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Custom Properties - Extracting Part Number and Description from Title Text

Question asked by Jan Hendrik Hollenbach on Nov 30, 2020
Latest reply on Dec 1, 2020 by Peter Kennedy

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Comment • 6

Background:

I am a Solidworks 2019 user, and our company does not have a PDM system. I would like to streamline the saving convention and make the BOM data extraction process quicker. I am not very familiar with APIs.

Requirement: An equation that can be run to detect and assign a combination of text within a part's title, to automatically compile MATERIAL and DESCRIPTION properties.

Example:

After modelling, I would like to save a part as "M30405 Gusset". I would manually type all text, and save the file in the applicable folder.
I would then like to run an equation that detects the first 6 characters in the title, and assign them to the 'PART NUMBER' property of the current file.
If possible, the same equation should be able to detect all characters after the space, and assign them to the 'DESCRIPTION' property of the file.

What I have done so far:

"dummy"= part.Extension.CustomPropertyManager("").Set("partno", Left(part.GetTitle,6))

"dummy2"= part.Extension.CustomPropertyManager("").Set("description", Mid(part.GetTitle,8,50))

However, when pasting these lines into the File Properties -> Summary Information table, I am not getting any solution.

There are a few resources I investigated, but I can't make it function properly using SolidWorks 2019/2020:

How do I use a PART name and pieces of it to populate Drawings and BOM's?

https://forum.solidworks.com/message/174200#174200#174200

Any help would be appreciated!!

Jan-Hendrik

Peter Kennedy Dec 1, 2020 11:02 AM

Correct Answer

This is hard set to a 6 digit part number, if your part number length varies you'll have to adjust the code. I did test it for file name 123456 Test1.SLDPRT

Dim swApp As SldWorks.SldWorks
Dim swModel As ModelDoc2
Dim swPart As PartDoc

Dim swCustProp As CustomPropertyManager
Dim PartNumber As Variant

Dim Description As Variant
Dim CurrentFileName As Variant

Option Explicit

Sub main()

Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swPart = swModel

Set swCustProp = swModel.Extension.CustomPropertyManager("")

CurrentFileName = Mid(swModel.GetPathName, InStrRev(swModel.GetPathName, "\") + 1)

PartNumber = Left(CurrentFileName, 6)

Description = Left(CurrentFileName, InStrRev(CurrentFileName, ".SLD") - 1)
Description = Right(Description, Len(Description) - 7)

Debug.Print PartNumber
Debug.Print Description

swModel.AddCustomInfo3 "", "partno", swCustomInfoText, PartNumber

swModel.AddCustomInfo3 "", "description", swCustomInfoText, Description

Debug.Print CurrentFileName

End Sub

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Krzysztof Wojcik Nov 30, 2020 6:24 AM

Hi.

What if you could reverse the steps? Fill in properties and generate file name from those.

I'm using a short macro that gathers some of the properties and combine it to a file name that is pasted to the clipboard.

You need to run it prior to saving a file and just paste in the generated name from the clipboard.

Sub main()
Dim swApp As SldWorks.SldWorks
Dim SWmoddoc As SldWorks.ModelDoc2
Dim proj As String
Dim drg As String
Dim rev As String
Dim Filetxt As String

Set swApp = Application.SldWorks
Set SWmoddoc = swApp.ActiveDoc
proj = SWmoddoc.CustomInfo("Project")
drg = SWmoddoc.CustomInfo("drgnumber")
rev = SWmoddoc.CustomInfo("Revision")
Filetxt = proj + "-" + drg + "_rev_" + rev

Dim Clip As MSForms.DataObject

Set Clip = New MSForms.DataObject

'Set Clip = CreateObject("new:{1C3B4210-F441-11CE-B9EA-00AA006B1A69}")

'Clip.GetFromClipboard
MsgBox Filetxt, vbOKOnly, "DRG Number"

Clip.SetText Filetxt
Clip.PutInClipboard

Set Clip = Nothing

End Sub

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Jan Hendrik Hollenbach @ Krzysztof Wojcik on Dec 1, 2020 6:23 AM

Thank you Krzysztof

I will test the macro and see whether it works for our design methodology.

