Hi every body,
I'm trying to use VBA to write some part of an assembly in step, unsuccessfully!!
My part has many configuration, and I want to save each of them in step, with a special coordinate system I have create.. I have trye to record a macro and then edit it, as I simply do in other software, but here it seems to be al little more commplicated... Do you have any ideas?
Many thanks
Regards
Hello Maxime!
I hope you're doing well.
This code will traverse through all of your parts' configurations and saves them in step format in the folder of your original part!
It will prompt a message at the end whether you want to open the folder or not. You can change the variable CoordinateSystemStr's value with the name of your coordinate system from the feature tree manager.
Your feedback will be appreciated!
Bonjour Maxime!
J'espère que tout va bien!
Le code ci-dessus parcourt les configurations de votre modèle et puis sauvegarde chaque configuration, en format step, dans le dossier du fichier du modèle original! A la fin de l’exécution du code, un message vous proposera d'ouvrir le dossier après la conversion. Vous pouvez changer la valeur variable CoordinateSystemStr avec le nom du votre système de coordonnées dans votre arabe de création.
Regards/Best,
Code:
'' Code par JLILI Amen / Jliliamen@gmail.com CSWA/CSWP QA-Mechanical Engineer
'' https://tn.linkedin.com/in/djelly
Dim swApp As SldWorks.SldWorks
Sub main()
'' Nom de systeme de coordonnes
Dim CoordinateSystemStr As String: CoordinateSystemStr = "Coordinate System1"
'' Application SolidWorks
Set swApp = Application.SldWorks
'' Variable Modèle
Dim swModelDoc As SldWorks.ModelDoc2
'' Affectation de la modèle active
Set swModelDoc = swApp.ActiveDoc
'' Liste de noms des configurations
Dim VConfiguration As Variant
VConfiguration = swModelDoc.GetConfigurationNames
'' Test sur la liste de noms (si elle est vide)
If Not IsEmpty(VConfiguration) Then
'' Parcours de la liste de noms des configurations
For i = LBound(VConfiguration) To UBound(VConfiguration)
'Activer la configuration
Dim Bol As Boolean
Bol = swModelDoc.ShowConfiguration2(VConfiguration(i))
'Cochez l'option du systeme de coordonnes
Dim swModelExtension As SldWorks.ModelDocExtension
Set swModelExtension = swModelDoc.Extension
Bol = swModelExtension.SetUserPreferenceString(swUserPreferenceStringValue_e.swFileSaveAsCoordinateSystem, swUserPreferenceOption_e.swDetailingNoOptionSpecified, CoordinateSystemStr)
'Sauvegarder
Bol = swModelDoc.SaveAs(VConfiguration(i) + ".step")
Next i
Dim result As VbMsgBoxResult: result = MsgBox("Conversion terminée!", vbYesNo, "Conversion à step")
If result = vbYes Then
Shell "cmd /C start """" /max """ & swModelDoc.GetPathName & """", vbHide
End If
End If
End Sub
Dear Jlili,
Thanks a lot for your quick and efficient answer.
However I won't be able to explain what I wanted . I won't save the entire assembly in STEP, but only 1 piece wich have several configuration, build
with a table: this is a familly of piece: the hilighted blue one.
Is this as easy for you, or it's a new challenge
Many thanks in advance.
Regards
Maxime
Understood (Correct me if I'm wrong). You want to be able to save an assembly component while utilizing the assembly's system of coordinate as the component's default coordinate system. I'll take a look at it sometime tonight. My desk is clouded with paperwork right now.
As for the challenge, rien est impossible !
I want to save an assembly component while utilizing a system of coordinates I created (called "speos" in the preview image) in step format. In other word, to avoid all misunderstanding:
Without a macro, I will do this:
1) Put the higlighted in blue component in the right configuration.
2) Select with the mouse this component in this configuration
3) select the "save as" command
4) Select the "step" format, and then with "option" button select the coordinate system.
5) do it till I saved all my component configuration in step.
If Y could save them with the name of component configuration name, it would be "the cherry on the cake"!!
Thanks
Maxime
Hello Maxime!
I'm so sorry for my late response.
Please try this following code and give me your feedback.
There is only one pre-condition for this code to execute without error:
Your designated part must be the only selected object in your assembly. To perform a proper selection, click on the component from the feature tree manager.
Change the coordinateSystemStr's value accordingly.
