From the Trenches with Autodesk Inventor

Are you looking for a video tutorial series for Autodesk Inventor?

Infinite Skills has recently released its Learning Autodesk Inventor 2014 series featuring instructor Adam Cooper. I was provided the DVD and asked to review this tutorial series, and was very pleased with the content found within.

When I popped in the DVD, the autoplay opened the viewing application and presented me with the Chapter menu as shown here:

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Once I clicked on Chapter 1, I was presented with a list of topics as shown here:

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A status legend on the right shows which videos I've watched with a shaded dot, as well as a partially shaded dot for those videos that I only watched part of. As you can image this can be a great help when jumping around within the chapters.

Once a topic is selected the video plays in the application. The author's pace is quite good, but since it is a video you can always use the buttons found in the video control tool bar to pause and rewind as needed.

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Also included on the DVD are all of the working files needed for the exercises. The files can be accessed easily via the video interface.

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This DVD contains some outstanding material from a very knowledgeable instructor. You'll have the feeling you're in the classroom being led through the course material with Adam Cooper right there helping you along the way!

For more information, have a look at the Infinite Skills website:
http://www.infiniteskills.com/training/learning-autodesk-inventor-2014.html

Issue:
You have some custom iProperties in your file that you want to remove. Because you have a lot of files that contain these custom iProperties, you find yourself doing this quite often. You'd like an iLogic rule that will help with this when you encounter these custom iProperties.

Solution:
Here are three rule variations to help with this.

Variation 1
Delete only the custom iProperties found in the list.

'------- start of ilogic ------

'define list of custom properties to delete

Dim MyArrayList As New ArrayList

MyArrayList.add("Hello World 001")

MyArrayList.add("Hello World 002")

MyArrayList.add("Hello World 003")

'define custom property collection

oCustomPropertySet = ThisDoc.Document.PropertySets.Item("Inventor User Defined Properties")

'look at each property in the collection

For Each oCustProp in oCustomPropertySet

'check property name against the list you want to delete

If MyArrayList.Contains(oCustProp.name)Then

'delete the custom iProperty

oCustProp.Delete

Else

'skip it

End If

Next

'------- end of ilogic ------

Variation 2
Delete only the custom iProperties NOT found in the list.

'------- start of ilogic ------

'define list of custom properties to keep

Dim MyArrayList As New ArrayList

MyArrayList.add("Hello World 001")

MyArrayList.add("Hello World 002")

MyArrayList.add("Hello World 003")

'define custom property collection

oCustomPropertySet = ThisDoc.Document.PropertySets.Item("Inventor User Defined Properties")

'look at each property in the collection

For Each oCustProp in oCustomPropertySet

'check property name against the list you don't want to delete

If MyArrayList.Contains(oCustProp.name)Then

'skip it

Else

'delete the custom iProperty

oCustProp.Delete

End If

Next

'------- end of ilogic ------

Variation 3
Delete All custom iProperties found in the part.

'------- start of ilogic ------

'define custom property collection

oCustomPropertySet = ThisDoc.Document.PropertySets.Item("Inventor User Defined Properties")

'look at each property in the collection

For Each oCustProp in oCustomPropertySet

'delete the custom iProperty

oCustProp.Delete

Next

'------- end of ilogic ------

Issue:
You have a title block that uses prompted entry, and you'd like to fill those fields in from data that is in a spread sheet. You know that the best way to set up a title block is to use the model file's iProperties, but unfortunately you can't make changes to the title block that you've been provided. But there must be a better way than just editing each sheet and re-typing the same information over and over, right?

Solution:
Here is an iLogic rule that asks the user to browse for an spreadsheet. Then it reads in the data and matches the field name to the title block field, and if a match is found it writes the field value to the title block's prompted entry field.

Here is an example spread sheet:

Here is an example Title Block:

And here you can see the field text in the title block, with those that are prompted entries denoted by carats: < >

So the iLogic code gets the information from the spreadsheet and then writes it to the title block for every sheet in the drawing.

I've added some lines to activate each drawing sheet and a delay timer to step through each text field so that you can watch the changes, but all of that could be removed if you'd prefer to speed up the running of the rule.

'Browse for the Excel file

Dim oFileDlg As inventor.FileDialog = Nothing

InventorVb.Application.CreateFileDialog(oFileDlg)

oFileDlg.Filter = "Excel Files (*.xls;*.xlsx)|*.xls;*.xlsx"

oFileDlg.DialogTitle = "Select a Project Information Excel File"

oFileDlg.InitialDirectory = ThisDoc.Path

oFileDlg.CancelError = True

On Error Resume Next

oFileDlg.ShowOpen()

If Err.Number <> 0 Then

'exit if file not selected

Return

ElseIf oFileDlg.FileName <> ""Then

myXLS = oFileDlg.FileName

End If

'look at sheet1 of the spreadsheet

GoExcel.Open(myXLS, "Sheet1")

'define the drawing

Dim oDoc As DrawingDocument

oDoc = ThisApplication.ActiveDocument

Dim oSheet As Sheet

Dim oPromptEntry

'gather the current sheet name

Dim oCurrentSheet

oCurrentSheet = oDoc.ActiveSheet.Name

'step through each sheet

i = 0

For Each oSheet In oDoc.Sheets

i = i+1

'activate the sheet

ThisApplication.ActiveDocument.Sheets.Item(i).Activate

oTitleBlock=oSheet.TitleBlock

oTextBoxes=oTitleBlock.Definition.Sketch.TextBoxes

For Each oTextBox In oTitleBlock.Definition.Sketch.TextBoxes

'look at the first 100 rows of the Excel file

'start at row 2, since row 1 contains headings

For rowCheck = 2 To 100

'read the value of the column A

Dim myCell As String

myCell = "<"& GoExcel.CellValue("A"& rowCheck) & ">"

'compare the titleblock field name to the value in column A

If myCell = oTextBox.Text Then

'get the value from column B

oPromptEntry = GoExcel.CellValue("B"& rowCheck)

'set the prompted entry value

Call oTitleBlock.SetPromptResultText(oTextBox, oPromptEntry)

'______ add a small delay between text field updates

PauseTime = 0.3 'seconds

Start = Timer

Do While Timer < Start + PauseTime

ThisApplication.UserInterfaceManager.DoEvents

'present a status bar message

ThisApplication.StatusBarText = _

oDoc.ActiveSheet.Name & " is updating...."

