Demystifying The Solid Works Api

Demystifying the SolidWorks API
Paul Gimbel, Business Process Sherpa
Razorleaf Corporation

What You Will NOT Hear
This is an INTRODUCTION to the SolidWorks API
Examples – YES
Syntax Details – NO
Not a lesson on how to use the VBA or VSTA Interface
That’s a great idea for another session!
Not a programming class
Not designed for programmers
You won’t hear “Polymorphic Inheritence” used properly in a sentence
Slide 2 of 39,430,177

My Main Goal
I want you to leave here saying:
“I can do that!”
“That even looks like fun”
“That could save me time”
“I could really go for a burrito”

Who Is This Guy and Where Did He Come From?
Razorleaf Corporation
SolidWorks Service Partner
Services ONLY (we’re not trying to sell you anything, we’re neutral)
Data Management (EPDM, SmarTeam, Aras)
Design Automation (DriveWorks, Tacton)
Workflow Automation (Microsoft SharePoint and Tools)
Paul Gimbel (aka “The Sherpa”)
10+ years as Demo Jock, Applications Engineer, Trainer, Support Tech
5 years as Design Automation Implementer
Specializing in SolidWorks, DriveWorks, Tacton, Custom Programming
(THERE! Now I can report this trip as reimbursable.)
The
Sherpa

Where Can I Find Programming?What Languages Can I Use?
Macros: Scripts called from inside of SolidWorks to do things automatically
Macro Features: Scripts run when at a point in the Feature Manager™
Add-Ins: Programs called from inside of SolidWorks through a custom UI
Companion Application: Another program’s macros can call SolidWorks
Standalone Application: A program that you wrote can call SolidWorks
FREE Visual Studio Express - http://www.microsoft.com/express/product/
(Use Coupon Code “RAZORLEAF”)

Why VB.NET?
This presentation uses VB.NET (VSTA) Macros
Macro Recorder (2010) supports VBA, VB.NET, C#.NET
All built into SolidWorks
VBA and VSTA (Visual Studio Tools for Applications) development environments are included with SolidWorks
VB.NET is the current version of VB
VBA is based on VB6 (1998 technology, Support ended 2008)
NOBODY uses VBA anymore…well, except Microsoft Office
Even AutoDesk dropped VBA out of AutoCAD products in January 2010
Tons of examples are out there in VB, more than any other language
Most SolidWorks examples are in VBA (since they’re old)
Not too difficult to convert from VBA to VB.NET

Macro Myths
Macros are in VBA
No Forms/Dialogs
Cannot be automated
Require you to preselect
Cannot handle advanced functionality (like classes)

The Ultimate Process For Non-Programmers
Determine what you want your program/code snippet to do
Think of some “keywords” to describe it (if you know the functions you need to use, you’re ahead of the game)
http://www.google.com (add “VB” or “Visual Basic”)
Ctrl-C
Ctrl-V
Tweak
Test
Tweak
Test
Repeat steps 6-10 ad nauseum
Also check out
www.krugle.org and
www.sourceforge.net
Also look to VBA/VSTA and SW API Help files.
They’re actually somewhat helpful with good examples.
I know! I was shocked, too.

Object-Oriented Programming**
“Everything you need to do in the SolidWorks API has to be done by or to an object.”
Class – A definition (blueprint) of something (think: blank spec for a washer or bolt)
Interface – A more generic definition incorporating multiple classes (ex. Hardware)
Object – A specific instance of a class (completed spec - ex. 1/4-20 x 3 SHCS)
Property – A parameter value that an object has (ex. Diameter)
Method – Something (sub or function) that an object can do (ex. Install)
Accessor – A method used to get an object (ex. GetFeature, GetChildren)
Dot(.) –Separates an object from its property or method or “child” objects
Ex. Bolt.Length or Bolt.Thread.item(“Lead”).Pitch
Instantiate – To make a real thing as defined by a class
Ex. Upper Flange Bolt #3 or Rear Axle Nut
Those are then called “instances” and “objects”
**To appease any true code junkies out there. VBA doesn’t REALLY support full OOP with inheritance and polymorphism, but this is a DEMYSTIFYING session. I don’t want to MYSTIFY this stuff any more than it is.