Best,
PS: I don't like cherry but cake would be fine
'' Code par JLILI Amen / Jliliamen@gmail.com CSWA/CSWP QA-Mechanical Engineer
'' https://tn.linkedin.com/in/djelly
Dim swApp As SldWorks.SldWorks
Sub main()
On Error GoTo Handler:
'' Nom de systeme de coordonnes
'''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''
Dim CoordinateSystemStr As String: CoordinateSystemStr = "Coordinate System1"
''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''
'' Application SolidWorks
Set swApp = Application.SldWorks
'' Variable Modèle
Dim swModelDoc As SldWorks.ModelDoc2
'' Affectation de la modèle active
Set swModelDoc = swApp.ActiveDoc
'' Selection Manager
Dim swSelectionManager As SldWorks.SelectionMgr
Set swSelectionManager = swModelDoc.SelectionManager
'' Affection du fichier d'assemblage
Dim swAssemblyDoc As SldWorks.AssemblyDoc
Set swAssemblyDoc = swModelDoc
'' Dossier de sauvegarde
Dim Folder As String: Folder = swModelDoc.GetPathName
'' Selection de la pièce
Dim swComponent As Component2
Set swComponent = swSelectionManager.GetSelectedObject(1)
Set swModelDoc = swComponent.GetModelDoc2
'' Liste de noms des configurations
Dim VConfiguration As Variant
VConfiguration = swModelDoc.GetConfigurationNames
'' Test sur la liste de noms (si elle est vide)
If Not IsEmpty(VConfiguration) Then
'' Parcours de la liste de noms des configurations
For i = LBound(VConfiguration) To UBound(VConfiguration)
'Activer la configuration
Dim Bol As Boolean
Bol = swModelDoc.ShowConfiguration2(VConfiguration(i))
'Cochez l'option du systeme de coordonnes
Dim swModelExtension As SldWorks.ModelDocExtension
Set swModelExtension = swModelDoc.Extension
Bol = swModelExtension.SetUserPreferenceString(swUserPreferenceStringValue_e.swFileSaveAsCoordinateSystem, swUserPreferenceOption_e.swDetailingNoOptionSpecified, CoordinateSystemStr)
'Sauvegarder
Bol = swModelDoc.SaveAs(VConfiguration(i) + ".step")
Next i
Dim result As VbMsgBoxResult: result = MsgBox("Conversion terminée!", vbYesNo, "Conversion à step")
If result = vbYes Then
Shell "cmd /C start """" /max """ & Folder & """", vbHide
End If
End If
Exit Sub
Handler:
swApp.SendMsgToUser ("Une erreur s'est produite lors de l'éxecution du macro.")
End Sub
Ok thanks a lot,
This is almost perfect.
The bad thing is: my coordinate system is not taken into account.
When I run the debug mode and the spy window, I can see after this line:
"Bol = swModelExtension.SetUserPreferenceString(swUserPreferenceStringValue_e.swFileSaveAsCoordinateSystem, swUserPreferenceOption_e.swDetailingNoOptionSpecified, CoordinateSystemStr)" that the Bol variable is set to "False"..
I search in the API help but didn't find anything which can help me...
One more question: where do you think can I learn the most efficiency the Solidworks API? Are there books, good tutoriel?
Thank you
Maxime
NB: For the cake, my friends tell that I am "black belt" in tiramisu!!
Hello Maxime!
Please excuse me! (I still want the cake though)
I was in such a rush to answer your question this morning that I made the mistake of assigning the system coordinate system to the component rather than the assembly file. That explains why the boolean was returning false. Here's the corrected code:
'' Code par JLILI Amen / Jliliamen@gmail.com CSWA/CSWP QA-Mechanical Engineer
'' https://tn.linkedin.com/in/djelly
Dim swApp As SldWorks.SldWorks
Sub main()
On Error GoTo Handler:
'' Nom de systeme de coordonnes
'''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''
Dim CoordinateSystemStr As String: CoordinateSystemStr = "Coordinate System1"
''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''''
'' Application SolidWorks
Set swApp = Application.SldWorks
'' Variable Modèle
Dim swModelDoc As SldWorks.ModelDoc2
'' Affectation de la modèle active
Set swModelDoc = swApp.ActiveDoc
'' Selection Manager
Dim swSelectionManager As SldWorks.SelectionMgr
Set swSelectionManager = swModelDoc.SelectionManager
'' Affection du fichier d'assemblage
Dim swAssemblyDoc As SldWorks.AssemblyDoc
Set swAssemblyDoc = swModelDoc
'' Dossier de sauvegarde
Dim Folder As String: Folder = swModelDoc.GetPathName
'' Selection de la pièce
Dim swComponent As Component2
Set swComponent = swSelectionManager.GetSelectedObject(1)
Dim SwModelFromComp As ModelDoc2
Set SwModelFromComp = swComponent.GetModelDoc2
'' Liste de noms des configurations
Dim VConfiguration As Variant
VConfiguration = swModelDoc.GetConfigurationNames
'' Test sur la liste de noms (si elle est vide)
If Not IsEmpty(VConfiguration) Then
'' Parcours de la liste de noms des configurations
For i = LBound(VConfiguration) To UBound(VConfiguration)
'Activer la configuration
Dim Bol1 As Boolean
Bol1 = swModelDoc.ShowConfiguration2(VConfiguration(i))
'Cochez l'option du systeme de coordonnes
Dim swModelExtension As SldWorks.ModelDocExtension
Set swModelExtension = swModelDoc.Extension
Dim Bol2 As Boolean
Bol2 = swModelExtension.SetUserPreferenceString(swUserPreferenceStringValue_e.swFileSaveAsCoordinateSystem, swUserPreferenceOption_e.swDetailingNoOptionSpecified, CoordinateSystemStr)
'Sauvegarder
Dim Bol3 As Boolean
Bol3 = SwModelFromComp.SaveAs(VConfiguration(i) + ".step")
Next i
Dim result As VbMsgBoxResult: result = MsgBox("Conversion terminée!", vbYesNo, "Conversion à step")
If result = vbYes Then
Shell "cmd /C start """" /max """ & Folder & """", vbHide
End If
End If
Exit Sub
Handler:
swApp.SendMsgToUser ("Une erreur s'est produite lors de l'éxecution du macro.")