Loop

'______ end of timer code

End If

Next

'return to original sheet

ThisApplication.ActiveDocument.Sheets.Item(oCurrentSheet).Activate

'clear the status bar message

ThisApplication.StatusBarText = ""

Issue:
You've upgraded to Autodesk Inventor 2015 from a previous version and find that some of the tool buttons have been hidden and stacked into grouped, fly-out menus. You've checked with a reputable attorney, and have found out that it's not legal to sneak into the Autodesk Inventor development team's office and release two dozen rabid ferrets, as payback for them once again dinking with Inventor's interface. So as "Plan B" you'd like to find some way to make the buttons more easily accessible. Can this be done?

Solution:
You can right click any tool group that has a dropdown arrow next to it and choose Ungroup. And you can also select a specific tool and choose Move to Main Panel if it's one you use often.

For further information on customizing the display of ribbon panels, visit this link:
http://help.autodesk.com/view/INVNTOR/2015/ENU/?guid=GUID-E5AB014C-D87B-4D7B-963C-00847E3DDE01

Issue:
You're working with sketches in some iLogic code and want to be able to find the active sketch name, or active sketch number.

Solution:
Here are a couple of quick rules that will do this. And also as a bonus there is a quick rule to delete all sketches in the part.

Rule1: Find the active sketch name

Dim oSketch As PlanarSketch

If Typeof ThisApplication.ActiveEditObject Is Sketch Then

oSketch = ThisApplication.ActiveEditObject

MessageBox.Show(oSketch.Name & " is the active Sketch", "iLogic")

Else

MessageBox.Show("Active Edit Object is not a Sketch", "iLogic")

End If

Rule2: Find the active sketch number

Dim oSketches As PlanarSketches

oSketches = ThisApplication.ActiveDocument.ComponentDefinition.Sketches

i=1

For Each oSketch in oSketches

oSketch = oSketches.Item(i)

If oSketch Is ThisApplication.ActiveEditObject Then

MessageBox.Show("The active sketch is number: "& i, "iLogic")

Else

End If

i=i+1

Next

Rule3: Delete all sketches.

Dim oSketches As PlanarSketches

oSketches = ThisApplication.ActiveDocument.ComponentDefinition.Sketches

If Typeof ThisApplication.ActiveEditObject Is Sketch Then

ThisApplication.ActiveEditObject.ExitEdit

Else

End If

For Each oSketch in oSketches

oSketch = oSketches.Item(oSketch.Name)

oSketch.Delete

Next

Issue:
You have some iLogic code to help you setup your drawing sheets and title block size (see this link from Jonathan Landeros for a great example of using iLogic to configure title block and borders). But when you change sheet to a larger size the dimension text is hard to read. You'd like to be able to adjust the dimension style text size as well.

Solution:
Here is a quick iLogic rule that prompts the user to set the text size. You could remove the user input lines, and just have the value set depending on the sheet size as well.

'set active document as drawing document

Dim oDoc As DrawingDocument

oDoc = ThisApplication.ActiveDocument

'get the active dim style

Dim oDStyle As DimensionStyle

oDStyle = oDoc.StylesManager.ActiveStandardStyle. _

ActiveObjectDefaults.LinearDimensionStyle

'get current font size

Dim sFontSize as String

sFontSize = oDStyle.TextStyle.FontSize

'get user input

oInput = InputBox("Active Dimesnion Style = "& oDStyle.Name _

& vblf & vblf & "Enter a new font size in inches.", "iLogic", _

Round(sFontSize / 2.54,3))

'set font size for dim style

oDStyle.TextStyle.FontSize = oInput * 2.54

Here is a related topic also:
http://inventortrenches.blogspot.com/2011/05/use-ilogic-to-change-sheet-orientation.html

Issue:
Your assembly has several Level of Detail Representations set up, which works well. The problem is that when you add a new component to the assembly, you have to go to each Level of Detail and suppress the component in order to prevent it from showing up in those existing Level of Detail Representations.

Solution:
Here is an iLogic rule that will suppress any selected components in all of the other LOD's, with the exception of the active LOD.

This allows you to place the component in the assembly with the LOD you want to add the component to set active, then select the component (or components) and run this iLogic rule to remove the component(s) from the other LODs.

This iLogic rule also doesn't suppress the selected components in the standard LODs, such as the "Master" LOD, the "All Content Center Suppressed" LOD, etc.

Note too that it saves the file each time one of the other LODs is modified in order to make the changes "stick", so if you have a large assembly with many LODs it might take a bit for this rule to run.

Dim oDoc As AssemblyDocument

oDoc = ThisApplication.ActiveDocument

' Find all selected components and add them to an ObjectCollection.

