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Submitted byAnonymouson03-10-202112:47 AM
Status:
Accepted
Display component origin planes on mouseover when holding CTRL-button
I prefer to create constraints on the origin planes of components.
I think it would be a great enhancement if the origin planes of a component will become temporarily visible and selectable by mouseover the component in combination with (for example) the CTRL-key.
Many thanks for posting the idea, and tracked as [INVGEN-54453].
@anna_bostelmann@SteveK88 As to the work feature, are the ones within the component we select for constraint? Or the ones are global work features in top assembly? Thanks!
For those who never saw it, have a look at this gem of a plugin: Show/hide planes (It's not in the store sadly, only on the forums.)
This make life so much easier. Now it's up to Autodesk to integrate something similar. The mouse filters are already there, should not be much of a challenge right?? Option for right-mouse menu and keybind would be great.
Edit: See 6th reply in mentioned topic for plugin.
@DRoam In Solidworks™ when you click on a face, you have access to a visual tree of the assembly, the subassembly, the part, body, feature up down to the face. You can select the constraints on top and the planes on bottom. If something like that were available in Inventor®. I would be so happy.
@Mathieu_Ouellet Yes, this would be nice. But if all you need is to constrain one part's origin planes to the assembly origin planes or to another part's origin planes, there is plenty of iLogic code which I dare say work even better. See for example this post here:
I have a shortcut (for example, number 3) - constrain one part's origin to this assembly's origin and shortcut (number 4) - constrain to another part's origin. This means, when I click number 3 it runs an iLogic rule to do the constraining of the 3 planes. All I have to do then, is to first select the part which needs to be constrained and voila... it is constrained to the origin of this assembly. If I click number 4, then first select the part that needs to be constrained and next the part that you're constraining to (you can select it from the model tree too). And it's that simple.
Now if you need other planes / axis then yes it's more work, but there are a few shortcuts that can be made there too. I do, much more often need constrains based on origin planes, cause that's just how my workflow goes...
I'll attach the 2 iLogic codes and I hope it helps. Credit goes to @WCrihfield
Constrain to this Assembly's Origin:
'https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/ilogic-vba-place-component-at-origin-constraining-planes-without/td-p/9404120
Sub Main()
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("This rule '" & iLogicVb.RuleName & "' only works for Assembly Documents.",vbOK, "WRONG DOCUMENT TYPE")
Return
End If
Dim oADoc As AssemblyDocument = ThisApplication.ActiveDocument
Dim oADef As AssemblyComponentDefinition = oADoc.ComponentDefinition
Dim oAsmYZPlane As WorkPlane = oADef.WorkPlanes.Item(1)
Dim oAsmXZPlane As WorkPlane = oADef.WorkPlanes.Item(2)
Dim oAsmXYPlane As WorkPlane = oADef.WorkPlanes.Item(3)
ReDo :
Dim oOcc As ComponentOccurrence = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter,"Select an Occurrence to constrain.")
Dim oCompAsmDef As AssemblyComponentDefinition
Dim oCompPtDef As PartComponentDefinition
Try
If oOcc.DefinitionDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
oCompAsmDef = oOcc.Definition
oOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(1),oCompYZPlane)
oOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(2),oCompXZPlane)
oOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(3),oCompXYPlane)
ElseIf oOcc.DefinitionDocumentType = DocumentTypeEnum.kPartDocumentObject Then
oCompPtDef = oOcc.Definition
oOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(1),oCompYZPlane)
oOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(2),oCompXZPlane)
oOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(3),oCompXYPlane)
End If
Catch
MessageBox.Show(" Nothing was selected" + vbLf + vbLf + " Or we ran into a mistery...", "Issues", MessageBoxButtons.OK, MessageBoxIcon.Exclamation)
Exit Sub
End Try
oADef.Constraints.AddFlushConstraint(oAsmYZPlane, oCompYZPlane, 0)
oADef.Constraints.AddFlushConstraint(oAsmXZPlane, oCompXZPlane, 0)
oADef.Constraints.AddFlushConstraint(oAsmXYPlane, oCompXYPlane, 0)
Redo = MsgBox("Repeat?", vbYesNoCancel + vbQuestion, "REPEAT?")
