AnsweredAssumed Answered

Is it possible to add global variables to several files (+50) at the same time, for example, with the task scheduler?

Question asked by Daniel Restrepo on Oct 31, 2014
Latest reply on Nov 4, 2014 by Daniel Restrepo

Like • Show 1 Like1
Comment • 12

Hello everybody,

I got a design with some parts and assemblies and I realized I could use a couple of global variables to calculate something that will later be used in a custom property, but I don't know how to add variables in batches. For now I solved the problem for the new files by creating a template which already includes the variables and properties, but the other parts that were already there and did not have any variables... I'm looking for a way to do it all at once, maybe with the task scheduler or a macro?

Thanks for your help!

Daniel Restrepo

Daniel Andersson Oct 31, 2014 1:31 AM

Correct Answer

Yes it is possible. You can also add the custom properties in batch runs. But... if the files are in a PDM system, then it might be more difficult depending on which system you are running.

Here is a link to a blog at cadsharp.com. It instruct how to run macros with Task schedule.

http://www.cadsharp.com/blog/run-solidworks-macros-using-task-scheduler/

and here is a link to the equation manager API interface (click members to see properties and methods)

http://help.solidworks.com/2014/English/api/sldworksapi/SolidWorks.Interop.sldworks~SolidWorks.Interop.sldworks.IEquationMgr.html

And here is a link to the Add3 method in equation manager API, which is used to add global variables and equations.

http://help.solidworks.com/2014/English/api/sldworksapi/SolidWorks.Interop.sldworks~SolidWorks.Interop.sldworks.IEquationMgr~Add3.html

Just let us know if you need further help.

See the reply in context

No one else had this question

Outcomes

Daniel Andersson Oct 31, 2014 1:31 AM

Yes it is possible. You can also add the custom properties in batch runs. But... if the files are in a PDM system, then it might be more difficult depending on which system you are running.

Here is a link to a blog at cadsharp.com. It instruct how to run macros with Task schedule.

http://www.cadsharp.com/blog/run-solidworks-macros-using-task-scheduler/

and here is a link to the equation manager API interface (click members to see properties and methods)

http://help.solidworks.com/2014/English/api/sldworksapi/SolidWorks.Interop.sldworks~SolidWorks.Interop.sldworks.IEquationMgr.html

And here is a link to the Add3 method in equation manager API, which is used to add global variables and equations.

http://help.solidworks.com/2014/English/api/sldworksapi/SolidWorks.Interop.sldworks~SolidWorks.Interop.sldworks.IEquationMgr~Add3.html

Just let us know if you need further help.

Actions

Daniel Restrepo @ Daniel Andersson on Oct 31, 2014 11:52 AM

Hello Daniel,

Thanks for your help! I took a look at the links you sent me and that is exactly what I need, but now I just have a doubt, I think I can't write the macro myself because I don't have the API add-in available...

Daniel

Actions

Deepak Gupta @ Daniel Restrepo on Oct 31, 2014 11:59 AM

There is no add-in required for the API. Start a new macro under Tools > Macro > New

Best of luck

Actions

Daniel Restrepo @ Deepak Gupta on Oct 31, 2014 1:13 PM

Hello Deepak,

Thanks for answering so quickly, I just made a macro using one of your previous answers to another post like this:

____________________________________________

Dim swApp As Object

Dim Part As Object

Dim boolstatus As Boolean

Dim swEquationMgr As Object

Dim longstatus As Long, longwarnings As Long

Sub main()

Set swApp = Application.SldWorks

Set Part = swApp.ActiveDoc

'Adds the below mentioned Equations

Set swEquationMgr = Part.GetEquationMgr()

swEquationMgr.Add -1, """weight in kg""=""SW-Mass""/1000"

'Rebuild and Save the file.

boolstatus = Part.ForceRebuild()

Part.Save

End Sub

____________________________________________

It did work and it added the global variable, but it didn't recognize the hyphen correctly so it breaks up the standard solidworks mass property... Do you know what to do here?

See the picture below

Actions

Deepak Gupta @ Daniel Restrepo on Oct 31, 2014 1:37 PM

Works fine for me on SW2014. What is your SW version and SP?