Dim oSelected As ObjectCollection

oSelected = ThisApplication.TransientObjects. _

CreateObjectCollection (oDoc.SelectSet)

'define LOD rep

Dim oLODRep As LevelOfDetailRepresentation

'define rep manager

Rep_Manager =ThisApplication.ActiveDocument. _

ComponentDefinition.RepresentationsManager

'define an arraylist to hold the list of LOD rep names

Dim NameList As New ArrayList()

'look at the LOD reps in the assembly

For Each oLODRep in Rep_Manager.LevelOfDetailRepresentations

'add the LOD names to the array list

NameList.add(oLODRep.Name)

Next

Dim myLOD as LevelOfDetailRepresentation

'get the name of the active LOD

myLOD = Rep_Manager.ActiveLevelOfDetailRepresentation

'remove active LOD from list

NameList.remove(myLOD.name)

'remove standard LODs from list

NameList.remove("Master")

NameList.remove("All Components Suppressed")

NameList.remove("All Parts Suppressed")

NameList.remove("All Content Center Suppressed")

'step through the LOD list

'and suppress the selected components

Dim sName as String

For Each sName in NameList

'Activate the LOD

Rep_Manager.LevelOfDetailRepresentations(sName).Activate

For Each oObject in oSelected

Try

'suppress component

Component.IsActive(oObject.Name) = False

Catch ' catch any errors

End Try

Next

ThisDoc.Save

Next

'set the original active LOD back to active

Rep_Manager.LevelOfDetailRepresentations(Trim(myLOD.Name)).Activate

Issue:
You need your iLogic code to check to see if the file type is a part file first, before running. Otherwise it generates an error. Is there a way to do this?

Solution:
Here are a couple of quick code snippets that demonstrate how to do this using the DocumentType enumerators:

'start of iLogic rule - - - - - - - - - - - - - - - - - -

doc = ThisDoc.ModelDocument

'check file type

If doc.DocumentType = kPartDocumentObject Then

MessageBox.Show("This is a part file.", "iLogic")

Else if doc.DocumentType = kAssemblyDocumentObject Then

MessageBox.Show("This is an assembly file.", "iLogic")

End if

'end of iLogic rule - - - - - - - - - - - - - - - - - -

'start of iLogic rule - - - - - - - - - - - - - - - - - -

doc = ThisDoc.ModelDocument

'check file type

If doc.DocumentType = kPartDocumentObject Then

'do nothing

Return

Else if doc.DocumentType = kAssemblyDocumentObject Then

'do something

MessageBox.Show("This is an assembly file.", "iLogic")

End if

'end of iLogic rule - - - - - - - - - - - - - - - - - -

Here is a list of all of the the DocumentType enumerators available in the API:

kUnknownDocumentObject
kPartDocumentObject
kAssemblyDocumentObject
kDrawingDocumentObject
kPresentationDocumentObject
kDesignElementDocumentObject
kForeignModelDocumentObject
kSATFileDocumentObject

kNoDocument

Update July 02, 2013
Here is another version of the rule that will report the file type and check to see if a sketch is active. This example rule will report the file type even when editing within another file type. Meaning that if you have a part file active within an assembly, this rule reports that it is a part file.

'start of iLogic rule - - - - - - - - - - - - - - - - - -

Dim oDoc As Document

oDoc = ThisDoc.Document

If oDoc.DocumentType = Inventor.DocumentTypeEnum.kPartDocumentObject Then

If Typeof ThisApplication.ActiveEditObject Is Sketch Then

MessageBox.Show("You have a sketch active in a part file.", "iLogic")

Else

MessageBox.Show("This is a part file.", "iLogic")

End If

Else If oDoc.DocumentType = Inventor.DocumentTypeEnum.kAssemblyDocumentObject Then

If Typeof ThisApplication.ActiveEditObject Is Sketch Then

MessageBox.Show("You have a sketch active in an assembly file.", "iLogic")

Else

MessageBox.Show("This is an assembly file.", "iLogic")

End If

Else If oDoc.DocumentType = Inventor.DocumentTypeEnum.kDrawingDocumentObject Then

If Typeof ThisApplication.ActiveEditObject Is Sketch Then

MessageBox.Show("You have a sketch active in a drawing file.", "iLogic")

Else

MessageBox.Show("This is a drawing file.", "iLogic")

End If

'end of iLogic rule - - - - - - - - - - - - - - - - - -

Update 5/27/2014
Luke Davenport's blog article "iLogic – Exit Rule Based on File Type"
http://www.cadlinecommunity.co.uk/Blogs/Blog.aspx?ScoId=d94fe4c0-e7d8-49ae-921d-04910a7d9740

Issue:
You have other members of your design team that do not remember to turn off work features at the part level or sub-assembly level when they are done working with those files. As a result file previews and view representations get messed up. You'd like to have a quick way to toggle all of the work features off. Can this be done with iLogic?

Solution:
You can use this example iLogic rule to toggle all work features on or off.

'catch and skip errors

On Error Resume Next

'define the active assembly

Dim oAssyDoc As AssemblyDocument

oAssyDoc = ThisApplication.ActiveDocument

'get user input as True or False

wfBoolean = InputRadioBox("Turn all Work Features On/Off", "On", "Off", False, "iLogic")

'Check all referenced docs

Dim oDoc As Inventor.Document

For Each oDoc In oAssyDoc.AllReferencedDocuments

'set work plane visibility

For Each oWorkPlane In oDoc.ComponentDefinition.WorkPlanes

oWorkPlane.Visible = wfBoolean

Next

'set work axis visibility

For Each oWorkAxis In oDoc.ComponentDefinition.WorkAxes

oWorkAxis.Visible = wfBoolean

Next

'set work point visibility

For Each oWorkPoint In oDoc.ComponentDefinition.WorkPoints

oWorkPoint.Visible = wfBoolean

Next

'update the files

InventorVb.DocumentUpdate()

Issue:

You have a number of standard Virtual parts that you find yourself adding over and over. You'd like to have the ability to add them based on a predefined list.

Solution:

Here is an example iLogic rule that will read a *.txt file and present the contents to the user in an input box list. The user is then asked to enter a quantity for the virtual part, and then the virtual part occurrences are added to the assembly. If one or more occurrences of the virtual part exist in the assembly, the iLogic rule deletes them and just adds back the total number needed.