If Redo = vbYes Then
GoTo Redo
Else
Exit Sub
End If
End Sub
Constrain to Another Part's Origin:
'https://forums.autodesk.com/t5/inventor-ilogic-and-vb-net-forum/ilogic-vba-place-component-at-origin-constraining-planes-without/td-p/9404120
Sub Main()
If ThisApplication.ActiveDocumentType <> DocumentTypeEnum.kAssemblyDocumentObject Then
MsgBox("This rule '" & iLogicVb.RuleName & "' only works for Assembly Documents.",vbOK, "WRONG DOCUMENT TYPE")
Return
End If
Dim oADoc As AssemblyDocument = ThisApplication.ActiveDocument
Dim oADef As AssemblyComponentDefinition = oADoc.ComponentDefinition
Dim oAsmYZPlane As WorkPlane = oADef.WorkPlanes.Item(1)
Dim oAsmXZPlane As WorkPlane = oADef.WorkPlanes.Item(2)
Dim oAsmXYPlane As WorkPlane = oADef.WorkPlanes.Item(3)
Dim oOcc As ComponentOccurrence = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter,"1. Select First Part to Constrain.")
Dim oCompAsmDef As AssemblyComponentDefinition
Dim oCompPtDef As PartComponentDefinition
Try
If oOcc.DefinitionDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
oCompAsmDef = oOcc.Definition
oOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(1),oCompYZPlane)
oOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(2),oCompXZPlane)
oOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(3),oCompXYPlane)
ElseIf oOcc.DefinitionDocumentType = DocumentTypeEnum.kPartDocumentObject Then
oCompPtDef = oOcc.Definition
oOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(1),oCompYZPlane)
oOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(2),oCompXZPlane)
oOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(3),oCompXYPlane)
End If
Dim iOcc As ComponentOccurrence = ThisApplication.CommandManager.Pick(SelectionFilterEnum.kAssemblyOccurrenceFilter,"2. Select Part to Constrain to.")
If iOcc.DefinitionDocumentType = DocumentTypeEnum.kAssemblyDocumentObject Then
oCompAsmDef = iOcc.Definition
iOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(1),iCompYZPlane)
iOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(2),iCompXZPlane)
iOcc.CreateGeometryProxy(oCompAsmDef.WorkPlanes.Item(3),iCompXYPlane)
ElseIf iOcc.DefinitionDocumentType = DocumentTypeEnum.kPartDocumentObject Then
oCompPtDef = iOcc.Definition
iOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(1),iCompYZPlane)
iOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(2),iCompXZPlane)
iOcc.CreateGeometryProxy(oCompPtDef.WorkPlanes.Item(3),iCompXYPlane)
End If
oADef.Constraints.AddFlushConstraint(iCompYZPlane, oCompYZPlane, 0)
oADef.Constraints.AddFlushConstraint(iCompXZPlane, oCompXZPlane, 0)
oADef.Constraints.AddFlushConstraint(iCompXYPlane, oCompXYPlane, 0)
Catch
MessageBox.Show(" Nothing was selected" + vbLf + vbLf + " Or we ran into a mistery...", "Issues", MessageBoxButtons.OK, MessageBoxIcon.Exclamation)
End Try
End Sub
@basautomationservices But with your plugin is it as quick as 2 or 3 clicks? All I do literally is click number 3 and click the part I need constrained to origin and it's there. And it'll even repeat, so that I can click like 10 parts in seconds.
Now if I would constrain to other planes / origins I could consider it for those.
All good but usually I like to constrain one plane to one component and the others to other components. I align the top to top of and other and then the face to a face and the last plane to an other component.
@Mathieu_Ouellet, I try to avoid constraining to other part's faces and features as much as possible and rather constrain to planes, axis and points. Features can change. Planes, axis, points - not as much. But indeed my work flow condones this much more, since I do a lot more top down designing.
