solidworks零件批量导出CAD展开图宏文件

求可以直接通过零件转为CAD的展开图宏，
不需要转为工程图

最好可以标识厚度

735057167 发表于 2020-2-26 17:06
判断厚度的代码我有了，就差零件自动转为cad的代码

以下代码为API VBA源码，在下部倒数第二个参数是钣金输出选项，参见API帮助。以下代码略加修改可以做成批量处理工具。我用VB.NET写的代码给你应该没什么用如下图。


VBA代码：

1. Option Explicit
   
2. 
   
3. Dim swApp As SldWorks.SldWorks
   
4. Dim swModel As SldWorks.ModelDoc2
   
5. Dim swPart As SldWorks.PartDoc
   
6. Dim sModelName As String
   
7. Dim sPathName As String
   
8. Dim varAlignment As Variant
   
9. Dim dataAlignment(11) As Double
   
10. Dim varViews As Variant
    
11. Dim dataViews(1) As String
    
12. Dim options As Long
    
13. 
    
14. Sub main()
    
15.     Set swApp = Application.SldWorks
    
16.     Set swModel = swApp.ActiveDoc   
    
17.     sModelName = swModel.GetPathName
    
18.     sPathName = swModel.GetPathName
    
19.     sPathName = Left(sPathName, Len(sPathName) - 6)
    
20.     sPathName = sPathName + "dwg"   
    
21. 
    
22.     Set swPart = swModel   
    
23. 
    
24.     dataAlignment(0) = 0#
    
25.     dataAlignment(1) = 0#
    
26.     dataAlignment(2) = 0#
    
27.     dataAlignment(3) = 1#
    
28.     dataAlignment(4) = 0#
    
29.     dataAlignment(5) = 0#
    
30.     dataAlignment(6) = 0#
    
31.     dataAlignment(7) = 1#
    
32.     dataAlignment(8) = 0#
    
33.     dataAlignment(9) = 0#
    
34.     dataAlignment(10) = 0#
    
35.     dataAlignment(11) = 1#   
    
36. 
    
37.     varAlignment = dataAlignment   
    
38. 
    
39.     dataViews(0) = "*Current"
    
40.     dataViews(1) = "*Front"   
    
41. 
    
42.     varViews = dataViews   
    
43. 
    
44.     'Export each annotation view to a separate drawing file
    
45.     swPart.ExportToDWG2 sPathName, sModelName, swExportToDWG_ExportAnnotationViews, False, varAlignment, False, False, 0, varViews
    
46.    
    
47.     'Export sheet metal to a single drawing file
    
48.     options = 1   'include flat-pattern geometry
    
49.     swPart.ExportToDWG2 sPathName, sModelName, swExportToDWG_ExportSheetMetal, True, varAlignment, False, False, options, Null
    
50. 
    
51. End Sub

复制代码

可以，判断厚度，最好是钣金零件，
Value = Part.ExportFlatPatternView(MyFileNameDXF, swExportFlatPatternOption_None) '保留折弯线
value = Part.ExportFlatPatternView(FilePath, swExportFlatPatternOption_RemoveBends)'去掉折弯线

有转cad代码就够了

yx1991 发表于 2020-2-26 10:54
可以，判断厚度，最好是钣金零件，
Value = Part.ExportFlatPatternView(MyFileNameDXF, swExportFlatPatt ...

判断厚度的代码我有了，就差零件自动转为cad的代码

wenmk 发表于 2020-2-26 21:46
以下代码为API VBA源码，在下部倒数第二个参数是钣金输出选项，参见API帮助。以下代码略加修改可以做成批 ...

这个可以，谢谢

yx1991 发表于 2020-2-26 10:54
可以，判断厚度，最好是钣金零件，
Value = Part.ExportFlatPatternView(MyFileNameDXF, swExportFlatPatt ...

这个代码知道怎么用，直接加上会出错

735057167 发表于 2020-2-27 11:47
这个代码知道怎么用，直接加上会出错

哪里出错，可以说出来我们讨论下，楼上发的那个代码适合选择面然后输出CAD格式那样会好点

yx1991 发表于 2020-2-27 13:27
哪里出错，可以说出来我们讨论下，楼上发的那个代码适合选择面然后输出CAD格式那样会好点

已经解决了取得厚度代码附

1. Option Explicit
   
2. Sub thiness0()
   
3.     Dim swApp As SldWorks.SldWorks
   
4.     Dim swModel As SldWorks.ModelDoc2
   
5.     Dim swPart As SldWorks.PartDoc
   
6.     Dim i As Long
   
7.     Dim swFeatMgr As FeatureManager
   
8.     Dim swFeat As Feature
   
9.     Dim swSheetMetalFol As SheetMetalFolder
   
10.     Dim swSheetFeatData As SheetMetalFeatureData
    
11.     Dim swBaseFlangeFeatData As BaseFlangeFeatureData
    
12.     Dim vSheetMetalFeat As Variant
    
13.     Dim ThicknessM As String
    
14.     Dim Path As String
    
15.     Dim sModelName As String
    
16.     Dim sPathName As String
    
17.     Dim varAlignment As Variant
    
18.     Dim dataAlignment(11) As Double
    
19.     Dim options As Long
    
20.   
    
21.     Set swApp = Application.SldWorks
    
22.     Set swModel = swApp.ActiveDoc
    
23.     Set swFeatMgr = swModel.FeatureManager
    
24.     Set swSheetMetalFol = swFeatMgr.GetSheetMetalFolder
    
25.   
    
26.     If Not swSheetMetalFol Is Nothing Then
    
27.         vSheetMetalFeat = swSheetMetalFol.GetSheetMetals
    
28.         For i = 0 To UBound(vSheetMetalFeat)
    
29.             Set swFeat = vSheetMetalFeat(i)
    
30.             If swFeat.GetTypeName2 = "SheetMetal" Then
    
31.                 Set swSheetFeatData = swFeat.GetDefinition
    
32.               Exit For
    
33.             End If
    
34.         Next i
    
35.     Else
    
36.         Set swFeat = swModel.FirstFeature
    
37.         Do While Not swFeat Is Nothing
    
38.             If swFeat.GetTypeName2 = "SMBaseFlange" Then
    
39.                 Set swBaseFlangeFeatData = swFeat.GetDefinition
    
40.                 Exit Do
    
41.             ElseIf swFeat.GetTypeName2 = "SheetMetal" Then
    
42.                 Set swSheetFeatData = swFeat.GetDefinition
    
43.                 Exit Do
    
44.             End If
    
45.             Set swFeat = swFeat.GetNextFeature
    
46.         Loop
    
47.     End If
    
48.     ThicknessM = swSheetFeatData.Thickness * 1000
    
49.    C = ThicknessM
    
50.   C = "（T=" & C & "mm）"
    
51. msgbox c
    
52. End Sub
    

复制代码

735057167 发表于 2020-2-29 23:26
已经解决了取得厚度代码附

我运行此楼代码    提示编译错误变量未定义，能否上传  .swp附件  谢谢