(update: see also iLogic - Add Standard Virtual Parts From an Excel File or a similar solution)

An example text file list

The list presented to the user in an input list box.

The input box presented to the user to set the quantity.

The virtual parts added to the assembly.

Adjusting the quantity.

The iLogic rule deletes the original 18 occurrences and just adds back the number specified.

Here is the example iLogic rule:
(special thanks to Brian Ekins for the code he posted at this link.)

Imports System.IO

'open and read a text file

Dim oRead As New StreamReader("U:\iLogic examples\Virtual Part List.txt")

Dim sLine As String = ""

Dim MyArrayList As New ArrayList

'build list from text file

sLine = oRead.ReadLine()

If Not sLine Is Nothing Then

MyArrayList.Add(sLine)

End If

Loop Until sLine Is Nothing

oRead.Close()

'get user input from list

sVirtPart = InputListBox("Select a virtual part to add.", _

MyArrayList, MyArrayList.Item(0), "iLogic", "Standard Virtual Parts")

'check for empty input

'in the case where the user

'cancels out of the input box

If sVirtPart = ""Then

Return 'end rule

Else

End if

'get quantity from user

iQTY = InputBox("Enter the TOTAL number of:"_

& vblf & " ''"& sVirtPart & "''"_

& vblf & "to place in the assembly."_

& vblf & vblf & "Note: Enter 0 to delete all existing instances.", "iLogic", "1")

'check for empty input

'in the case where the user

'cancels out of the input box

If iQTY = ""Then

Return 'end rule

Else

End if

'define assembly

Dim asmDoc As AssemblyDocument

asmDoc = ThisApplication.ActiveDocument

'define assembly Component Definition

Dim oAsmCompDef As AssemblyComponentDefinition

oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

'Iterate through all of the occurrences in the assembly

Dim asmOcc As ComponentOccurrence

For Each asmOcc In oAsmCompDef.Occurrences

'get name of occurence only (sees only everything left of the colon)

Dim oOcc As Object

oOcc = asmOcc.name.Split(":")(0)

'look at only virtual components

If TypeOf asmOcc.Definition Is VirtualComponentDefinition Then

'compare name selected from list to the

'existing virtual parts

If oOcc = sVirtPart Then

'delete existing virtual parts if name matches

asmOcc.delete

Else

End if

Else

End If

Next

Dim occs As ComponentOccurrences

occs = asmDoc.ComponentDefinition.Occurrences

Dim identity As Matrix

identity = ThisApplication.TransientGeometry.CreateMatrix

'create first instance of the virtual part

Dim virtOcc As ComponentOccurrence

if iQTY >= 1 Then

virtOcc = occs.AddVirtual(sVirtPart, identity)

Else

Return

End if

'add next instance starting at instance2 (if applicable)

Dim index As Integer

index = 2

Do While index <= iQTY

occs.AddByComponentDefinition(virtOcc.Definition, identity)

index += 1

Loop

Issue:
You're looking for an integrated CAM solution to use with Autodesk Inventor.

Potential Solution:
Check out the Inventor HSM Express Beta tools.

From the Autodesk CAM Team:

The Autodesk CAM Team has launched the official Public Beta of Inventor HSM Express, a free 2-1/2 Axis CAM solution for Inventor users.

Powered by HSMWorks CAM technology, Inventor HSM Express has all the capabilities of HSMXpress – the Free CAM Solution for SolidWorks and is seamlessly integrated inside the design environment of Autodesk Inventor. This integration allows Inventor users to take advantage of workflow and tools they are used to when programming CNC toolpaths for their 2.5D machining projects.

If you are an experienced Inventor user we could really use your help. Our goal is to have a CAM solution so tightly integrated with Inventor that you don’t perceive any difference when switching between the modeling environment and the CAM environment. Your feedback is crucial in helping us achieve this goal. And, for those of you with CNC programming experience, we would love to hear your first impressions in working with our new CAM tools.

If you'd like to participate in our Beta but don’t have Autodesk Inventor you can download a 30-day trial at this link: http://www.autodesk.com/products/autodesk-inventor-family/free-trial

To participate in the Inventor HSM Express Beta and watch a quick preview of Inventor HSM Express, you can visit this link: https://beta.autodesk.com/callout/?callid=22396638F5374AC28E2F1A24CC7EEFA8

Issue:

You have a number of standard Virtual parts that you find yourself adding over and over. You'd like to have the ability to add them based on a predefined list.

You saw the post about adding these parts from a text file, but you'd like to be able to add standard iProperties for these virtual parts also. This way your Bill of Materials information for the virtual parts can be set when the virtual part is created. So you were wanting to read data from an XLS file that contains all of the information that you typically add for virtual parts.

Solution:

Here is an example iLogic rule that will read a *.xls file and present the contents to the user in an input box list. The user is then asked to enter a quantity for the virtual part, and then the virtual part occurrences are added to the assembly. If one or more occurrences of the virtual part exist in the assembly, the iLogic rule deletes them and just adds back the total number needed.

As the virtual parts are added, the iProperty information found in the *.xls file is added also.

In this example the parts are placed by using the A column, which is the description. Then the other columns are read in and used to populate the virtual part's iProperties.

An example XLS file list with iProperty information.