SolidWorks Objects
“Everything you need to do in the SolidWorks API has to be done by or to an object.”
Everything in SolidWorks (even SolidWorks itself) has an object
The SolidWorks Object Model is a hierarchy of objects/classes/interfaces
You use an object higher in the tree to fetch an object “beneath” it (accessors)
Be prepared to go several steps down (objects beget objects beget objects…)
Be VERY SPECIFIC as to what type of objects you have (fully qualified)
Easier to read
Easier to write (Microsoft will help you)
Learn your way around the HELP file to figure out the object path you need
Throwing darts is most effective in many cases

The SolidWorks API Object Example (VBA)
Early Bound Object Declarations aka “Fully Qualified” (+5 Style Points)
Object assignment (instantiation) requires the keyword Set in VBA only
HoleDepth and HoleDiameter are Properties
of the WizardHoleFeatureData2 object
Example: Creating a Hole Wizard Hole
Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swFeatMgr As SldWorks.FeatureManager
Dim swFeat As SldWorks.Feature
Dim swWzdHole As WizardHoleFeatureData2
Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swFeatMgr = swModel.FeatureManager
…more code here…
Set swWzdHole = swFeatMgr.CreateDefinition(swFmHoleWzd)
swWzdHole.HoleDepth = 0.15
swWzdHole.HoleDiameter = 0.0555
…
Set swFeat = swFeatMgr.CreateFeature(swWzdHole)
…more code here…
CreateDefinition and CreateFeature are Methods (functions)

Seek Professional HelpAn Interface Definition in the API Help

Members = Properties and Methods

Properties have Get and/or Set
x = object.property (Get)
object.property = x (Set)
Methods are actions an object performs

This has Get only. It’s an accessor.

This is no longer a property. It now uses methods to get and set it.
(And forget it)

Old functions never die…

The SolidWorks API Development Process

API Sample #1
Cycle Through All Configurations of a Part

What The Macro Does
Grabs the current open part document (Works only for parts)
Grabs a list of all of the configuration names
Loops through the configurations one at a time
Changes the Material of the configuration
Saves a PDF of the configuration
Sets a configuration-specific custom property value

Important Concepts – Example 1
Programmatic Framework
Accessing Objects
ModelDoc/PartDoc Objects
Accessing / Looping Through Configurations
Editing Material Properties
SaveAs – Exporting File Formats
Adding Custom Properties

Macro Record (VB.NET) – 1 of 2
Legend
Imports SolidWorks.Interop.sldworks
Imports SolidWorks.Interop.swconst
Imports System
Partial Class SolidWorksMacro
Public Sub main()
Dim swDoc As ModelDoc2 = Nothing
Dim swPart As PartDoc = Nothing
Dim swDrawing As DrawingDoc = Nothing
Dim swAssembly As AssemblyDoc = Nothing
Dim boolstatus As Boolean = false
Dim longstatus As Integer = 0
Dim longwarnings As Integer = 0
swDoc = CType(swApp.ActiveDoc,ModelDoc2)
boolstatus = swDoc.Extension.SelectByID2("Unknown", "BROWSERITEM", 0, 0, 0, false, 0, Nothing, 0)
swDoc.ClearSelection2(true)
swPart = CType(swDoc,PartDoc)
swPart.SetMaterialPropertyName2("Copper", "C:/Program Files/SW/lang/english/sldmaterials/SolidWorks "& _
"Materials.sldmat", "Copper")
useless Content

Macro Record (VB.NET) – 2 of 2
boolstatus = swDoc.Extension.SelectByID2("Brass", "CONFIGURATIONS", 0, 0, 0, false, 0, Nothing, 0)
boolstatus = swDoc.ShowConfiguration2("Brass")
boolstatus = swDoc.Extension.SelectByID2("Unknown", "BROWSERITEM", 0, 0, 0, false, 0, Nothing, 0)
End Sub

