Export all Flat Patterns from iPart file to DWG with Part Number as file name.

[philip1009]

Hello to all.  I have working iLogic code that exports sheet metal flat patterns to a dwg file with the correct options needed by the programming team.  We have code elsewhere that works great with normal parts to automate the exporting process.

Here's the code as of now:

SyntaxEditor Code Snippet

Dim oDoc As PartDocument
oDoc=ThisApplication.ActiveDocument
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=oDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim sFname As String
sFname=oDoc.FullFileName
sFname=Left$(sFname,Len(sFname)-3)&"dwg"
oCompDef.DataIO.WriteDataToFile(sOut,sFname)

The problem is when it exports a flat pattern from an iPart file it, of course, reads the file name such as "PANELS" instead of the iProperties Part Number such as "ST9".

How do I change the code so that it saves the dwg file with the name from the Part Number instead of the File Name?

I've tried simply changing the code to this:

SyntaxEditor Code Snippet

Dim oDoc As PartDocument
oDoc=ThisApplication.ActiveDocument
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=oDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim sFname As String
sFname=iProperties.Value("Project", "Part Number")&".dwg"
oCompDef.DataIO.WriteDataToFile(sOut,sFname)

But all I get is the typical HRESULT fail code which doesn't tell me anything.  I've also tried using the Convert to String code like below:

SyntaxEditor Code Snippet

sFname=CStr(iProperties.Value("Project", "Part Number"))&".dwg"

But that doesn't work either, if I can get a solution on this that would save the step of having to rename each export one at a time, that would be awesome.

My second request would be to add code to automatically do these steps for every member in the iPart table instead having to run the code, change the iPart member, then run the code again for every member.

Thanks so much in advance, I've learned plenty about iLogic in the past few months, it's just the little details here and there that trip me up.

[MechMachineMan]

Hi,

Likely what you need to do is access the document's component definition, check isiPartmember, then iterate through the rows using the available function calls. You will be able to use the changerow call to swap through each iPart, and use the .Row property to grab the part number for that item.

http://help.autodesk.com/view/INVNTOR/2018/ENU/?guid=GUID-FE230CC1-D9A7-4050-9018-2BBE35941067

or it might be the same, but using the iPart factory things. Not too familiar with anything else, but you should be able to find some samples within the programming help resources.

[philip1009]

There is a code sample that's supposed to get the value Part Number:

SyntaxEditor Code Snippet

Public Sub GetPropertySample()
    ' Get the active document.
    Dim invDoc As Document
    Set invDoc = ThisApplication.ActiveDocument
    
    ' Get the design tracking property set.
    Dim invDesignInfo As PropertySet
    Set invDesignInfo = invDoc.PropertySets.Item("Design Tracking Properties")
    
    ' Get the part number property.
    Dim invPartNumberProperty As Property
    Set invPartNumberProperty = invDesignInfo.Item("Part Number")
    
    MsgBox "Part Number: " & invPartNumberProperty.Value
End Sub

I tried to put it in my code below:

SyntaxEditor Code Snippet

Dim oDoc As PartDocument
oDoc=ThisApplication.ActiveDocument
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=oDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim invDesignInfo As PropertySet
invDesignInfo=oDoc.PropertySets.Item("Design Tracking Properties")
Dim invPartNumberProperty As Property
invPartNumberProperty=invDesignInfo.Item("Part Number")
Dim sFname As String
sFname=invPartNumberProperty & ".dwg"
oCompDef.DataIO.WriteDataToFile(sOut,sFname)

But I get an error on Line 22 (Dim invPartNumberProperty As Property) that says:

Keyword does not name a type.

I am lost on what this means.  I also noticed that when I type in "Property" it turns red and begins an outline ticker, is that what's causing the Keyword error?  Am I supposed to close this with a "End Property" line or something.  It honestly should not be this difficult to get the Part Number into an object or string so I can use it as the file name when I export the dwg.