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Peter Kennedy Nov 30, 2020 10:32 AM

Like Krysztof Wojcik mentioned you'd probably be a lot better off added the properties and making the filename from that. I think this should be the code, I never tested it though.

Dim swApp As SldWorks.SldWorks

Dim swModel As ModelDoc2
Dim swModelDocExt As ModelDocExtension
Dim swCustProp As CustomPropertyManager

Dim bool As Bool

Dim val as string

Dim partno as string

Dim description as string

Dim folder as string

Option Explicit

Sub main()

Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swModelDocExt = swModel.Extension
Set swCustProp = swModelDocExt.CustomPropertyManager("")

Folder = "Folder Location to save the file"

bool = swCustProp.Get4("partno", False, val, partno)

bool = swCustProp.Get4("description", False, val, description)

If (swModel.GetType = swDocPART) Then
swModel.SaveAs (folder + partno + " " + "description" + ".sldprt")
ElseIf (swModel.GetType = swDocASSEMBLY) Then
swModel.SaveAs (folder + partno + " " + "description" + ".sldasm")
End If

End Sub

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Jan Hendrik Hollenbach @ Peter Kennedy on Dec 1, 2020 6:27 AM

Thank you Peter

I will test the code and adapt it to our folders.

Even though my saving convention may not be ideal, could you perhaps still advise on a solution to my question?

Regards

Actions

Peter Kennedy @ Jan Hendrik Hollenbach on Dec 1, 2020 11:02 AM

This is hard set to a 6 digit part number, if your part number length varies you'll have to adjust the code. I did test it for file name 123456 Test1.SLDPRT

Dim swApp As SldWorks.SldWorks
Dim swModel As ModelDoc2
Dim swPart As PartDoc

Dim swCustProp As CustomPropertyManager
Dim PartNumber As Variant

Dim Description As Variant
Dim CurrentFileName As Variant

Option Explicit

Sub main()

Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swPart = swModel

Set swCustProp = swModel.Extension.CustomPropertyManager("")

CurrentFileName = Mid(swModel.GetPathName, InStrRev(swModel.GetPathName, "\") + 1)

PartNumber = Left(CurrentFileName, 6)

Description = Left(CurrentFileName, InStrRev(CurrentFileName, ".SLD") - 1)
Description = Right(Description, Len(Description) - 7)

Debug.Print PartNumber
Debug.Print Description

swModel.AddCustomInfo3 "", "partno", swCustomInfoText, PartNumber

swModel.AddCustomInfo3 "", "description", swCustomInfoText, Description

Debug.Print CurrentFileName

End Sub

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John Stoltzfus Dec 1, 2020 6:59 AM

Jan Hendrik Hollenbach - I would create a Custom Property called PartNumber and then combine the File Name and Description, then in the Drawing Title Block insert that Custom Property. Then Save the Part File Template. No need for a macro when you do new components... Old Files you would just need to add the Custom Properties to the part or assembly, which would be easy to do using the Custom Property Tab Builder..

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6 Replies

Krzysztof Wojcik Nov 30, 2020 6:24 AM
Mark Correct
Correct Answer
Hi.
What if you could reverse the steps? Fill in properties and generate file name from those.
I'm using a short macro that gathers some of the properties and combine it to a file name that is pasted to the clipboard.
You need to run it prior to saving a file and just paste in the generated name from the clipboard.

Sub main()
Dim swApp As SldWorks.SldWorks
Dim SWmoddoc As SldWorks.ModelDoc2
Dim proj As String
Dim drg As String
Dim rev As String
Dim Filetxt As String

Set swApp = Application.SldWorks
Set SWmoddoc = swApp.ActiveDoc
proj = SWmoddoc.CustomInfo("Project")
drg = SWmoddoc.CustomInfo("drgnumber")
rev = SWmoddoc.CustomInfo("Revision")
Filetxt = proj + "-" + drg + "_rev_" + rev
Dim Clip As MSForms.DataObject