''' <summary>
''' The SldWorksswApp variable is pre-assigned for you.
''' </summary>
Public swApp As SldWorks

End Class
The Summary explains what the macro does and how it works (that’s why it’s shoved at the end like an afterthought)
This is SUCH an important variable that SolidWorks makes it PUBLIC (then stuffs it at the end where nobody sees it)

Basic Framework (VB.NET)
(Final code does NOT have these)

''' <summary>
''' Put a description, tracking and revision information here
''' </summary>
Public Sub main()
Your code goes here
End Sub ‘main
End Class ‘SolidWorksMacro
Shortcut
Shortcut
!!!ALWAYS Use
macro record
or
Tools>Macro>New!!!


''' <summary>
''' </summary>
Public Sub main()
Your code goes here
End Sub ‘main
DO NOT RENAME HERE
PARTIAL means there’s other stuff you don’t see…LOTS of it.

Renaming Classes
If you feel that you MUST rename things
Rename from the Project Explorer
It will make the update where it needs to
Don’t believe me there’s lots you can’t see? Just click on SHOW ALL.


''' <summary>
''' </summary>
Public Sub main()
Your code goes here
End Sub ‘main
Move these up from the bottom of the class

Do Your Research: HELP>API HELP

Keep Following The Trail

We’ve Got a Lead!
Variants have (rightly) been BANNED from .NET

OK, Now To Find The Method

OK, Now To Find The Method
!!
!!
!!
!!

Performance Characteristics of Key Muppets on Syndicated Educational Television Programs
Mandatory Charts (Gratuitous Chart of Fictitious Data)(per Microsoft PowerPoint code 2009 Section XXIV Subsection 441.K.9.ii.v)

Instantiating an Object Class
Visual Basic.NET requires you to declare your variables
Declare…
PUBLICvariablenameASclassname
DIMvariablenameASclassname
Assign…
variablename = otherVariable.accessor()
Sometimes you need to guarantee the class
variablename = Ctype(oVar.accessor, Class)
variablename = DirectCast(oVar, Class)

Variables! Get Yer Variables Right Here!
PUBLIC declare variables that can be used outside of the module
Useful for your SldWorks.SldWorks and ModelDoc objects
Macro Recorder puts these at the bottom, we recommend the top
DIM or PRIVATE declares a variable for use within a function or sub
Imports SolidWorks.Interop.Sldworks
'''<Summary>
'''Fill this in at some point
'''</Summary>
'Declare the SolidWorks application as global so it can be used throughout the class
PublicswApp As SldWorks'SW Application Object
PublicSub main()
DimbStatusAs Boolean = False ‘Used as SolidWorks return for most functions
DimiErrorsAs Integer = 0
DimiWarningsAs Integer = 0
DimConfigNames() AsString‘The list of names that we’re going to get back
Declare and define in one step
You can define as you go

You’ve Declared, Now Define
SET Keyword is not required for VB.NET or C#.NET (a must in VBA)
Macro Record or Tools>Macro>New will get your SolidWorks object for you
3 Methods of instantiating your SldWorks.SldWorks Object (VBA)
swApp = Application.SldWorks
Grabs existing application (open session REQUIRED)
OK to use in macros
swApp = GetObject( , “SldWorks.Application”)
First parameter is a pathname of file to open
Second parameter is object class
Must have one or the other
If no pathname is specified and SolidWorks is not open, error will occur
swApp = CreateObject(“SldWorks.Application”)
Grabs open SolidWorks application
If no SolidWorks application is open, starts a SolidWorks instance

Use swApp.ActiveDoc to grab currently open document
or ActivateDoc or OpenDoc7 or LoadFile4 or…
Ctype guarantees that we’re getting a ModelDoc2 object
Check API for return, some return “object”
ALWAYS TEST FOR PRESENCE OF AN OBJECT
'Grab the object for the Active SolidWorks Model
DimswDocAs ModelDoc2
swDoc = CType(swApp.ActiveDoc, ModelDoc2)
'Make sure that we have a document object
'If we have no model document object to work with, we cannot go on
IfswDocIs Nothing Then Exit Sub
Got ModelDoc2?
got 3D?
Test Early, Test Often