[MechMachineMan]

Dim oDoc As PartDocument
oDoc=ThisApplication.ActiveDocument
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=oDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim invDesignInfo As PropertySet
invDesignInfo=oDoc.PropertySets.Item("Design Tracking Properties")
Dim invPartNumberProperty As Inventor.Property
invPartNumberProperty=invDesignInfo.Item("Part Number")
Dim sFname As String
sFname=invPartNumberProperty.Value & ".dwg"
oCompDef.DataIO.WriteDataToFile(sOut,sFname)
oCompDef.ExitEdit

[philip1009]

Thanks for the reply, I tried your fix and it generates another error I haven't seen before:

Error Message:

Error in rule: FLAT PATTERN DWG OUT, in document: B-PANELS.ipt

Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))

More Info:

System.Runtime.InteropServices.COMException (0x80004005): Unspecified error (Exception from HRESULT: 0x80004005 (E_FAIL))
at System.RuntimeType.ForwardCallToInvokeMember(String memberName, BindingFlags flags, Object target, Int32[] aWrapperTypes, MessageData& msgData)
at Inventor.DataIO.WriteDataToFile(String Format, String FileName)
at LmiRuleScript.Main()
at Autodesk.iLogic.Exec.AppDomExec.ExecRuleInAssembly(Assembly assem)
at iLogic.RuleEvalContainer.ExecRuleEval(String execRule)

I found a blog, http://modthemachine.typepad.com/my_weblog/2010/02/accessing-iproperties.html

In the middle it shows some sample code where it dims Property Sets before dimming the Property Set, then finally the Property Itself:

SyntaxEditor Code Snippet

 ' Get the active document. 
    Dim oDoc As Document 
    Set oDoc = ThisApplication.ActiveDocument 

    ' Get the PropertySets object. 
    Dim oPropSets As PropertySets 
    Set oPropSets = oDoc.PropertySets 

    ' Get the design tracking property set. 
    Dim oPropSet As PropertySet 
    Set oPropSet = oPropSets.Item("Design Tracking Properties") 

    ' Get the part number iProperty. 
    Dim oPartNumiProp As Property 
    Set oPartNumiProp = oPropSet.Item("Part Number") 

So I tried to insert that step in with the code you provided and came up with this:

SyntaxEditor Code Snippet

Dim oDoc As PartDocument
oDoc=ThisApplication.ActiveDocument
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=oDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim invPropSets As PropertySets 
invPropSets=oDoc.PropertySets 
Dim invPropSet As PropertySet 
invPropSet=invPropSets.Item("Design Tracking Properties") 
Dim invPartNumiProp As Inventor.Property 
invPartNumiProp=invPropSet.Item("Part Number")
Dim sFname As String
sFname=invPartNumiProp.Value & ".dwg"
oCompDef.DataIO.WriteDataToFile(sOut, sFname)
oCompDef.ExitEdit

But it gives the same error code as above, I'll keep digging around for the solution, thanks so much for your help.

I've attached the part file to this reply, please feel free to use it to test your code, I'm sure the solution will be found soon.

Cheers. 

[MechMachineMan]

This code worked fine for me!

Dim oDoc As PartDocument
oDoc=ThisApplication.ActiveDocument

Dim oCompDef As SheetMetalComponentDefinition
oCompDef=oDoc.ComponentDefinition

Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO

Dim oFlatPattern As SheetmetalComponentDefinition

If oCompDef.HasFlatPattern=False Then
	oCompDef.Unfold
Else
	oCompDef.FlatPattern.Edit
End If

Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"

Dim oPN As String
oPN=oDoc.PropertySets.Item("Design Tracking Properties").Item("Part Number").Value

Dim sPath As String
Dim sFname As String
sPath = "C:\Users\Public\Documents\"
sFname= sPath & oPN & ".dwg"

oCompDef.DataIO.WriteDataToFile(sOut, sFname)
oCompDef.FlatPattern.ExitEdit

[philip1009 · Accepted solution]

