Inserting ACAD DFX into Sketch of a part file

[Daan_M]

Hi,

I'm trying to insert a DFX file into a sketch of a part file, Unfortunatly not everything in my DFX file appears.

I think some layers are missing or something.

Here is my DFX when i open it

Here is the result in the Part file

Code;

Dim oLaserTemplateLoc = "Partfile.ipt"
Dim oPart As PartDocument = ThisApplication.Documents.Open(oLaserTemplateLoc, True)
oPart.Activate
Dim oPCD As PartComponentDefinition = oPart.ComponentDefinition

Dim oDXFTranslator As TranslatorAddIn
    oDXFTranslator = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}") 

    Dim oDataMedium As DataMedium
    oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
    oDataMedium.FileName = "DFX Location"
 
    Dim oTranslationContext As TranslationContext
    oTranslationContext = ThisApplication.TransientObjects.CreateTranslationContext
    oTranslationContext.Type = kFileBrowseIOMechanism
    
	Dim oPlaneXZ As WorkPlane = oPCD.WorkPlanes.Item(2) 
    Dim oSketch As PlanarSketch
    oSketch = oPCD.Sketches.Add(oPlaneXZ)

    oSketch.Edit
    oTranslationContext.OpenIntoExisting = oSketch
    Dim oOptions As NameValueMap
    oOptions = ThisApplication.TransientObjects.CreateNameValueMap
    oOptions.Add ("FileUnits", "Millimeters")
    Call oDXFTranslator.Open(oDataMedium, oTranslationContext, oOptions, oPart)
	oSketch.ExitEdit

[JelteDeJong]

I could not test this but you might have some luck with the DWG import options. According to help, there is the option "SelectedLayers ". This specifies the layer names to import. The names are comma delimited. 

https://help.autodesk.com/view/INVNTOR/2023/ENU/?guid=GUID-25D24E28-7517-4903-8AEE-123F8C71A89E&v=In...

Dim oLaserTemplateLoc = "Partfile.ipt"
Dim oPart As PartDocument = ThisApplication.Documents.Open(oLaserTemplateLoc, True)
oPart.Activate
Dim oPCD As PartComponentDefinition = oPart.ComponentDefinition

Dim oDXFTranslator As TranslatorAddIn
    oDXFTranslator = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}") 

    Dim oDataMedium As DataMedium
    oDataMedium = ThisApplication.TransientObjects.CreateDataMedium
    oDataMedium.FileName = "DFX Location"
 
    Dim oTranslationContext As TranslationContext
    oTranslationContext = ThisApplication.TransientObjects.CreateTranslationContext
    oTranslationContext.Type = kFileBrowseIOMechanism
    
	Dim oPlaneXZ As WorkPlane = oPCD.WorkPlanes.Item(2) 
    Dim oSketch As PlanarSketch
    oSketch = oPCD.Sketches.Add(oPlaneXZ)

    oSketch.Edit
    oTranslationContext.OpenIntoExisting = oSketch
    Dim oOptions As NameValueMap
    oOptions = ThisApplication.TransientObjects.CreateNameValueMap
    oOptions.Add ("FileUnits", "Millimeters")
    oOptions.Add ("SelectedLayers", "YOUR,LAYER,NAMES,HERE")
    Call oDXFTranslator.Open(oDataMedium, oTranslationContext, oOptions, oPart)
	oSketch.ExitEdit

[Daan_M]

@JelteDeJong Thank you for the advice.

I added the following line in my code, but still only the text gets added onto the .ipt file and not the lines:

oOptions.Add ("SelectedLayers", "0")

When i check the .dwg, the layer with lines should be "0"?

The same goes for the text:

I attached my .dwg file.

Curious what i'm doing wrong

[JelteDeJong · Accepted solution]

In your OP you wrote that you wanted to import a DXF. But you posted a DWG file. On closer inspection, I discovered that the options that you use are also for DWG files. But the GUID is for the DXF translator (I did not see any import options for the DXF translator btw.) Anyway, if you want to import DWG files you need to use a different GUID.  This iLogic rule worked for me.

 Dim oDXFTranslator As TranslatorAddIn = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC2-122E-11D5-8E91-0010B541CD80}") 
'Dim oDXFTranslator As TranslatorAddIn = ThisApplication.ApplicationAddIns.ItemById("{C24E3AC4-122E-11D5-8E91-0010B541CD80}")

Dim oPart As PartDocument = ThisDoc.Document
Dim oPCD As PartComponentDefinition = oPart.ComponentDefinition

Dim oPlaneXZ As WorkPlane = oPCD.WorkPlanes.Item(2)
Dim oSketch As PlanarSketch = oPCD.Sketches.Add(oPlaneXZ)
oSketch.Edit()

Dim oDataMedium As DataMedium = ThisApplication.TransientObjects.CreateDataMedium
oDataMedium.FileName = "D:\forum\Laserding.dwg"

Dim oTranslationContext As TranslationContext = ThisApplication.TransientObjects.CreateTranslationContext
oTranslationContext.Type = kFileBrowseIOMechanism
oTranslationContext.OpenIntoExisting = oSketch

Dim oOptions As NameValueMap = ThisApplication.TransientObjects.CreateNameValueMap
oOptions.Add("SelectedLayers", "0")
oOptions.Add("InvertLayersSelection", True)
oOptions.Add("FileUnits", "Centimeters")
oOptions.Add("ConstrainEndPoints", True)


oDXFTranslator.Open(oDataMedium, oTranslationContext, oOptions, oDoc)
oSketch.ExitEdit()