What is ModelDoc2?...Part? Assembly? Drawing? Yup.
PartDoc Object
MirrorPart
SetMaterialPropertyName2
AssemblyDoc Object
AddComponent
EditMate
DrawingDoc Object
ActivateView
InsertWeldSymbol
ModelDoc2 Object
CustomInfo
CreateLine
EditConfiguration
FeatureCut
FirstFeature
ForceRebuild
InsertNote
Parameter
SaveAs
SetUnits
SketchFillet
…everything else useful
ModelDoc2.Extension
CreateMeasure
GetAnnotations
InsertBomTable
SaveAs
SetUserPreferencex
…and lots more

Use ModelDoc2 to Get Configuration Names
GetConfigurationNames returns an array of strings with our configuration names
Test to make sure that we have names
For Each…Next loop cycles through entries in an array
We dimension new variables “inline” as we go
'Get the list of configuration names. This will be blank where it's not appropriate.
ConfigNames = swDoc.GetConfigurationNames
IfConfigNames.Length >= 1 Then
For Each ConfigNameAs String In ConfigNames
'Switch to the current configuration
bStatus = swDoc.ShowConfiguration2(ConfigName)
'Rebuild the Model
bStatus = swDoc.ForceRebuild3(True)
Must be an array or collection of strings to use For Each …In…
These methods return a boolean (True/False) indicating success. We can (and should) test it.
(NextConfigName– will be coming later)

Get PartDoc and Change Materials
We know that Material requires the PartDoc Object
PartDoc comes directly from ModelDoc2 (DirectCast)
So do AssemblyDoc and DrawingDoc
If there’s a doubt, use Ctype (IF typeofswPart IS PartDoc…)
WARNING!! You may suffer SEVERAL MILLISECONDS performance degradation!!
'Setting the Material is a method of the PartDoc object. We get that object by recasting the ModelDoc2 object.
'WE ONLY USE DIRECTCAST BECAUSE WE’VE TESTED swDoc.GetType. WE ARE CERTAIN IT IS A PART!!!
DimswPartAsPartDoc = DirectCast(swDoc, PartDoc)
…Back in the loop…
'Set the material property for this configuration. This assumes that the configuration name matches an existing material.
swPart.SetMaterialPropertyName2(ConfigName, “M:/RazorleafMatlLib/Materials.sldmat", ConfigName)
We want to do this outside the loop so we only do it once

Save the Model Out As a PDF
'Do a zoom to fit
swDoc.ViewZoomtofit2()
'Retrieve the full pathname including the file name
DimsFileNameAsString = swDoc.GetPathName
'Remove the extension
sFileName = sFileName.Remove(sFileName.LastIndexOf(".")) 'remove all text after the last dot
bStatus = swDoc.Extension.SaveAs(sFileName & "_" & ConfigNames(index) & ".pdf", _
swSaveAsVersion_e.swSaveAsCurrentVersion, _
swSaveAsOptions_e.swSaveAsOptions_Silent, _
Nothing, iErrors, iWarnings)
.NET string members, check ‘em out!
_ means “Continued on next line”
Must have a space before it
enumerations
More return values, listed as ByRef in the Class Definition

Enumerations
Parameter values can be integer or long in many cases
What is the integer for SolidWorks 2009?
Enumerations replace numbers
IMPORTS SolidWorks.Interop.swconst
That’s the Type Constant Library
My code fully qualifies
Intellisense will help you if you fully qualify
Enumerations are more readable
ByVal means input
ByRef means output

Set Configuration-Specific Custom Property
AddCustomInfo3 allows you to specify a configuration
Be sure to comment your loop and IF closers
swDoc.AddCustomInfo3(ConfigName, "Material Code", _
swCustomInfoType_e.swCustomInfoText, ConfigName.Remove(4))
NextConfigName'move to the next configuration
End If 'there are one or more configurations in the document
End Sub ‘main
Another kewl .NET string function
Documenting here makes blocks easier to follow and troubleshoot

