Saturday, February 21, 2015

Solidworks Macros via Python

I finally figured out how to write Solidworks macros in python (yay!). Almost all the of Solidworks API works with one exception described at the end of this post. The Solidworks API is via the windows COM interface (ugh).

Here's the initial setup:

  1. Download and install Python. I used Active Python 2.7.8
  2. Get Solidworks. Python macros have worked pretty seamlessly across 2012, 2014 and 2015.
  3. Get familiar with the Solidworks online API help. E.g., is for the 2014 API. Note you can change the year in the URL to access the docs for other versions of Solidworks.
Ok, with that, we can dig right in. Before I run a macro, I make sure Solidworks is running and the document I want to modify is active (e.g., visible on the screen). I think you can use macros to start solidworks and open documents, but I'm less familiar with those commands.

Basic startup

This code snippet connects to running instance of Solidworks of the year specified. For example to connect to Solidworks 2015, set swYearLastDigit = 5:
import win32com.client
import pythoncom
swYearLastDigit = 5
sw = win32com.client.Dispatch("SldWorks.Application.%d" % (20+(swYearLastDigit-2)))  # e.g. 20 is SW2012,  23 is SW2015
You can also invoke Dispatch without the year specification, as in ....Dispatch("SldWorks.Application"). If there's only one version on your machine, this connects to that version.

At this point, the python code looks similar to the VBA code in the API docs. Sometimes you have to play with whether a function wants args or not. Here's the next piece of the boilerplate I have at the beginning of my scripts:

model = sw.ActiveDoc
modelExt = model.Extension
selMgr = model.SelectionManager
featureMgr = model.FeatureManager
sketchMgr = model.SketchManager
eqMgr = model.GetEquationMgr
As an example of difference in arguments, consider the Equation method on the IEquationMGR object (eqMgr in my code above). The 2014 API docs for the Equation member says that you read an equation by reading Equation(idx), and set by putting an equal sign after the expression. In python the binding is a bit different:
print("Equation 1 is: " + eqMgr.Equation(1))
eqMgr.Equation(1, "\"myVar\" = 42")
print("Equation 1 is now: " + eqMgr.Equation(1))
The most common difference I see between the Visual Basic docs and python are whether to put parenthesis after the member name or not. I just try both and see which works.

By the way, I see little rhyme or reason to the return values of method invocations, both at the API level as well as the values returned in practice. I usually go with the API docs, and assert return values, then delete the assertion if/when the method doesn't follow the API docs.

Creating arguments of the correct type (aka, getting SelectById2 to work)

Sometimes the method requires some fancy arguments, like reference arguments, or you otherwise just can't figure out what the thing is expecting. The Visual Basic interface is better at automatically converting types into the appropriate COM objects. The python bindings for the API don't work quite as well all the time. So here's what to do when you need to dig deeper and understand how to invoke a method:
  1. Generate the static python COM bindings for solidworks
    1. First, run python c:\Python27\Lib\site-packages\win32com\client\
    2. Select "SldWorks 2015 Type Library" and hit OK. You'll see output like this:
      Generating to C:\Users\myhappyuser\AppData\Local\Temp\gen_py\2.7\
      Building definitions from type library...
      Importing module
      The exact file name may change depending on your version of Solidworks.
  2. Open up that generated file in a viewer, like Komodo or Notepad
  3. Open up the web page VARIANT Type Constants in a browser
The generated python file has info on what arguments each method is expecting and that web page helps decode the arguments into something a bit more actionable.

Let's work a few common examples.