Set Clip = New MSForms.DataObject

'Set Clip = CreateObject("new:{1C3B4210-F441-11CE-B9EA-00AA006B1A69}")

'Clip.GetFromClipboard
MsgBox Filetxt, vbOKOnly, "DRG Number"

Clip.SetText Filetxt
Clip.PutInClipboard

Set Clip = Nothing
End Sub
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- Jan Hendrik Hollenbach @ Krzysztof Wojcik on Dec 1, 2020 6:23 AM
  Mark Correct
  Correct Answer
  Thank you Krzysztof
  
  I will test the macro and see whether it works for our design methodology.
  Like • Show 1 Like1
  Actions
Peter Kennedy Nov 30, 2020 10:32 AM
Mark Correct
Correct Answer
Like Krysztof Wojcik mentioned you'd probably be a lot better off added the properties and making the filename from that. I think this should be the code, I never tested it though.

Dim swApp As SldWorks.SldWorks
Dim swModel As ModelDoc2
Dim swModelDocExt As ModelDocExtension
Dim swCustProp As CustomPropertyManager
Dim bool As Bool
Dim val as string
Dim partno as string
Dim description as string
Dim folder as string

Option Explicit
Sub main()

Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swModelDocExt = swModel.Extension
Set swCustProp = swModelDocExt.CustomPropertyManager("")

Folder = "Folder Location to save the file"

bool = swCustProp.Get4("partno", False, val, partno)
bool = swCustProp.Get4("description", False, val, description)

If (swModel.GetType = swDocPART) Then
swModel.SaveAs (folder + partno + " " + "description" + ".sldprt")
ElseIf (swModel.GetType = swDocASSEMBLY) Then
swModel.SaveAs (folder + partno + " " + "description" + ".sldasm")
End If
End Sub
Like • Show 2 Likes2
Actions
- Jan Hendrik Hollenbach @ Peter Kennedy on Dec 1, 2020 6:27 AM
  Mark Correct
  Correct Answer
  Thank you Peter
  
  I will test the code and adapt it to our folders.
  
  Even though my saving convention may not be ideal, could you perhaps still advise on a solution to my question?
  
  Regards
  Like • Show 1 Like1
  Actions
  - Peter Kennedy @ Jan Hendrik Hollenbach on Dec 1, 2020 11:02 AM
    Unmark Correct
    Correct Answer
    This is hard set to a 6 digit part number, if your part number length varies you'll have to adjust the code. I did test it for file name 123456 Test1.SLDPRT
    
    Dim swApp As SldWorks.SldWorks
    Dim swModel As ModelDoc2
    Dim swPart As PartDoc
    Dim swCustProp As CustomPropertyManager
    Dim PartNumber As Variant
    Dim Description As Variant
    Dim CurrentFileName As Variant
    Option Explicit
    Sub main()
    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swPart = swModel
    Set swCustProp = swModel.Extension.CustomPropertyManager("")
    CurrentFileName = Mid(swModel.GetPathName, InStrRev(swModel.GetPathName, "\") + 1)
    PartNumber = Left(CurrentFileName, 6)
    Description = Left(CurrentFileName, InStrRev(CurrentFileName, ".SLD") - 1)
    Description = Right(Description, Len(Description) - 7)
    Debug.Print PartNumber
    Debug.Print Description
    swModel.AddCustomInfo3 "", "partno", swCustomInfoText, PartNumber
    swModel.AddCustomInfo3 "", "description", swCustomInfoText, Description
    Debug.Print CurrentFileName
    End Sub
    Like • Show 1 Like1
    Actions
John Stoltzfus Dec 1, 2020 6:59 AM
Mark Correct
Correct Answer
Jan Hendrik Hollenbach - I would create a Custom Property called PartNumber and then combine the File Name and Description, then in the Drawing Title Block insert that Custom Property. Then Save the Part File Template. No need for a macro when you do new components... Old Files you would just need to add the Custom Properties to the part or assembly, which would be easy to do using the Custom Property Tab Builder..
Like • Show 0 Likes0
Actions

Custom Properties - Extracting Part Number and Description from Title Text

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