Actions

Daniel Restrepo @ Deepak Gupta on Oct 31, 2014 1:44 PM

I'm using SW 2014 SP4.0

Could it be happening because my windows language is different to english?

Actions

Daniel Andersson @ Daniel Restrepo on Oct 31, 2014 2:52 PM

Works fine on SW2012 SP5 as well.

What language do you use? I doubt that it would influence since the syntax is what it is and using double quote marks "" will result in a single qoute mark " in the string. But it might be intresting to know what language you have installed.

Noted that the Add method is obsolete, but I doubt it will make difference... but you should use Add2.

What is the warning saying about the equation?

Actions

Daniel Restrepo @ Daniel Andersson on Nov 4, 2014 10:43 AM

Hello Daniel,

I just found out that the language was causing the problem. My windows is in spanish and therefore the mass property is "SW-Masa" with an "a" instead of the second s...

So now it's working fine and I will use your recommendation of changing also the weight units in the part template to kg.

Thanks for your help! And Deepak if you read this too, thanks!

Daniel

Actions

Deepak Gupta @ Daniel Restrepo on Nov 1, 2014 3:36 AM

Can you record a macro while adding the the equation manually and see what are the codes in the recorded one??

Actions

Daniel Andersson @ Daniel Restrepo on Oct 31, 2014 2:32 PM

Except from adding the equation and property I would recommend that you also set the document setting of mass to kg as you add the equation and property.

It is better to be safe then sorry, if some user have made a change or if there is an old file with different settings around....

SetUserPreferenceInteger Method (IModelDocExtension)

See swUnitsMassPropMass_e for enumeration to use.

Actions

Deepak Gupta Oct 31, 2014 2:35 AM

Dan if you can share more information on what are you trying to add/update them someone may write a macro for you.

Actions

Daniel Restrepo @ Deepak Gupta on Oct 31, 2014 11:40 AM

Hello Deepak,

For the moment I'm just trying to add a global variable to calculate the mass of my part/assembly in kg (not in g) and with just one decimal, like this:

"weight in kg" = ROUND ( "SW-Mass" / 1000 , 1 )

then I add a custom property that calls this value and later it the value is used in some of my drawings.

so, that's what I need for now... I'm also going to take a look at the links Daniel Andersson sent me.

Thanks for your help!

Daniel

Actions

12 Replies

Daniel Andersson Oct 31, 2014 1:31 AM
Unmark Correct
Correct Answer
Yes it is possible. You can also add the custom properties in batch runs. But... if the files are in a PDM system, then it might be more difficult depending on which system you are running.

Here is a link to a blog at cadsharp.com. It instruct how to run macros with Task schedule.

http://www.cadsharp.com/blog/run-solidworks-macros-using-task-scheduler/

and here is a link to the equation manager API interface (click members to see properties and methods)

http://help.solidworks.com/2014/English/api/sldworksapi/SolidWorks.Interop.sldworks~SolidWorks.Interop.sldworks.IEquationMgr.html

And here is a link to the Add3 method in equation manager API, which is used to add global variables and equations.

http://help.solidworks.com/2014/English/api/sldworksapi/SolidWorks.Interop.sldworks~SolidWorks.Interop.sldworks.IEquationMgr~Add3.html

Just let us know if you need further help.
Like • Show 1 Like1
Actions
- Daniel Restrepo @ Daniel Andersson on Oct 31, 2014 11:52 AM
  Mark Correct
  Correct Answer
  Hello Daniel,
  Thanks for your help! I took a look at the links you sent me and that is exactly what I need, but now I just have a doubt, I think I can't write the macro myself because I don't have the API add-in available...
  
