dxf

[Anonymous]

I have created a simple model of a web (gusset) . A  2d drawing has also been created (idw).  Its my intention to send this to the sheet metal fabricators to enable them to laser cut the web from sheet steel.

In autocad 2d this would be done by creating a dxf file and sending that to the fabricator,the question is now,

using inventor does this process still work and which needs to be converted to a dxf ie the. ipt or the .idw

Any suggestions please

[mdavis22569]

yes it's very possible...

here is a Inventor Link

https://knowledge.autodesk.com/support/inventor-products/learn-explore/caas/CloudHelp/cloudhelp/2014...

here is a link to a quite a few ways to do it..

https://www.google.com/webhp?sourceid=chrome-instant&ion=1&espv=2&ie=UTF-8#q=dxf%20sheetmetal%20inve...

[Cadmanto · Accepted solution]

DXF, is definately a method you could use.  My suggestion would be to contact the manufacturer of these parts and see if they can work from a model transfer file like iges or step.  Then you can export out your model into one of these formats and give that to them.  With the model you can export the flat pattern and maybe if they have a burn table can use that.

If this solved your issue please mark this posting "Accept as Solution".

Or if you like something that was said and it was helpful, Kudos are appreciated. Thanks!!!! 

     

[brendan.henderson · Accepted solution]

It's pretty simple to create the DXF at the part (model) level and send that to the laser burner. Below is some VB(A) some that I use to create the DXF file. Depending on the version of Inventor your on it may need some subtle changes. SOmeone on the forum will assist you with that :-

Sub FP2DXF()

Dim oPartDoc As Document
Set oPartDoc = ThisApplication.ActiveDocument

' The Active document must be a part
If oPartDoc.DocumentType <> kPartDocumentObject Then
MsgBox "The Active document must be a 'Part'"
Exit Sub
End If

' The Active document must be a Sheet metal Part
If oPartDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
MsgBox "The Active document must be a 'Sheet Metal Part'"
Exit Sub
End If

' Check if part needs to be saved
If oPartDoc.Dirty = True Then
MsgBox "Please save this Sheet metal part"
Exit Sub
End If

Dim oFlatPattern As FlatPattern
Set oFlatPattern = oPartDoc.ComponentDefinition.FlatPattern

Dim Issue As String
Issue = oPartDoc.PropertySets.Item("Summary Information").Item("Revision Number").Value

' There must be a flat pattern
If oFlatPattern Is Nothing Then
MsgBox "Please create the flat pattern"
Exit Sub
End If

Dim oDXFfileNAME As String
oDXFfileNAME = Left(oPartDoc.FullFileName, Len(oPartDoc.FullFileName) - 4) & "-" & Issue & ".DXF"

Dim oDataIO As DataIO
Set oDataIO = oPartDoc.ComponentDefinition.DataIO

Dim sOut As String

sOut = "FLAT PATTERN DXF?AcadVersion=2000" _
+ "&OuterProfileLayer=OUTER_PROF&OuterProfileLayerColor=255;0;0" _
+ "&InteriorProfilesLayer=INNER_PROFS&InteriorProfilesLayerColor=0;255;255" _
+ "&FeatureProfileLayer=FEATURE&FeatureProfileLayerColor=0;0;255" _
+ "&InvisibleLayers=IV_TANGENT;IV_BEND;IV_BEND_DOWN;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS;IV_FEATURE_PROFILES"
'+ "&BendUpLayer=BEND_UP&BendUpLayerColor=255;0;255&BendUpLayerLineType=37634" _
'+ "&BendDownLayer=BEND_DOWN&BendDownLayerColor=255;255;0&BendDownLayerLineType=37634" _
'+ "&SimplifySplines=True&MergeProfilesIntoPolyline=True" _
'+ "&InvisibleLayers=IV_TANGENT;IV_TOOL_CENTER;IV_TOOL_CENTER_DOWN;IV_ARC_CENTERS"

oDataIO.WriteDataToFile sOut, oDXFfileNAME

' &SplineTolerance=0,1 // Bruges hvis der ønsken lavere opløsning

'Below added by BH 06-12-2010

' Check for a non-part document
If oPartDoc.DocumentType <> kPartDocumentObject Then
MsgBox "The Active document must be a 'Part'"
Exit Sub
End If

' The Active document must be a Sheet metal Part
If oPartDoc.SubType <> "{9C464203-9BAE-11D3-8BAD-0060B0CE6BB4}" Then
MsgBox "The 'Part' must be a Sheet Metal Part"
Exit Sub
End If

Dim oSheetMetalCompDef As SheetMetalComponentDefinition
Set oSheetMetalCompDef = oPartDoc.ComponentDefinition

' Get the cut length
Dim oFace As Face
Set oFace = oSheetMetalCompDef.FlatPattern.TopFace

' Find the outer loop.
Dim dOuterLength As Double
dOuterLength = 0
Dim oLoop As EdgeLoop
For Each oLoop In oFace.EdgeLoops
If oLoop.IsOuterEdgeLoop Then
Dim oEdge As Edge
For Each oEdge In oLoop.Edges
' Get the length of the current edge.
Dim dMin As Double, dMax As Double
Call oEdge.Evaluator.GetParamExtents(dMin, dMax)
Dim dLength As Double
Call oEdge.Evaluator.GetLengthAtParam(dMin, dMax, dLength)
dOuterLength = dOuterLength + dLength
Next
'MsgBox "Outer Loop is " & FormatNumber(dOuterLength, 1)
Exit For
End If
Next

' Iterate through the inner loops.
Dim iLoopCount As Long
iLoopCount = 0
Dim dTotalLength As Double
For Each oLoop In oFace.EdgeLoops
Dim dLoopLength As Double
dLoopLength = 0
If Not oLoop.IsOuterEdgeLoop Then
For Each oEdge In oLoop.Edges
' Get the length of the current edge.
Call oEdge.Evaluator.GetParamExtents(dMin, dMax)
Call oEdge.Evaluator.GetLengthAtParam(dMin, dMax, dLength)
dLoopLength = dLoopLength + dLength
Next

' Add this loop to the total length.
dTotalLength = dTotalLength + dLoopLength
'MsgBox "Inner Loops are " & FormatNumber(dTotalLength, 1)
End If
Next

'Dim oUom As UnitsOfMeasure
'Set oUom = oPartDoc.UnitsOfMeasure

'outerCutlength = oUom.GetStringFromValue(dOuterLength, kMillimeterLengthUnits)
'innerCutlength = oUom.GetStringFromValue(dTotalLength, kMillimeterLengthUnits)
'TotalCutLength = oUom.GetStringFromValue(dTotalLength + dOuterLength, kMillimeterLengthUnits)

'Write data to properties, creating or updating (if property exists)
'Dim oCustomPropSet As PropertySet
'Set oCustomPropSet = oPartDoc.PropertySets.Item("{D5CDD505-2E9C-101B-9397-08002B2CF9AE}")

'On Error Resume Next
'oCustomPropSet.Item("OuterPerimeter").Value = outerCutlength
'If Err Then
'Err.Clear
'Call oCustomPropSet.Add(outerCutlength, "OuterPerimeter")
'End If
'oCustomPropSet.Item("InnerPerimeters").Value = innerCutlength
'If Err Then
'Err.Clear
'Call oCustomPropSet.Add(innerCutlength, "InnerPerimeters")
'End If
'oCustomPropSet.Item("TotalPerimeter").Value = TotalCutLength
'If Err Then
'Err.Clear
'Call oCustomPropSet.Add(TotalCutLength, "TotalPerimeter")
'End If
End Sub