First let's try the macro command to select an object by name. The recommended version of the method is modelExt.SelectByID2. If you try putting in some actual args, you'll see:

ActivePython (ActiveState Software Inc.) based on
Python 2.7.8 (default, Jul  2 2014, 19:48:49) [MSC v.1500 64 bit (AMD64)] on win32
Type "help", "copyright", "credits" or "license" for more information.
>>> import win32com.client
>>> sw = win32com.client.Dispatch("SldWorks.Application")
>>> model = sw.ActiveDoc
>>> modelExt = model.Extension
>>> modelExt.SelectByID2("mysketch", "SKETCH", 0, 0, 0, False, 0, None, 0)
Traceback (most recent call last):
  File "", line 1, in 
  File ">", line 2, in SelectByID2
pywintypes.com_error: (-2147352571, 'Type mismatch.', None, 8)
The last number in the Type mismatch. line indicates the argument that is causing the problem. In this case it is the None, which is the eighth argument. The API man page says it is expecting a "pointer to a callout". We just want to pass None, but the None isn't getting converted to the right COM object, so we have to do the conversion manually.

To do this, open the generated python file, for Solidworks 2015 it should be named, and search for 'SelectById2'. You should find a hit that looks like:

	def SelectByID2(self, Name=defaultNamedNotOptArg, Type=defaultNamedNotOptArg, X=defaultNamedNotOptArg, Y=defaultNamedNotOptArg
			, Z=defaultNamedNotOptArg, Append=defaultNamedNotOptArg, Mark=defaultNamedNotOptArg, Callout=defaultNamedNotOptArg, SelectOption=defaultNamedNotOptArg):
		'Select a specified entity'
		return self._oleobj_.InvokeTypes(68, LCID, 1, (11, 0), ((8, 1), (8, 1), (5, 1), (5, 1), (5, 1), (11, 1), (3, 1), (9, 1), (3, 1)),Name
			, Type, X, Y, Z, Append
			, Mark, Callout, SelectOption)
The list of tuples ( ((8,1), (8, 1), (5, 1), ...) above ) contains info on the expected type of each argument. The eighth tuple corresponds to the problematic eighth argument. That tuple is (9, 1). Now look up '9' in that MSDN web page titled "VARIANT Type Constants" and you'll see it matches with VT_DISPATCH. Here's the magic on how to generate the correct object manually:
    arg1 = win32com.client.VARIANT(pythoncom.VT_DISPATCH, None)
The first arg to VARIANT is the type of the object to create, and the second arg is the initial contents. So now we can use that and:
>>> arg1 = win32com.client.VARIANT(pythoncom.VT_DISPATCH, None)
>>> modelExt.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, arg1, 0)

Now let's try a different example. Continuing on, let's get a sketch we selected:

>>> selMgr = model.SelectionManager
>>> aSketch = selMgr.GetSelectedObject(1).GetSpecificFeature2
>>> aSketch.Name
and let's get the plane it came from:
>>> aSketch.GetReferenceEntity(0)
Traceback (most recent call last):
  File "", line 1, in 
  File ">", line 2, in GetReferenceEntity
pywintypes.com_error: (-2147352571, 'Type mismatch.', None, 1)
Oops, that didn't work. Well looking into the generate python file and searching for GetReferenceEntity, we find:
	def GetReferenceEntity(self, LEntityType=defaultNamedNotOptArg):
		'Get entity that this sketch is created on'
		return self._ApplyTypes_(52, 1, (9, 0), ((16387, 3),), u'GetReferenceEntity', None,LEntityType
And then looking at the VARIANT web page, we find that 16387 = pythoncom.VT_BYREF | pythoncom.VT_I4 So GetReferenceEntity uses an output argument to return the entity type. We can construct an output argument similar to what we did for SelectByID2:
    arg1 = win32com.client.VARIANT(pythoncom.VT_BYREF | pythoncom.VT_I4, -1)
    refPlane = aSketch.GetReferenceEntity(arg1)
and now we can see:
>>> arg1 = win32com.client.VARIANT(pythoncom.VT_BYREF | pythoncom.VT_I4, -1)
>>> arg1.value
>>> refPlane = aSketch.GetReferenceEntity(arg1)
>>> arg1.value
To decode the '4', look at the doc for GetReferenceEntity, which points to the doc for an enumeration type swSelectType_e , which says that 4 maps to swSelDATUMPLANES