Dim MyArrayList As New ArrayList

MyArrayList = GoExcel.CellValues("U:\iLogic examples\Virtual Part List.xls", "Sheet1", "A2", "A1000")

Dim sVirtPart As String

'get user input from list

sVirtPart = InputListBox("Select a virtual part to add.", _

MyArrayList, MyArrayList.Item(0), "iLogic", "Standard Virtual Parts")

'check for empty input in the case where the user cancels out of the input box

If sVirtPart = ""Then

Return 'end rule

Else

End if

'get iProperties from the XLS file

For MyRow = 2 To 1000 'index row 2 through 1000

'find the cell in column A that matches the user selection

If sVirtPart = (GoExcel.CellValue("A"& MyRow)) Then

'get the iProperty from the XLS file for each column

oProp1 = GoExcel.CellValue("A"& MyRow )

oProp2 = GoExcel.CellValue("B"& MyRow )

oProp3 = GoExcel.CellValue("C"& MyRow)

oProp4 = GoExcel.CellValue("D"& MyRow)

oProp5 = GoExcel.CellValue("E"& MyRow)

Exit For

End If

Next

'get quantity from user

iQTY = InputBox("Enter the TOTAL number of:"_

& vblf & " ''"& sVirtPart & "''"_

& vblf & "to place in the assembly."_

& vblf & vblf & "Note: Enter 0 to delete all existing instances.", "iLogic", "1")

'check for empty input in the case where the user cancels out of the input box

If iQTY = ""Then

Return 'end rule

Else

End if

'define assembly

Dim asmDoc As AssemblyDocument

asmDoc = ThisApplication.ActiveDocument

'define assembly Component Definition

Dim oAsmCompDef As AssemblyComponentDefinition

oAsmCompDef = ThisApplication.ActiveDocument.ComponentDefinition

'Iterate through all of the occurrences in the assembly

Dim asmOcc As ComponentOccurrence

For Each asmOcc In oAsmCompDef.Occurrences

'get name of occurence only (sees only everything left of the colon)

Dim oOcc As Object

oOcc = asmOcc.name.Split(":")(0)

'look at only virtual components

If TypeOf asmOcc.Definition Is VirtualComponentDefinition Then

'compare name selected from list to the

'existing virtual parts

If oOcc = sVirtPart Then

'delete existing virtual parts if name matches

asmOcc.delete

Else

End if

Else

End If

Next

Dim occs As ComponentOccurrences

occs = asmDoc.ComponentDefinition.Occurrences

Dim identity As Matrix

identity = ThisApplication.TransientGeometry.CreateMatrix

'create first instance of the virtual part

Dim virtOcc As ComponentOccurrence

if iQTY >= 1 Then

virtOcc = occs.AddVirtual(sVirtPart, identity)

Try

iProperties.Value(sVirtPart & ":1", "Project", "Description") = oProp1

Catch 'catch error when oProp1 = nothing

End Try

Try

iProperties.Value(sVirtPart & ":1", "Project", "Part Number") = oProp2

Catch 'catch error when oProp2 = nothing

End Try

Try

iProperties.Value(sVirtPart & ":1", "Project", "Revision Number") = oProp3

Catch 'catch error when oProp3 = nothing

End Try

Try

iProperties.Value(sVirtPart & ":1", "Project", "Vendor") = oProp4

Catch 'catch error when oProp4 = nothing

End Try

Try

iProperties.Value(sVirtPart & ":1", "Summary", "Comments") = oProp5

Catch 'catch error when oProp5 = nothing

End Try

Else

Return

End if

'add next instance starting at instance2 (if applicable)

Dim index As Integer

index = 2

Do While index <= iQTY

occs.AddByComponentDefinition(virtOcc.Definition, identity)

index += 1

Loop

Issue:
You use the Frame Generator tools in Autodesk Inventor all of the time, but you find that creating the base 3D sketch is tedious, time consuming, and doesn't always take edits well. Is there another way to do this?

Solution:
There are some times when a creating a 3D sketch is required, but often time it's helpful to know that you can use the edges of a 3D base part to place Frame Generator members. When you select a part edge, Frame Generator automatically projects the geometry into the Frame Reference Model that it creates using the selected edges.

For instance you could create a basic 3D solid part model such as the one shown, and place it into an assembly file:

If you need more edges to use for the frame selection you can edit the base part model, and sketch on the faces of the solid:

There are times where you might want to create a 3d Sketch based upon 2D sketch geometry. Here a 3D sketch is created and the 2D sketch is projected to the face pf the part to provide more edges to use in the frame. This is done using the 3D Project to Surface tool:
http://wikihelp.autodesk.com/Inventor/enu/2012/Help/3320-Show_Me_3320/3321-Show_Me_3321/3538-3D_Sket...

Often it's helpful to make the base part a clear color so you can see all of the edges to be used for selection:

In order to prevent the base model from impacting the mass of your assembly, you can set it to Reference:

Once you are finished selecting edges, you can just turn off the Visibility setting of the base part file, leaving only the frame showing:

Issue:
You've been somewhat successful using iLogic code examples that you find online, but you'd really like to learn how to create your own code from scratch. So how do these other people find the programming calls to create new code? It seems that there is some missing puzzle piece that you can't seem to locate, something that explains how to get started programming in Inventor. Does something like that exist?

Solution:
Programming in iLogic involves two different methods, that are often mixed together. The first method is to use "native" iLogic functions, the second is to use "raw" API functions by employing Inventor's Application Programming Interface (API).

"Native" iLogic functions are a dictionary of automation functions that deliver the power of Inventor's Application Programming Interface (API) to users by using single-line automation functions. So you can think of iLogic as a collection of the more common programming and automation tasks that the developers have "cleaned" up so that users can create some Rule based automation in their design. This mean that the iLogic dictionary is just a simple subset of the larger API collection.

"Raw"API language can be run using the iLogic tools as well, but will require more knowledge of VB.Net based syntax, and more need to declare and define within the code language. To get started with Inventor's Application Programming Interface (API) you can use the following links.

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This paper provides a brief overview of Inventor’s programming interface and illustrates this with examples using iProperties:
VBA & Inventor API Introduction (zip file - 11.2 MB)

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The following resource will help you get started with programming Inventor. It assumes familiarity with Autodesk Inventor and general programming concepts:

DevTV: Introduction to Inventor Programming, a self-paced video tutorial demonstrating how to get started developing with Autodesk Inventor.
View online | Download (zip file- 51.8 MB)
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The links above as well as additional information concerning the Autodesk Developer Network resources, can be found at this link:

http://usa.autodesk.com/adsk/servlet/index?id=1079044&siteID=123112

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Issue:
You want to create a view on your drawing that has some parts shaded and some that look wire-framed, so you can show some particular detail of your assembly in your detailed drawing.

