-
Re: How to select Cutlist Item and create a 3D Bounding Box
How about feature.Name?
CutItem = swfeat.Name-
Re: How to select Cutlist Item and create a 3D Bounding Box
Hi Amen,
I tried this solution, but it didn't generate a 3D Bounding Box. It didn't even give me a debug option as no errors came up.
-
-
Re: How to select Cutlist Item and create a 3D Bounding Box
Hi Raymond,
try this one:
Sub main()
Dim swApp As Object
Dim swmodel As ModelDoc2
Dim swPart As PartDoc
Dim boolstatus As Boolean
Dim swSelMgr As ISelectionMgr
Dim swBody As Body2
Dim vBodies As Variant
Dim j As Integer
Dim BodyFolder As SldWorks.BodyFolder
Dim CutListBdy As Body2
Set swApp = Application.SldWorks
Set swmodel = swApp.ActiveDoc
Set swPart = swmodel
Set swSelMgr = swmodel.SelectionManager
Set swBody = swSelMgr.GetSelectedObject6(0, -1)
Dim Feat As Feature
Set Feat = swmodel.FirstFeature
While Not Feat Is Nothing
If Feat.GetTypeName2 = "CutListFolder" Then
Dim swFeatName As String
swFeatName = Feat.Name
Feat.Select2 True, 0
Debug.Print swFeatName
Set BodyFolder = Feat.GetSpecificFeature2
vBodies = BodyFolder.GetBodies
For j = 0 To UBound(vBodies)
Set CutListBdy = vBodies(j)
Debug.Print CutListBdy.Name
swmodel.Extension.Create3DBoundingBox
Next j
End If
Set Feat = Feat.GetNextFeature()
Wend
End Sub
It is little bit messy, but it works.
It traverse thru all features, then select cutlist folders, then creates a bounding box for every body in cutlist folders.
Loop j is responsible for it, if you want to select only first item, then change this loop.
Preconditions:
Part need to have weldment feature and updated cutlist.
You can achive it, by using IbodyFolder --> UpdateCutList, and InsertWeldmentFeature Method (IFeatureManager)
I hope it will help you.
-
Re: How to select Cutlist Item and create a 3D Bounding Box
Thanks Dariusz, your solution works very well.
I added some extra lines of code as I just realised that a weldment-cut-list table would have to first exist in the FeatureManagerTree before running your macro, so I added a line of code to create a weldment table before the While Not statement.
Here is the line of code added (in BOLD) to you your solution:
.....
Set swPart = swmodel
Set swSelMgr = swmodel.SelectionManager
Set swBody = swSelMgr.GetSelectedObject6(0, -1)
Dim Feat As Feature
Set Feat = swmodel.FeatureManager.InsertWeldmentFeature() 'Insert weldment feature
Set Feat = swmodel.FirstFeature
While Not Feat Is Nothing
If Feat.GetTypeName2 = "CutListFolder" Then
.....
This successfully creates a weldment cutlist table, but it doesn't continue to process the rest of the code and create a 3D Bounding Box. When I re-run the same macro, it unusually generates multiple weldment cutlists. Any ideas why this might happen?
-
Re: How to select Cutlist Item and create a 3D Bounding Box
Raymond,
currently I have do access to my PC with Sw installed, but try this:
Delete "Set Feat =" and leave only
swmodel.FeatureManager.InsertWeldmentFeature()
or
try assign a boolean for example:
dim bool as boolean
bool = swmodel.FeatureManager.InsertWeldmentFeature()
Please check it, it it fails, i will look into it later.
-
Re: How to select Cutlist Item and create a 3D Bounding Box
I've tried assigning a boolean, but it still creates multiple weldment tables (as shown in the image) and it doesn't execute the latter part of the code. Since I've removed the 'Set Feat', I also get an object error:
-
Re: How to select Cutlist Item and create a 3D Bounding Box
Raymond, here you go (still messy, but with little bit of comments inside of code), now its working, and does not insert multiple instances of weldment feature, if part is already a weldment:
Sub main()
Dim swApp As Object
Dim swmodel As ModelDoc2
Dim swPart As PartDoc
Dim boolstatus As Boolean
Dim swSelMgr As ISelectionMgr
Dim swBody As Body2
Dim vBodies As Variant
Dim j As Integer
Dim BodyFolder As SldWorks.BodyFolder
Dim CutListBdy As Body2
Dim Feat As Feature
Dim swIsWeldment As Boolean
Set swApp = Application.SldWorks
Set swmodel = swApp.ActiveDoc
Dim bool As Boolean
Set swPart = swmodel
Set swSelMgr = swmodel.SelectionManager
Set swBody = swSelMgr.GetSelectedObject6(0, -1)
swIsWeldment = swPart.IsWeldment
If swIsWeldment = False Then 'Check if part is weldment, if not, create weldment feature
swmodel.FeatureManager.InsertWeldmentFeature
swmodel.EditRebuild3
Else
End If
Set Feat = swmodel.FirstFeature 'get first feature
While Not Feat Is Nothing
If Feat.GetTypeName2 = "CutListFolder" Then 'check that first feature is cutlistfolder
Dim swFeatName As String
Set BodyFolder = Feat.GetSpecificFeature2 'get body folder interface
BodyFolder.GetAutomaticCutList
BodyFolder.UpdateCutList
swmodel.EditRebuild3
swFeatName = Feat.Name
Feat.Select2 True, 0
Debug.Print swFeatName
vBodies = BodyFolder.GetBodies
For j = 0 To UBound(vBodies)
Set CutListBdy = vBodies(j)
Debug.Print CutListBdy.Name
swmodel.Extension.Create3DBoundingBox
Next j
End If
Set Feat = Feat.GetNextFeature()
Wend
End Sub
-
Re: How to select Cutlist Item and create a 3D Bounding Box
IsWeldment would only work if there is a weldment feature (like feature created using weldment profile).
-
Re: How to select Cutlist Item and create a 3D Bounding Box
Hi Deepark,
It appears to work very well with both extruded solids and weldment profiles.
-
Re: How to select Cutlist Item and create a 3D Bounding Box
Not sure but it was not working for me on extruded components and was adding multiple weldment feature (like you were facing earlier).
Glad to know it is working for you.
-
-
-
Re: How to select Cutlist Item and create a 3D Bounding Box
Thanks Dariusz, this is amazing. It works like a charm. I'm still learning the API as I go and this is a great learning exercise for me. I hope others might find this useful as well. Cheers.
-
-
-
-
-
