef_FORM.Parameters.Item("CIRC_HOLE_SP").Value=CIR_HOLE_SP_V
oPartDef_FORM.Parameters.Item("FLAT_SPOT").Value=FLAT_SPOT_V
oPartDef_FORM.Parameters.Item("LEG_S").Value=LEG_S_V 
oPartDef_FORM.Parameters.Item("LEG").Value = LEG_LENGTH_V
oPartDef_FORM.Parameters.Item("THICKNESS").Value = THICKNESS_V
For Each oFeat As PartFeature In oPartDef_FORM.Features
	If oFeat.Name.Contains("HAUNCH_SIDE_HOLES") Then
		oFeat.Suppressed = True
	End If
Next

[WCrihfield · Accepted solution]

I don't know what version of Inventor you may have, but this sounds like a good place to use multiple ModelStates in the part with different parameter values & feature suppression statuses in each one, then simply switch which ModelState the view is set to, instead of trying to control all of those different aspects of the model backwards from the drawing.  Just looking at the situation from a different perspective...perhaps without all of the needed design intent knowledge.

[tmathieson]

thanks @Andrii_Humeniuk  !!

just what I needed!

works great!  thanks again!

[tmathieson]

Morning @WCrihfield .  thanks for the suggestion on model states.  for this particular task, there is only one set of holes that are suppress or not suppressed, so @Andrii_Humeniuk  code works fine in this case.  i have used model states in other projects, but have been bitten by them a couple times as shown in the attached picture. so i've been shying away from them, but still use them, but with caution.

thanks, and a have a good one!!