End Sub
The boolean is now returning true.
Want to learn the API?
There's a great book titled automating Solidworks using macros. That's the only book I know (and read). It's a good introduction to the world of CAD automation (VBA and VSTA macros). You can find tons of good answers here too. If you want to go to the extreme professional side of SW then you should learn about add-ins which are complements that extend SW functionanlities. The possibilities are limitless. (Notable mention goes to CAMWorks, DriveWorks...). They require a strong background on the API, .NET and COM objects. The best way to learn is to ask questions so do not be afraid to ask. I, hereby, extend you the invitation to ask me questions on my personal email (jliliamen@gmail.com), no problem.
Best,
Amen
I really Thank you for your time and advise.
This code still doesn't have the good behavior, although the 3 boolean variables take the "true" value!
I perhaps saw some mistake, correct me if I'm wrong:
line 31. VConfiguration = swModelDoc.GetConfigurationNames <=> VConfiguration = SwModelFromComp.GetConfigurationNames ?
line 38. Bol1 = swModelDoc.ShowConfiguration2(VConfiguration(i)) <=> Bol1 = SwModelFromComp.ShowConfiguration2(VConfiguration(i)) ?
line 41. Set swModelExtension = swModelDoc.Extension => no idea!!
Moreover, I don't understand when you use the "Folder" string to set the folder where to save the part.
Thank you
Maxime
Hello,
Need not to worry about the folder variable. The last command merely opens the folder of the your assembly file because that's where your step files are saved. The SwModelDoc is your assembly file. We need that in order to change the coordinate in the export window since we're doing the saving from the assembly file as our active doc (This might be where the problem resides and there's a painful solution). The swModelFromComp is the selected part from the feature tree manager. It's an assembly component2 object from which an modeldoc is taken and saved as using the saveas method as a step file.
I might be missing something?
What I want to know is does the step files have the assembly's coordinate system when you open them?
There's the solution of hiding the rest of the parts and exporting as step. I'll code something tomorrow if I can.
Export only “Selected Parts” from SolidWorks Assembly | Boxer's CAD CAM Blog
Best,
Hello,
My step file must have the coordinate system I have created in my assembly, and not the original assembly coordinate system!
Thank you again for your time!
Maxime
Yes. Your coordinate system not the assembly's. I'll code something out this weekend.
Hi Maxime!
Here attached is an example using the Export only “Selected Parts” from SolidWorks Assembly | Boxer's CAD CAM Blog method. It works fine except that when saving the different configurations, you get prompted a warning to suppress/unsuppress hidden components (click no to that). I couldn't find anything in the API that hides that message. The saved steps have the customized system of coordinates. Perhaps, you should try this and give me your feedback.
Best,
Dear Amen Allah Jlili,
I've tried this, it work fine for my needs, actually this is what I do every day in step format, with the coordinate system I choose.
What I want is to write something wich could do this without my intervention: I spend a lot of time to chose the component, go to "save as", throught the windows explorer, et choose my coordinate system!!
Have a great day!
Maxime
Dear Amen Allah Jlili,
My appologyze for my late answer, but these last Macro does excactly what I want!
Thank you very much.
Maxime
Hi Maxime!
Here attached is an example using the Export only “Selected Parts” from SolidWorks Assembly | Boxer's CAD CAM Blog method. It works fine except that when saving the different configurations, you get prompted a warning to suppress/unsuppress hidden components (click no to that). I couldn't find anything in the API that hides that message. The saved steps have the customized system of coordinates. Perhaps, you should try this and give me your feedback.
Best,