In the past you could do it as described in tip #1 at this link, but that seems not to work now.
http://inventortrenches.blogspot.com/2011/06/autodesk-inventor-tips-from-around-web.html

Solution:
Here is another way to do this.

Create one new Positional Representation ( no need to do anything else with it, other than creating it).

Create 2 View Representations

In View Representation 1, turn off the visibility of the part you want to show wireframe

In View Representation 2, turn off the visibility of everything else

Create a drawing Base View and set it to use View Representation 2

Create an Overlay View, and set it to use the Positional Representation and View Representation 1

In the Overlay View dialog box set the style to be not shaded & hidden lines removed

And also in the Overlay View dialog box set the Layer dropdown to be 'As Parts'.

Here's a link to a quick video.

Issue:
You want to "filter" a list (List B) based on the selection from another list (List A), but the lists are long and writing the If/Then or Select Case statements are repetitive, and difficult to maintain. Is there a better way?

Solution:
You can use ArrayLists and For Each Statements to do this, as shown in this example.

Here an illogic form is used, and when a value is selected from List A, then List B and C are reset to include only values less than or equal to the current selected List A value.

Example file:

SyntaxEditor Code Snippet
Example code:

'reset List B list to default
MultiValue.SetList("List_B", 1,2,3,4,5,6,7,8,9,10,11,12,13,14,15,16)

'reset List C list to default
MultiValue.SetList("List_C", 2,4,6,8,10,12,14,16)

DimB_ListAsNewArrayList
B_List=MultiValue.List("List_B")

DimC_ListAsNewArrayList
C_List=MultiValue.List("List_C")

DimTemp_ListAsNewArrayList

Temp_List.Clear
ForEachoIteminB_List
IfList_A>=oItemThen
Temp_List.Add(oItem)
EndIf
Next

MultiValue.List("List_B")=Temp_List

Temp_List.Clear
ForEachoIteminC_List
IfList_A>=oItemThen
Temp_List.Add(oItem)
EndIf
Next

MultiValue.List("List_C")=Temp_List

Issue:
You want to to quickly select and set standard tolerances for your sketch dimensions.

Solution:
Here is a quick routine written for iLogic using the API to do this. This employs the CommandManager's Pick function to allow you to select individual dimensions and set the tolerance.

Thank you! to Ron Moore, for the question/post idea.

oMsg = "Select sketch dimensions to apply default tolerance (Press Esc to continue)"

WhileTrue

DimoDimensionAsDimensionConstraint

oDimension= ThisApplication.CommandManager.Pick(

SelectionFilterEnum.kSketchDimConstraintFilter, oMsg)

' If nothing gets selected then we're done

IfIsNothing(oDimension) ThenExitWhile

oDimension.Parameter.Tolerance.SetToSymmetric(0.05)

EndWhile

Issue:

You're writing a bit of code that might be used in Inventor documents of varying unit types. For instance maybe this code is sometimes used in inch based parts, other times it's used in millimeter based parts, and sometime centimeter based parts. Or maybe the part has some dimensions entered in inches and some entered in millimeters. In any case you want your code to handle all of this.

Recall that when we work with the API, inventor returns values in its internal units, which is always centimeters. So we often need to have our code apply a conversion factor.

Because of this you want the code to detect the units and do the conversion automatically.

Note:

If we're working with straight iLogic and no API calls, then the conversion is *often* handled for us internally in the iLogic function.

*I won't say always*

Solution:
Below is a quick example that you can use to do the units detection and conversion in your code.

Here is the basic function. It uses the document's length units and centimeters to determine the conversion factor, and displays this in a message box to return the conversion factor.

DimoUOMAsUnitsOfMeasure
oUOM = ThisDoc.Document.UnitsOfMeasure
oLenUnits = oUOM.GetStringFromType(UnitsTypeEnum.kDefaultDisplayLengthUnits)
oInvUnits = UnitsTypeEnum.kCentimeterLengthUnits
oInvUnitString = oUOM.GetStringFromType(oInvUnits)
oConversion = oUOM.ConvertUnits(1, oUOM.LengthUnits, oInvUnits)

MsgBox("Document Units = "& oLenUnits& vbLf& _
"Inventor Internal Units = "& oInvUnitString& vbLf& _
"Conversion factor = "& oConversion, , "Inventor")

And here is a quick example using it to return the value of a selected sketch dimension.
This part is set to inches (Tools tab > Document Setting button > Units tab > Length setting)

Here a sketch dimension/parameter named length is set to 70 mm, even though the part file is using Inches. And because our code is using the API to get the parameter value, we know that it's going to be returned in centimeters.

Without the conversion factor, the code returns 7, which is the value in Inventor's internal units of centimeters.








So we use the UnitsOfMeasure.ConvertUnits function to handle all of this and return the expected value in the document units. 






With the conversion code, it returns 2.756, which is the value in inches.

Here's the working example:

DimoUOMAsUnitsOfMeasure
oUOM = ThisDoc.Document.UnitsOfMeasure
oConversion = oUOM.ConvertUnits(1, oUOM.LengthUnits, _
UnitsTypeEnum.kCentimeterLengthUnits)

oMsg = "Select a sketch dimension(Press Esc to continue)"

WhileTrue
DimoDimensionAsDimensionConstraint
oDimension = ThisApplication.CommandManager.Pick(
SelectionFilterEnum.kSketchDimConstraintFilter, oMsg)

' If nothing gets selected then we're done	
IfIsNothing(oDimension) ThenExitWhile
oParam = oDimension.Parameter
oParamVal = Round(oParam.Value() / oConversion, 3)

MsgBox(oParamVal,,"Inventor")	
EndWhile

Issue:

You have a parts list that has a challenging sort criteria, due to needing to sort for values that might or might not exist in the same column.