I have a macro mapped to keyboard which cycles through the selected part/assembly planes. With holding CTRL you can add another plane to selection and you can proceed to Constrain Command
Public Sub selectplane()
Dim invDoc As Document
Set invDoc = ThisApplication.ActiveDocument
If invDoc.DocumentType <> kAssemblyDocumentObject Then
MsgBox "Command works only in Assemblies"
Exit Sub
End If
Dim SelectedItem, RefObj As Object
Dim SelectedSet As SelectSet
Dim i, cindex As Integer
Dim workPlanes As workPlanes
Dim workPlane, firstplane, selectedPlane As workPlane
Dim workPlaneProxy, firstplaneProxy, selectedplaneProxy As workPlaneProxy
Dim Planename As String
Dim oStartHLSet As HighlightSet
Dim RefOcc As ComponentOccurrence
Set SelectedSet = invDoc.SelectSet
If SelectedSet.Count <> 0 And SelectedSet.Count < 5 Then
cindex = SelectedSet.Count
Set SelectedItem = SelectedSet.Item(cindex)
Select Case SelectedItem.Type
Case kEdgeProxyObject, kVertexProxyObject, kFaceProxyObject
Set RefObj = SelectedItem.ContainingOccurrence.Definition
Set RefOcc = SelectedItem.ContainingOccurrence
Set workPlanes = RefObj.workPlanes
Set firstplane = workPlanes.Item(1)
invDoc.SelectSet.Remove (cindex)
Call RefOcc.CreateGeometryProxy(firstplane, selectedplaneProxy)
Call invDoc.SelectSet.Select(selectedplaneProxy)
GoTo ccc
Case kComponentOccurrenceObject, kComponentOccurrenceProxyObject
Set RefObj = SelectedItem.Definition
Set workPlanes = RefObj.workPlanes
Set firstplane = workPlanes.Item(1)
Call SelectedItem.CreateGeometryProxy(firstplane, selectedplaneProxy)
Call invDoc.SelectSet.Select(selectedplaneProxy)
GoTo ccc
End Select
If SelectedItem.Type = kWorkPlaneProxyObject Then
If SelectedItem.ContainingOccurrence.Type = kComponentOccurrenceObject Or SelectedItem.ContainingOccurrence.Type = kComponentOccurrenceProxyObject Then
Planename = SelectedItem.name
Set RefObj = SelectedItem.ContainingOccurrence.Definition
Set RefOcc = SelectedItem.ContainingOccurrence
Set workPlanes = RefObj.workPlanes
Set firstplane = workPlanes.Item(1)
For i = 1 To workPlanes.Count
If workPlanes.Item(i).name = Planename Then
If i = workPlanes.Count Then
Set selectedPlane = firstplane
invDoc.SelectSet.Remove (cindex)
Call RefOcc.CreateGeometryProxy(selectedPlane, selectedplaneProxy)
Call invDoc.SelectSet.Select(selectedplaneProxy)
GoTo ccc
Else
Set selectedPlane = workPlanes.Item(i + 1)
invDoc.SelectSet.Remove (cindex)
Call RefOcc.CreateGeometryProxy(selectedPlane, selectedplaneProxy)
Call invDoc.SelectSet.Select(selectedplaneProxy)
GoTo ccc
End If
End If
Next
End If
End If
If SelectedItem.Type = kWorkPlaneObject Then
Planename = SelectedItem.name
Set workPlanes = invDoc.ComponentDefinition.workPlanes
Set firstplane = workPlanes.Item(1)
For i = 1 To workPlanes.Count
If workPlanes.Item(i).name = Planename Then
If i = workPlanes.Count Then
Set selectedPlane = firstplane
invDoc.SelectSet.Remove (cindex)
invDoc.SelectSet.Select selectedPlane
Else
Set selectedPlane = workPlanes.Item(i + 1)
invDoc.SelectSet.Remove (cindex)
invDoc.SelectSet.Select selectedPlane
End If
End If
Next
End If
End If
ccc:
End Sub
First, I have mapped this VBA macro to a keyboard key. You can then select any component or assembly within assembly (It is based on you current Selection filter) and by pressing assigned key, command cycles through all planes (starting with Default planes and then all created). By holding CTRL you can select the second component/subassembly to cycle the planes.
