Good evening
I'm looking for a macro that would update the SOLIDWORKS properties of a configuration.
Currently I use these two lines of code to update the properties but the update is done on the document and not on a specified configuration.
bRet = swmodel. DeleteCustomInfo2("", "ma_propriété")
bRet = swmodel. AddCustomInfo3("", "ma_propriété", swCustomInfoText, "here the value of the property")
Do you have any information to give me on this subject?
In advance, thank you
Sylvain
At the risk of being a bit "heavy", why not use Smartproperties (Axemble utility for sale on Lynkoa) rather than running macros (personally I don't master, that's why !!!).
For people who don't master macro programming, this type of utility is still the best thing we do, right?
For your information, I don't get a cent on the sale of the Smartproperties van!!!!!!!!
http://www.lynkoa.com/store/fr/tools-et-macros/utilitaire-smartproperties.html
@flegendre
It is true that smartproperties fulfills this function, but it is complex because it does more
Hello
You have to use the CustomPropertyManager api where you specify the name of the configuration to be modified "" for custom properties.
Then on the object you have the Add, Get, Set, and Delete APIs to create, retrieve, modify, and delete them:
@Lucas Prieur : your link is the API to use if the document is closed
Example:
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As ModelDoc2
Dim swModelDocExt As ModelDocExtension
Dim swCustProp As CustomPropertyManager
Dim val As String
Dim valout As String
Dim bool As Boolean
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp. ActiveDoc
Set swModelDocExt = swModel. Extension
' Get the custom property data
Set swCustProp = swModelDocExt. CustomPropertyManager("Configuration Name")
bool = swCustProp. Get4("Property_Name", False, val, valout)
Debug.Print "Value: " & val
Debug.Print "Evaluated value: " & valout Debug.Print "Up-to-date data: " & bool
End Sub
Hello
Thanks for those answers, I'll look into it.
As for SMARTPROPERTIES, I use it. In fact, I have a button in the SMARTPROPERTIES that lanes a macro with a SQL query that points to the ERP.
From the values of a property, I retrieve some parameters from the ERP to put them back in the SOLIDWORKS properties.
I'll keep you posted
Thank you
sylvain
Hello
Here is an example that completes prossignol's answer
I use this macro to remove properties in all part and assembly configurations:
Option Explicit
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swModelDocExt As SldWorks.ModelDocExtension
Dim swConfig As SldWorks.Configuration
Dim swCustPropMgr As SldWorks.CustomPropertyManager
Sun i As Long
Dim vConfName as Variant
Dim valOut As String
Public Enum swDocumentTypes_e
swDocNONE = 0 ' Used to be TYPE_NONE
swDocPART = 1 ' Used to be TYPE_PART
swDocASSEMBLY = 2 ' Used to be TYPE_ASSEMBLY
swDocDRAWING = 3 ' Used to be TYPE_DRAWING
End Enum
Sub main()
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
'Removed properties in the Configuration Specific tab
If swModel.GetType <> swDocDRAWING Then
vConfName = swModel.GetConfigurationNames
For i = 0 TB UBound(vConfName)
Set swConfig = swModel.GetConfigurationByName(vConfName(i))
'Debug.Print' Configuration = ' & vConfName(i)
Set swCustPropMgr = swConfig.CustomPropertyManager
swCustPropMgr.Delete "Author"
swCustPropMgr.Delete "Project"
swCustPropMgr.Delete "Status"
swCustPropMgr.Delete "Number"
Next i
End If
End Sub
For minimal modification with your code
just specify the name of the config instead of the empty field
bRet = swmodel. DeleteCustomInfo2("Config Name", "ma_propriété")
bRet = swmodel. AddCustomInfo3("Config name", "ma_propriété", swCustomInfoText, "here is the value of the property")
But it is advisable to go through the response of prossignol
Have you managed to update your macro???
Hello everyone,
Thank you for your answers that just solved the problem.
Sylvain