In the example above we want to sort the description column based on all items with a mark number (MK) value, and then sort those without a mark number alphabetically.

Solution:

Although we can't accomplish this out of the box, here is a code example to this that using iLogic and some API calls.

sSortColumnName = "KEYWORDS"

' Set a reference to the drawing document.
' This assumes a drawing document is active.
DimoDrawDocAsDrawingDocument
oDrawDoc = ThisApplication.ActiveDocument

' Set a reference to the first parts list on the active sheet.
DimoPartsListAsPartsList
Try
oPartsList = oDrawDoc.ActiveSheet.PartsLists.Item(1)
Catch
Return'exit rule
EndTry

DimoADocAsAssemblyDocument
oADoc = oPartsList.ReferencedDocumentDescriptor.ReferencedDocument
DimoPropSetAsPropertySet
oPropSet = oADoc.PropertySets.Item("Inventor Summary Information")

'add temporary column to the parts list
oID = oPropSet.Item(sSortColumnName).PropId
Try
oPartsList.PartsListColumns.Add _
	(PropertyTypeEnum.kFileProperty, oPropSet.InternalName, oID)
Catch
EndTry

' Iterate through the contents of the parts list.
DimiAsLong
Fori = 1 TooPartsList.PartsListRows.Count

'get the Description value
oCell = oPartsList.PartsListRows.Item(i).Item("DESCRIPTION")

'split the string at the comma
'expecting a string like: 
'		Bracket, MK B-114
sArray = Split(oCell.Value, ",")
sType = sArray(0)

Try
sMK = sArray(1)
Catch'error when no comma in string
sMK = ""
EndTry


'get the temp column cell
oTempColumnCell = oPartsList.PartsListRows.Item(i).Item(sSortColumnName)

'write to temp column
IfsMK.Contains("MK") Then
'strip off the MK
sMK = Replace(sMK, "MK ", "")
oTempColumnCell.Value = sMK
Else
oTempColumnCell.Value = sType
EndIf
Next

'sort and renumber
oPartsList.Sort(sSortColumnName)
oPartsList.Renumber
'remove temp column
oPartsList.PartsListColumns(sSortColumnName).remove

Issue:
An update to an older post on this topic:

http://inventortrenches.blogspot.com/2013/03/turn-onoff-all-workfeatures-with-ilogic.html

Solution:
You can use this example iLogic rule to traverse the assembly (and subassemblies) to turn off all work features and sketches.

SubMain

DimoDocAsAssemblyDocument = ThisApplication.ActiveDocument
DimoOccsAsComponentOccurrences = oDoc.ComponentDefinition.Occurrences

DimsNameAsString
sName = oDoc.DisplayName

'set vis in the top level
CallSetVis(oDoc, sName)

CallTraverseAssembly(oOccs)

EndSub

SubTraverseAssembly(oOccsAsComponentOccurrences)

DimoOccAsComponentOccurrence
ForEachoOccInoOccs

DimoDocAsDocument
oDoc = oOcc.Definition.Document

DimsNameAsString
sName = oOcc.Name

'set vis in the component
CallSetVis(oOcc.Definition.Document, sName)

'if sub assembly step into it's Occurrences collection
IfoOcc.DefinitionDocumentType = _
DocumentTypeEnum.kAssemblyDocumentObjectThen
Logger.Info("Stepping into: "& sName)

oSubOccs = oDoc.ComponentDefinition.Occurrences
CallTraverseAssembly(oSubOccs)
EndIf
Next

EndSub

SubSetVis(oDocAsDocument, sNameAsString)

DimoDefAsComponentDefinition
oDef = oDoc.ComponentDefinition


ForEachoItemInoDef.Workplanes
Try
oItem.visible = False
Catch
Logger.Info("Could not set work plane vis for: "& sName)
EndTry
Next

ForEachoItemInoDef.WorkAxes
Try
oItem.visible = False
Catch
Logger.Info("Could not set work axis vis for: "& sName)
EndTry
Next

ForEachoItemInoDef.WorkPoints
Try
oItem.visible = False
Catch
Logger.Info("Could not set work point vis for: "& sName)
EndTry
Next

ForEachoItemInoDef.Sketches
Try
oItem.visible = False
Catch
Logger.Info("Could not set sketch vis for: "& sName)
EndTry
Next

EndSub

iLogic Copy Drawing Resources Autodesk Inventor

Issue:
You have drawings that you want to update with a new border, title block, sketch symbol or other Drawing Resource item.

Solution:
Here is a quick iLogic rule to do this.

oBorderName = "My Border"
oTitleBlockName = "My Title Block"
oSymbolName = "My Symbol"

oResourceFile = "C:\Temp\MyDrawingResourceFile.idw"

'open source file
DimoSourceFileAsDrawingDocument
oSourceFile = ThisApplication.Documents.Open(oResourceFile, False)

DimoDocAsDrawingDocument
oDoc = ThisDoc.Document

'copy the resources from the source file, replace existing
oSourceFile.BorderDefinitions.Item(oBorderName).CopyTo(oDoc, True)
oSourceFile.TitleBlockDefinitions.Item(oTitleBlockName).CopyTo(oDoc, True)
oSourceFile.SketchedSymbolDefinitions.Item(oSymbolName).CopyTo(oDoc, True)

'close source file
oSourceFile.Close(True)

Issue:

You would like to set the view scale of your drawing views using the predefined scale list as found at Manage tab > Styles Editor button > Standard > Standard name> General tab > Preset Values> Scale

Solution:

Here is a quick bit of code to get this list and set the scale based on the scale selected from the input list box.