Configuration Master 5000
Complete Code

Final Code: Configuration Master 5000 (Part 1 of 5)
'''<Summary>
'''Sample Code for SolidWorks World 2010: Demystifying the SolidWorks API
'''Razorleaf Corporation -- Paul Gimbel -- January 20, 2010
'''This macro loops through all of the configurations of a part
'''For each configuration, it saves a PDF, changes the material of the configuration and adds a configuration-specific custom property
'''See the Powerpoint Presentation (available from www.razorleaf.com) for complete documentation of the code
'''</Summary>
'Declare the SolidWorks application as a global variable so it can be used throughout the class
PublicswApp As SolidWorks.Interop.sldworks.SldWorks 'SolidWorks Application Object
PublicSub main()
DimbStatusAs Boolean = False
DimiErrorsAs Integer = 0
DimiWarningsAs Integer = 0
DimConfigNames() AsString

'Grab the object for the Active SolidWorks Model
DimswDocAs SolidWorks.Interop.sldworks.ModelDoc2 = CType(swApp.ActiveDoc, SolidWorks.Interop.sldworks.ModelDoc2)
'Make sure that we got a document object
IfswDocIs Nothing Then Exit Sub 'We have no model document to work with, we cannot go on
'This macro is only for part models. Check what type of document we have.
IfswDoc.GetType <> SolidWorks.Interop.swconst.swDocumentTypes_e.swDocPARTThen Exit Sub
'Get the list of configuration names. This will be blank where it's not appropriate.
ConfigNames = swDoc.GetConfigurationNames
'WE ONLY USE DIRECTCAST BECAUSE WE HAVE ALREADY TESTED swDoc.GetType. WE ARE CERTAIN IT IS A PART!!!
DimswPartAsSolidWorks.Interop.sldworks.PartDoc = DirectCast(swDoc, SolidWorks.Interop.sldworks.PartDoc)
If ConfigNames.Length >= 1 Then
For Each ConfigNameAs String In ConfigNames
'Switch to the current configuration
bStatus = swDoc.ShowConfiguration2(ConfigNames(index))

''<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
''Drive the material to be equal to the configuration name
''<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
'Set the material property for this configuration. This assumes that the configuration name matches an existing material.
swPart.SetMaterialPropertyName2(ConfigNames(index), _
"C:/Program Files/SolidWorks Corp/SolidWorks/lang/english/sldmaterials/SolidWorks " & "Materials.sldmat", _
ConfigNames(index))

''<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
''Save this configuration out as a PDF
''<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
'Do a zoom to fit
swDoc.ViewZoomtofit2()
'Retrieve the full pathname including the file name
DimsFileNameAsString = swDoc.GetPathName
'Remove the extension
sFileName = sFileName.Remove(sFileName.LastIndexOf(".")) 'remove from the location of the last dot on to the end
bStatus = swDoc.Extension.SaveAs(sFileName & "_" & ConfigNames(index) & ".pdf", _
SolidWorks.Interop.swconst.swSaveAsVersion_e.swSaveAsCurrentVersion, _
SolidWorks.Interop.swconst.swSaveAsOptions_e.swSaveAsOptions_Silent, _
Nothing, iErrors, iWarnings)

''<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
''Create a configuration specific custom property -
'' Material Code = 1st 4 letters of the material
''<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<<
swDoc.AddCustomInfo3(ConfigNames(index), "Material Code", _
SolidWorks.Interop.swconst.swCustomInfoType_e.swCustomInfoText, _
ConfigNames(index).Remove(4))
NextConfigName'move to the next configuration
End If 'there are one or more configurations in the document
End Sub ‘main

API Example #2
Suppressing Pattern Instances

Delete Pattern Instances
Part has one or more linear patterns
Custom property stores a text string of Xs and Os
X means there will be an instance here
O means that instance will be removed
Main Errors to check for:
No pattern features
No instance to suppress
Text string length ≠ Number of pattern instances
XOOXXOXOOXOXOOXOXOOXOXOO

Important Concepts – Example 2
Accessing Feature objects
Looping through all features in a part
Handling FeatureData objects
Reading custom properties

