I have a long model tree. In the Fx (Parameter dialog) I can see tons of d## numbers. I see one of it as d136. I want to know where in the model its used.
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Hi CAD-One,
I have a rough iLogic rule to do this, but it's a bit buggy. If I have time to clean it up, would iLogic work for you?
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
I tried this quickly, and it seemed to point me to the sketch I needed anyway. Go to the "find" button. Under property select "sketch parameter name", and for the condition, select "contains". Type the search parameter (d136) and Add to the search list, and hit "find now". The sketch containing the dimension should highlight. From here, edit the sketch to show dims, which you can do by changing the dimension display to name instead of value.
Hope that helps. Not as quick and slick as maybe right clicking on the value in the parameter list, and zeroing in on it from there.
Hi CAD-One,
Here's an ilogic rule to search for parameters. It's not promised to be perfect, but it seems to be working fairly smoothly now. Attached is an example file also.
I hope this helps.
Best of luck to you in all of your Inventor pursuits,
Curtis
http://inventortrenches.blogspot.com
Dim oDoc As Inventor.PartDocument Dim TargetName As String Dim oCompDef As Inventor.PartComponentDefinition Dim oSketch As PlanarSketch Dim oFeature As PartFeature Dim oConstr As DimensionConstraint Dim oParams As Parameters Dim oModelParam As ModelParameter Dim oParam As Parameter Dim oCmdMgr As CommandManager Dim oSet1 As Inventor.HighLightSet Dim oFound As Boolean ‘get the Inventor user name from the Inventor Options myName= ThisApplication.GeneralOptions.UserName oDoc = ThisApplication.ActiveDocument oCompDef = oDoc.ComponentDefinition oParams = oCompDef.Parameters oSet1 = oDoc.CreateHighlightSet TargetName = InputBox("Enter the name of the paramter you wish to find.", "iLogic", "") For Each oSketch In oCompDef.Sketches For Each oConstr In oSketch.DimensionConstraints If oConstr.Parameter.Name = TargetName Then oSketch.Edit oDoc.SelectSet.Select(oSketch) ThisApplication.CommandManager.ControlDefinitions.Item("AppZoomSelectCmd").Execute ThisApplication.CommandManager.ControlDefinitions.Item("AppLookAtCmd").Execute ThisApplication.ActiveView.Update() oSet1.AddItem(oConstr) oSet1.SetColor(255,0,0) MessageBox.Show("Hi " & myName & ", " & vblf & _ TargetName & vblf & "is highlighted.", "iLogic") oFound = True End If Next Next If oFound = True then Return Else For Each oFeature In oCompDef.Features For Each oParam in oFeature.Parameters If oParam.Name = TargetName Then oDoc.SelectSet.Select(oFeature) ThisApplication.CommandManager.ControlDefinitions.Item("AppZoomSelectCmd").Execute ThisApplication.ActiveView.Update() oSet1.AddItem(oFeature) oSet1.SetColor(255,0,0) MessageBox.Show("Hi " & myName & ", " & vblf & _ TargetName & vblf & "is located in: " & vblf & oFeature.Name, "iLogic") oFound = True End If Next Next End if If oFound <> True then MessageBox.Show("A model parameter named: " _ & vblf & TargetName & vblf & "was NOT found.", "iLogic") End if
In the paramaters dialog box, hover your cursor over the parameter name (d136 in your example). Do you get a tooltip with info about where the parameter is used?
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