( Thank you! to Zach B. for the idea for the rule)

DimoDocAsDrawingDocument = ThisApplication.ActiveDocument
DimoStyleManagerAsDrawingStylesManager = oDoc.StylesManager

DimoActiveStandardAsDrawingStandardStyle
oActiveStandard = oDoc.StylesManager.ActiveStandardStyle

DimoListAsNewList(OfString)
ForEachoItemInoActiveStandard.PresetScales
oList.Add(oItem)
Next

DimoViewAsDrawingView
oCurrentScale = oDoc.ActiveSheet.DrawingViews.Item(1).ScaleString

DimoScaleAsString = InputListBox("Select a scale", _
oList, oCurrentScale, "iLogic", "Standard Scale List")

IfString.IsNullOrWhiteSpace(oScale) ThenExitSub

ForEachoViewInoDoc.ActiveSheet.DrawingViews
IfoView.ScaleFromBase = FalseThen
oView.ScaleString = oScale
EndIf
Next

Planning to attend Autodesk University 2023 in November?

If so join me on Tuesday, November 14th as I present a practical guide to transitioning from iLogic to Inventor add-ins.

Hope to see you there!

MFG601910 | Bridging the Gap Between iLogic Automation and Inventor Add-Ins

Tuesday, Nov 1410:30 AM - 12:00 PM PST

All sessions: Sessions | AU 2023 | Autodesk University

Issue:

You'd like to be able to open a component drawing by selecting a balloon from an assembly drawing.

Solution:

Here is an iLogic rule that uses a bit of API code to do this.

DimoDocAsDrawingDocument = ThisApplication.ActiveDocumentWhileTrue'select BalloonDimoBalloonAsBalloon = NothingoBalloon = ThisApplication.CommandManager.Pick _
	(SelectionFilterEnum.kDrawingBalloonFilter, _
	"Select a balloon to open it's drawing. "& " (press ESC To Exit selection)")

	IfIsNothing(oBalloon) ThenExitWhileDimoLeaderAsLeaderIfoBalloonIsNotNothingThenoLeader = oBalloon.LeaderDimoLeaderNodeAsLeaderNode = oLeader.AllNodes(oLeader.AllNodes.Count)
	DimoIntentAsGeometryIntent = oLeaderNode.AttachedEntityDimoCurveAsDrawingCurve = oIntent.GeometryDimoOccAsComponentOccurrence = oCurve.ModelGeometry.ContainingOccurrenceDimoRefDocAsDocument = oOcc.Definition.DocumentDimoFilePathAsString = oRefDoc.FullFileName()
	DimoDrawingFilePathAsString = Left(oFilePath, Len(oFilePath) -3) & "idw"TryoDrawDoc = ThisApplication.Documents.Open(oDrawingFilePath, True)
		ExitWhileCatchMsgBox("Could not open "& oDrawingFilePath, , "iLogic")
	EndTryEndWhile

Autodesk has been wiping out old forum posts ( thousands of them 😠 ) so when I ran across this today, I thought I'd back it up here, so that we won't loose it in the next couple of years.

Credit to Pball for the instructions below.

This was originally written for Inventor 2017, I'm assuming it still works for current versions.

Use at your own risk, and all that jazz.

Original link:

https://forums.autodesk.com/t5/inventor-forum/silly-splash-screens/m-p/6774798#M625213

Here are some instructions for changing the splash screen.

I personally use Resource Hacker to modify icons and other resources in executables and dlls. http://www.angusj.com/resourcehacker/#download

Fire up resource hacker and open C:\Program Files\Autodesk\Inventor 20xx\bin\BrandRes.dll, changing 20xx for whichever version you might use

Navigate to the bitmap folder in the treeview and select the 108 entry which is the splash screen image

Then click Action and choose Save *.bmp resource and save the bitmap image somewhere

Either edit the saved image or create a new bmp with the same size and properties as the original

The click Action and choose Replace Bitmap, make sure the 108 splash screen entry is selected on the right side of the dialog and use the open file with new bitmap to select the replacement image and hit the Replace button

Hit save to save the edited dll file. (If you get an error either the file is being accessed and you need close inventor or you might need admin permissions to edit that file, save a copy of the file somewhere else and try to manually rename BrandRes.dll and copy the edited one over)

Resource Hacker will create a back up of the original file if you don't run into permission issues

Now you have a custom splash screen

Infinite Skills – Autodesk Inventor 2014 Tutorial Series

iLogic - Delete Custom iProperties

iLogic - TitleBlock Project Data From Excel

Inventor 2015 User Interface Is Missing Buttons?

iLogic: Working with the Active Sketch

iLogic - Dimension Text Scale

iLogic - Suppress Components in all but the Active Level of Detail

Determine File Type for iLogic Rule

Turn On/Off all Workfeatures with iLogic

Ilogic - Add Standard Virtual Parts From a Text File

Inventor HSM Express – The Free CAM Solution for Inventor Users – Beta Invitation

Ilogic - Add Standard Virtual Parts From an Excel File

Use 3D Solid Edges for Frame Generator Selection

iLogic: How to learn Inventor's Application Programming Interface (API)

Hybrid Wireframe and Shaded Views in Autodesk Inventor

iLogic - Dynamic MultiValue Parameter Lists "Filtered" By Current Selected Value

iLogic: Select and Set Sketch Dimension Tolerances

Inventor API: using UnitsOfMeasure.ConvertUnits

iLogic: Custom Sort PartsList with Temporary Column

Traverse Assembly to Turn Off all Work Features and Sketches with iLogic

iLogic Rule to Update Drawing Resources

iLogic : Set View Scale from Standard Preset Set List

Autodesk University 2023: Bridging the Gap Between iLogic Automation and Inventor Add-Ins, MFG601910

Open Drawing From Balloon

Hacking the Inventor startup screen