If you don't want to put '4' and other random constants in your python code, there are two possibilities. The first is to generate the python Solidworks COM constants bindings:
  1. Run python c:\Python27\Lib\site-packages\win32com\client\
  2. Select "SOLIDWORKS 2015 Constant type library"
  3. Add an EnsureModule command early in your python program using the number shown in the output of the makepy command. For example, with Solidworks 2015, that is:
    swconst = win32com.client.gencache.EnsureModule('{4687F359-55D0-4CD3-B6CF-2EB42C11F989}', 0, 23, 0).constants # sw2015
Now, by looking at a man page you can find the appropriate constant name in that module, though there isn't much structure there. For example, you can check the return type of the GetReferenceEntity, above by doing:
    assert arg1.value == swconst.swSelDATUMPLANES
This isn't quite as nice as the Visual Basic interface, which structures the constants.

The downside of the EnsureModule approach is that it requires that anyone using your beautiful python morsel to run makepy. A more crude approach is to copy the constants you need from the man pages. For example, I have:

class swconst:
    swSelDATUMPLANES = 4
    .... more constants here ...

A prayer for GetMathUtility

And here is the one bit of the API that I can't get to work. For the life of me, I can't seem to get GetMathUtility to work, and so can not figure out how to create a MathPoint. What happens is:
>>> mathUtil = sw.GetMathUtility
>>> mathUtil.CreatePoint
Traceback (most recent call last):
  File "", line 1, in 
  File "C:\Python27\lib\site-packages\win32com\client\", line 511, in __getattr__
    ret = self._oleobj_.Invoke(retEntry.dispid,0,invoke_type,1)
pywintypes.com_error: (-2147417851, 'The server threw an exception.', None, None)
The output I expect is an error saying an argument is missing. I can not find any argument that placates this method, nor any other method in the mathUtil object returned. Kudos to anyone who can figure this out! It works fine in Visual Basic, so my guess is something is either screwed up in the python binding, or there's some kind of bug in the interface that the visual basic binding manages to avoid.


  1. mathUtil = sw.GetMathUtility()

  2. Adding parenthesis only makes it fail earlier:
    Traceback (most recent call last):
    File "", line 91, in
    mathUtil = sw.GetMathUtility()
    File "C:\Python27\lib\site-packages\win32com\client\", line 192, in __call__
    return self._get_good_object_(self._oleobj_.Invoke(*allArgs),self._olerepr_.defaultDispatchName,None)
    pywintypes.com_error: (-2147352573, 'Member not found.', None, None)

  3. In the 2012 version of Solidworks helpfile, CreatePoint appears to require a variant array of coordinates. I assume this is a SafeArray of 3 doubles, 8197.
    I have yet to get this to work by directly editing the proxy stub file.
    I'm working on a Solidworks API problem at present (swModeler.CreateBodyFromBox()) and have used similar techniques to transfer SafeArrays of Dispatch pointers and doubles, swModel.RayIntersections().

  4. Woops, I mean 0x2000 + 0x5 = 0x2005 = 8197

  5. I'm trying to follow along to your post, and after this line:

    modelExt.SelectByID2("Sketch1", "SKETCH", 0, 0, 0, False, 0, arg1, 0),

    I get the following error:

    TypeError: Objects of type 'VARIANT' can not be converted to a COM VARIANT (but obtaining the buffer() of this object could)

    Any idea?

    Great post btw!

  6. I'm not sure what would cause it. Are you using the same kind/version of python as listed in the post? Do you get the same error when trying the other variant arg examples?

  7. woww... great job and nice idea.