Okay, then the issue was when the original code was pulling oDoc.FullFileName, it was pulling the full file path as well, and we didn't put that back and put the Part Number and file type behind that, the code didn't know where to save the file.  So we just need to add in a line of code to get the file path and add that to sFname:

SyntaxEditor Code Snippet

Dim oDoc As PartDocument
oDoc=ThisApplication.ActiveDocument
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=oDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim invPropSets As PropertySets 
invPropSets=oDoc.PropertySets 
Dim invPropSet As PropertySet 
invPropSet=invPropSets.Item("Design Tracking Properties") 
Dim invPartNumiProp As Inventor.Property 
invPartNumiProp=invPropSet.Item("Part Number")
Dim sFname As String
sFname=ThisDoc.Path & "\" & invPartNumiProp.Value & ".dwg"
oCompDef.DataIO.WriteDataToFile(sOut, sFname)
oCompDef.FlatPattern.ExitEdit

Thanks for your help.

[karipates6709]

Is this automatically generating the flat patterns on save or anything like that? or could it be programmed to do that? just kinda curious thanks.

[MechMachineMan]

Sure.

Ensure you have 2018.1 installed.

Add this to the Event Triggers under Part Documents.

Add some extra lines to make sure it is only exporting them for flat patterns, and not HSS cuts or round bar, or other weird parts and you will be good to go.

[karipates6709]

we are not currently running 2018, but that will change in a couple months. I will bring this to everyone's attention though. thank you for letting me know.

[philip1009 · Accepted solution]

You don't need 2018 for Event Triggers.

For running the code on save, just go to the iLogic section under the Manage tab and click on Event Triggers, then right-click on After Save Document, Select Rules, and then check the box next to the rule you want.

Depending on your needs, if you need the file in DXF format instead of DWG, all you have to do is change the DWG references in the lines

SyntaxEditor Code Snippet

sOut="FLAT PATTERN DWG?AcadVersion=2000" _

And

SyntaxEditor Code Snippet

sFname=ThisDoc.Path &"\"&invPartNumiProp.Value &".dwg"

 to "DXF" and ."dxf" appropriately and it will work as well.

If you're interested in a process that will export all flat patterns in one process, here's the code that's used in an assembly file that has all sheet metal parts placed, it doesn't require the previous code to be placed in each sheet metal part, so this will work with any sheet metal part placed as long as there is a flat pattern that can be generated without errors.  This also works with iParts for those who use them.

It's a great time saver that did about 80 parts, normal and iParts combined, in a few minutes instead of a few hours when done manually.

SyntaxEditor Code Snippet

Dim oDoc As Document
oDoc=ThisDoc.Document
Dim docFile As Document
For Each docFile In oDoc.AllReferencedDocuments
ThisApplication.Documents.Open(docFile.FullFileName,True)
Dim partDoc As PartDocument
partDoc=ThisApplication.ActiveDocument
If partDoc.SubType="{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=partDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim invPropSets As PropertySets
invPropSets=partDoc.PropertySets
Dim invPropSet As PropertySet
invPropSet=invPropSets.Item("Design Tracking Properties")
Dim invPartNumiProp As Inventor.Property
invPartNumiProp=invPropSet.Item("Part Number")
Dim sFname As String
sFname=ThisDoc.Path &"\"&invPartNumiProp.Value &".dwg"
oCompDef.DataIO.WriteDataToFile(sOut,sFname)
oCompDef.FlatPattern.ExitEdit
If partDoc.ComponentDefinition.IsiPartFactory Or
partDoc.ComponentDefinition.IsiPartMember Then
partDoc.Save()
End If
Else
End If
partDoc.Close
Next

[Anonymous]

---

@philip1009wrote:

You don't need 2018 for Event Triggers.

For running the code on save, just go to the iLogic section under the Manage tab and click on Event Triggers, then right-click on After Save Document, Select Rules, and then check the box next to the rule you want.