  Daniel
  Like • Show 0 Likes0
  Actions
  - Deepak Gupta @ Daniel Restrepo on Oct 31, 2014 11:59 AM
    Mark Correct
    Correct Answer
    There is no add-in required for the API. Start a new macro under Tools > Macro > New
    
    Best of luck
    Like • Show 0 Likes0
    Actions
    - Daniel Restrepo @ Deepak Gupta on Oct 31, 2014 1:13 PM
      Mark Correct
      Correct Answer
      Hello Deepak,
      
      Thanks for answering so quickly, I just made a macro using one of your previous answers to another post like this:
      ____________________________________________
      Dim swApp As Object
      Dim Part As Object
      Dim boolstatus As Boolean
      Dim swEquationMgr As Object
      Dim longstatus As Long, longwarnings As Long
      Sub main()
      
      Set swApp = Application.SldWorks
      Set Part = swApp.ActiveDoc
      'Adds the below mentioned Equations
      Set swEquationMgr = Part.GetEquationMgr()
      swEquationMgr.Add -1, """weight in kg""=""SW-Mass""/1000"
      
      'Rebuild and Save the file.
      boolstatus = Part.ForceRebuild()
      Part.Save
      
      End Sub
      ____________________________________________
      
      It did work and it added the global variable, but it didn't recognize the hyphen correctly so it breaks up the standard solidworks mass property... Do you know what to do here?
      See the picture below
      
      Like • Show 0 Likes0
      Actions
      - Deepak Gupta @ Daniel Restrepo on Oct 31, 2014 1:37 PM
        Mark Correct
        Correct Answer
        Works fine for me on SW2014. What is your SW version and SP?
        Like • Show 0 Likes0
        Actions
        Daniel Restrepo @ Deepak Gupta on Oct 31, 2014 1:44 PM
        Mark Correct
        Correct Answer
        I'm using SW 2014 SP4.0
        Could it be happening because my windows language is different to english?
        Like • Show 0 Likes0
        Actions
        Daniel Andersson @ Daniel Restrepo on Oct 31, 2014 2:52 PM
        Mark Correct
        Correct Answer
        Works fine on SW2012 SP5 as well.
        
        What language do you use? I doubt that it would influence since the syntax is what it is and using double quote marks "" will result in a single qoute mark " in the string. But it might be intresting to know what language you have installed.
        
        Noted that the Add method is obsolete, but I doubt it will make difference... but you should use Add2.
        
        What is the warning saying about the equation?
        Like • Show 0 Likes0
        Actions
        Daniel Restrepo @ Daniel Andersson on Nov 4, 2014 10:43 AM
        Mark Correct
        Correct Answer
        Hello Daniel,
        I just found out that the language was causing the problem. My windows is in spanish and therefore the mass property is "SW-Masa" with an "a" instead of the second s...
        So now it's working fine and I will use your recommendation of changing also the weight units in the part template to kg.
        
        Thanks for your help! And Deepak if you read this too, thanks!
        Daniel
        Like • Show 2 Likes2
        Actions
        Deepak Gupta @ Daniel Restrepo on Nov 1, 2014 3:36 AM
        Mark Correct
        Correct Answer
        Can you record a macro while adding the the equation manually and see what are the codes in the recorded one??
        Like • Show 0 Likes0
        Actions
      - Daniel Andersson @ Daniel Restrepo on Oct 31, 2014 2:32 PM
        Mark Correct
        Correct Answer
        Except from adding the equation and property I would recommend that you also set the document setting of mass to kg as you add the equation and property.
        It is better to be safe then sorry, if some user have made a change or if there is an old file with different settings around....
        
        SetUserPreferenceInteger Method (IModelDocExtension)
        See swUnitsMassPropMass_e for enumeration to use.
        
        Like • Show 0 Likes0
        Actions
Deepak Gupta Oct 31, 2014 2:35 AM
Mark Correct
Correct Answer
Dan if you can share more information on what are you trying to add/update them someone may write a macro for you.
Like • Show 0 Likes0
Actions
- Daniel Restrepo @ Deepak Gupta on Oct 31, 2014 11:40 AM
  Mark Correct
  Correct Answer
  Hello Deepak,
  
  For the moment I'm just trying to add a global variable to calculate the mass of my part/assembly in kg (not in g) and with just one decimal, like this:
  "weight in kg" = ROUND ( "SW-Mass" / 1000 , 1 )
  then I add a custom property that calls this value and later it the value is used in some of my drawings.
  
  so, that's what I need for now... I'm also going to take a look at the links Daniel Andersson sent me.
  Thanks for your help!
  
  Daniel
  Like • Show 0 Likes0
  Actions

Is it possible to add global variables to several files (+50) at the same time, for example, with the task scheduler?

Outcomes

Related Content

Recommended Content