  8. Hi Josh,

    My Name is Arvind, I have a small clarification. I wrote a code in vba for dissolving component pattern but it is not getting executed at all and I could not figure out why.

    here is my code:

    Sub main()
    Dim swApp As SldWorks.SldWorks
    Dim swModel As SldWorks.ModelDoc2
    Dim swfeat As SldWorks.Feature
    Dim swComp As SldWorks.Component2
    Dim swRootComp As SldWorks.Component2
    Dim swConfMgr As SldWorks.ConfigurationManager
    Dim swConf As SldWorks.Configuration
    Dim partname As SldWorks.Component2
    Dim swAssy As SldWorks.AssemblyDoc
    Dim swModelDoc As SldWorks.ModelDoc2

    Set swApp = Application.SldWorks
    Set swModel = swApp.ActiveDoc
    Set swAssy = swModel
    Set swfeat = swModel.FirstFeature
    Set swConfMgr = swModel.ConfigurationManager
    Set swConf = swConfMgr.ActiveConfiguration
    Set swRootComp = swConf.GetRootComponent3(True)
    While Not swfeat Is Nothing
    If swfeat.GetTypeName2 = "Reference" Then
    Set swComp = swfeat.GetSpecificFeature2
    If UCase(Right(swComp.GetPathName, 3)) = "ASM" Then
    MsgBox "Assembly:" & swComp.Name2
    ElseIf UCase(Right(swComp.GetPathName, 3)) = "PRT" Then
    MsgBox "Part :" & swComp.Name2
    End If
    End If
    If swfeat.GetTypeName2 = "ReferencePattern" Then
    swfeat.Select (False)
    End If
    Set swfeat = swfeat.GetNextFeature

    End Sub

    Kindly help me out.

  9. Hi Joshua,
    I just stumbled across your nice article above. I have similar issues with MathUtils.

    Did you get in any way closer to a solution ?
    Cheers Frank

  10. With Solidworks 2019 API, I am trying to use the cusPropMgr.GetAll3 from the ICustomPropertyManager class. Here is the code I run:

    PropNames = VARIANT(16396,"")
    PropTypes = VARIANT(16396,"")
    PropValues = VARIANT(16396, "")
    PropLink = VARIANT(16396, "")
    Resolved = VARIANT(16396, "")
    Prop = cusPropMgr.GetAll3(PropNames,PropTypes,PropValues,Resolved,PropLink)

    Analyzing the Data the function send me, the "PropNames" are the "PropLink" and the "PropTypes" are the "Resolved" and vice versa. Is this a Solidworks bug? Have you seen that before? Any fix?

    1. I have spent wayyy to much time solving this. Here is what I finaly got to work.

      import win32com.client
      from win32com.client import VARIANT
      from pythoncom import *

      swApp = win32com.client.Dispatch("SLDWORKS.Application")

      activedoc = swApp.ActiveDoc
      configname = # '' is default
      PropNames = VARIANT(VT_BYREF | VT_VARIANT, '');
      PropTypes = VARIANT(VT_BYREF | VT_VARIANT, '');
      PropValues = VARIANT(VT_BYREF | VT_VARIANT, '');

      # note this modifies the above variables, not return them like you would expect.
      bool_out = = activedoc.Extension.CustomPropertyManager(configname).GetAll(PropNames,PropTypes,PropValues);

      names = PropNames.value # python tuple
      types = PropTypes.value
      values = PropValues.value

      # also, here is how you get mass properties
      mp = swApp.GetMassProperties2(str(paths[0]), "Default", int(3))
      volume = mp[3] # m^3
      surface_area = mp[4] # m^2
      mass = mp[5] # kg

  11. Are there any video tutorials out there on this? Would help us noobs learn a bit faster lol

  12. Is there a way to extract number of mates used in an assembly?

  13. Just wanted to let you know that his has been a Godsend in my first try in writing python scripts to automate SolidWorks.


  14. Thank you for this awsome blog! I was wondering if you could help clarify one more thing: Let's say we write a Macro directly on Solidworks, (In my case, a Macro that rebuilds the shape after I change coordinates of control points), do you know of a way to run the macro from Python? I got an answer about 'sw.bindings.RunMacro' though I do not find any documentations regarding that. Thank you already!

    1. Good question. I don't know offhand. One suggestion is to run python from the command line and try invoking the RunMacro varoius ways manually and see if you can get it to work.

  15. Hi Joshua
    Can you share few python programs which you have worked on Solidworks. I've started learning and your programs would help me learn faster.
    I'll be thankful to you.