Depending on your needs, if you need the file in DXF format instead of DWG, all you have to do is change the DWG references in the lines

SyntaxEditor Code Snippet

sOut="FLAT PATTERN DWG?AcadVersion=2000" _

And

SyntaxEditor Code Snippet

sFname=ThisDoc.Path &"\"&invPartNumiProp.Value &".dwg"

 to "DXF" and ."dxf" appropriately and it will work as well.

If you're interested in a process that will export all flat patterns in one process, here's the code that's used in an assembly file that has all sheet metal parts placed, it doesn't require the previous code to be placed in each sheet metal part, so this will work with any sheet metal part placed as long as there is a flat pattern that can be generated without errors.  This also works with iParts for those who use them.

It's a great time saver that did about 80 parts, normal and iParts combined, in a few minutes instead of a few hours when done manually.

SyntaxEditor Code Snippet

Dim oDoc As Document
oDoc=ThisDoc.Document
Dim docFile As Document
For Each docFile In oDoc.AllReferencedDocuments
ThisApplication.Documents.Open(docFile.FullFileName,True)
Dim partDoc As PartDocument
partDoc=ThisApplication.ActiveDocument
If partDoc.SubType="{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
Dim oCompDef As SheetMetalComponentDefinition
oCompDef=partDoc.ComponentDefinition
Dim oDataIO As DataIO
oDataIO=oDoc.ComponentDefinition.DataIO
If oCompDef.HasFlatPattern=False Then
oCompDef.Unfold
Else
oCompDef.FlatPattern.Edit
End If
Dim sOut As String
sOut="FLAT PATTERN DWG?AcadVersion=2000" _
+"&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_ALTREP_FRONT;IV_ALTREP_BACK;IV_UNCONSUMED_SKETCHES;IV_ROLL_TANGENT;IV_ROLL" _
+"&SimplifySplines=True" _
+"&LINEAR TOLERANCE=0.010" _
+"&MergeProfilesIntoPolyline=True" _
+"&RebaseGeometry=False" _
+"&TrimCenterlines=True"
Dim invPropSets As PropertySets
invPropSets=partDoc.PropertySets
Dim invPropSet As PropertySet
invPropSet=invPropSets.Item("Design Tracking Properties")
Dim invPartNumiProp As Inventor.Property
invPartNumiProp=invPropSet.Item("Part Number")
Dim sFname As String
sFname=ThisDoc.Path &"\"&invPartNumiProp.Value &".dwg"
oCompDef.DataIO.WriteDataToFile(sOut,sFname)
oCompDef.FlatPattern.ExitEdit
If partDoc.ComponentDefinition.IsiPartFactory Or
partDoc.ComponentDefinition.IsiPartMember Then
partDoc.Save()
End If
Else
End If
partDoc.Close
Next

---

Would we be able to make this export the dxf without the bend lines? This ran flawlessly other that having bend lines on the dxf. 

---

---

Also I am pretty green (very new) to ilogic and was wondering how to save a rule so you can use it from any file without having to rewrite it. 

[Anonymous]

Hello phillip1009

I'm running your code [Inventor 2018] (copy-paste) and it only generates the iPart member selected.

What about the other ones?

I don't see (not that I know what to look for...) the lines that jump from member to member to save the next flat patterns.

Can you explain/help?

I also need to mention that i haven't been able to save iLogic rules as an external rule (to be used on other files) due to my lack of knowledge and / or the poor user interface of the whole iLogic world.

Thanks

[philip1009]

It sounds like you're trying to export from an iPart Master file, correct?

This code was meant to peruse all files in an assembly file and find sheet metal flats to export, my quick advice would be insert all of your generated iPart files into an assembly saved in the folder you want the flat exports saved to, then run the code.

Otherwise it's a different code to run through the list iPart Members in a Master file.

[Anonymous]

Hello phillip1009,

You are correct.

I will have to make it...

...or have it made...

Thanks,

Octavio