Anyone have a macro to link all drawing views back to a BOM that has been replaced on sheet 1. My guys like to swap out BOM, but sometime they don't re-link the BOM after they load a new one. I have some assemblies that are 5-12 sheets long and can be as many as 30-40 views. Manually linking them is very tedious.
Try this.......
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim vSheetNames() As String
Dim swView As SldWorks.View
Dim i As Integer
Dim sName As String
Sub main()
sName = "Bill of Materials1" 'Name of BOM table
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swDraw = swModel
vSheetNames = swDraw.GetSheetNames
Set swView = swDraw.GetFirstView
For i = 0 To UBound(vSheetNames)
swDraw.ActivateSheet vSheetNames(i)
Set swView = swDraw.GetFirstView
Do While Not swView Is Nothing
swView.SetKeepLinkedToBOM True, sName
Set swView = swView.GetNextView
Loop
Next
End Sub
Try this one. It doesn't need to know the name of the BOM. It will automatically find it.
What if you have a bom and a weldment cutlist?
looks good however "Bill of Materials1" might not always be the correct name
In my case i never have a weldment cut list and assembly BOM in the same Drawing.
Deepak, I believe i adapted this macro from your work so thank you for sharing it.
Tony, I modified Deepak original code to traverse through the feature manager tree and find the BOM. In API a BOM and a weldment cutlist are different. The code should automatically find the name of only the BOM.
Now, if there are multiple BOMs in your drawing that is another story.
Matt,
that one works great.
As a side question...how easy would it be to populate a list of all the BOMS in a drawing (if multiple) and select which to link to.
Matt's macro works in 95% of my application but in the other i have a parts only on the first page and the second page may contain a top level. Depending on the situation i could want one or the other....
For my direct application, Matt's Fills the gap...AWESOME
A user form would probably be the way to go to get a list to select from. But the easier way may be to have the user select the correct BOM in the feature tree and use code to get the name of the selected BOM. You could also have the code send up a prompt if they didn't have a BOM selected.
I use the bom on sheet 1 and a cutlist when detailing weldments on following sheets.
Matt,
Will this update all sheets at once... or does the macro need to be run on all sheets separately...
I'm not sure because I only deal in one sheet drawings and so I have never tested it on a multiple sheet drawing. Base on the code and how it traverses the drawing views I think it should do all views on all sheets.
Here is updated macro to work on all sheets.
Thanks Deepak Gupta.
I have the same problem, but I have many Bills of Materials per Drawing, is there anyway I can run the macro on one sheet, and have me select from the BoM's available?
Do you mean more than one BOM on one sheet?
No. Just more than one Bill of Materials per drawing.
Joseph Caswell wrote:
No. Just more than one Bill of Materials per drawing.
More than one BOM per drawing is fine but are there more than one BOM on same sheet?
There is not.
Then why you need to choose the BOM. The macro (the macros to do this are in bits and pieces and those need to be combined) can find the BOM on the active sheet and link views on that sheet to that BOM.
I don't have much experience with VBA, but I'll give it a try and publish it here for anybody else that needs something like this.
My drawings are for an assembly that have many subassemblies and weldments and I show a full page isometric view with the Bill of Materials for each subassembly and then spend the next one or two pages detailing out that subassembly.
My goal is to create a form so that my team members and I can place all the views on a sheet and then select which BOM to link all of the views on that sheet to.
This is a amalgamation of macros that others have written, but here is a macro that presents the user with a list of all BoM's (and Weldment lists) in the drawing and then assigns that BoM to all views on the active sheet.
I just tried this on SW2019sp3, with a weldment. I'm getting a runtime error. I have no clue how to edit the macro...
I didn't have this problem before installing SW19, but I can't find an Options settings
Try this one. It doesn't need to know the name of the BOM. It will automatically find it.