Recorded Macro: Remove Pattern Instances
Legend
Public Sub main()
Dim swDoc As ModelDoc2 = Nothing
Dim swPart As PartDoc = Nothing
Dim swDrawing As DrawingDoc = Nothing
Dim swAssembly As AssemblyDoc = Nothing
Dim boolstatus As Boolean = false
Dim longstatus As Integer = 0
Dim longwarnings As Integer = 0
swDoc = CType(swApp.ActiveDoc,ModelDoc2)
Dim myModelView As ModelView = Nothing
myModelView = CType(swDoc.ActiveView,ModelView)
myModelView.FrameState = CType(swWindowState_e.swWindowMaximized,Integer)
boolstatus = swDoc.Extension.SelectByID2("HolePattern", "BODYFEATURE", …)
boolstatus = swDoc.Extension.SelectByID2("", "EDGE", -0.04, 0.0127,…)
boolstatus = swDoc.Extension.SelectByID2("", "EDGE", -0.1016, …)
swDoc.ActivateSelectedFeature()
End Sub
Helpful Content

Seek the Path of Enlightenment
How do we get the info we need out of the object?
How do we get the object?

Find The Right Property or Method

OK, So How Do We Get The Object, Then?
Accessors List

IFeature.ILinearPatternFeatureData.SkippedItemArray
Let’s limit it to just ModelDoc2 and PartDoc
Once you have a feature, you can use it to get the next one

The Full Object Path
ModelDoc2
Feature
Feature IS Linear Pattern
Feature IS NOT Linear Pattern
LinearPattern
FeatureData

Set up the Framework and Grab the ModelDoc2
IMPORTS SolidWorks.Interop.sldworks
IMPORTS SolidWorks.Interop.swconst
''' <summary>
''' Don’t forget to put this in at some point!!
''' </summary>
PublicswAppAsSldWorks
Public Sub main()
‘A nice description here goes a long way!
'Get currently open document
DimswPartAs ModelDoc2 = CType(swApp.ActiveDoc, ModelDoc2)
'Make sure that we have an object
IfswDocIs Nothing Then Exit Sub
'This macro is only for part models. Check our document type.
IfswDoc.GetType <> swDocumentTypes_e.swDocPARTThen Exit Sub

Test for Proper Conditions and Get Feature Object
'Fetch the custom property list
DimsInputListAs String = swDoc.GetCustomInfoValue("", "SkipList")
'If the list does not exist, exit out of the function. We do not need to run the macro.
If sInputList.Length < 1 Then Exit Sub
'Get the first feature in the part.
'NOTE!! THIS DOES NOT MEAN THE BASE EXTRUSION.
'There are reference features.
DimswFeatureAs Feature
swFeature = swDoc.FirstFeature()
Declare as you define
Always put your tests up front - Try to run as little code as possible
Look how far down the tree the base extrusion is!

Loop the Loop
'We know from our research that we'll need the LinearPatternFeatureData
' object, the feature type, and some indices.
'We'll declare them outside of the loop so they only get declared once.
DimswFeatureDataAsLinearPatternFeatureData
DimsFeatureTypeAs String 'Type of feature
DimiRowsAs Integer 'Number of rows in the pattern
DimiColsAs Integer 'Number of columns in the pattern
DimTempStringAs String = ""
Do While swFeatureIsNotNothing'loop through the features
…OUR CODE GOES HERE…
Loop
DO WHILE tests BEFORE running any code
(Do … Loop Until tests after)
Got an object?
IsNot Nothing will tell you

Looping and Testing
Do While swFeatureIsNotNothing'loop through the features
'Check to see if this is a pattern feature
sFeatureType = swFeature.GetTypeName2
IfsFeatureType = "LPattern" Then'we have a pattern to process
swFeatureData = swFeature.GetDefinition'get the feature data
iRows = swFeatureData.D1TotalInstances
iCols = swFeatureData.D2TotalInstances
'Check to ensure that list matches pattern size
IfsInputList.Length = iRows * iColsThen'we're good to go
… The actual work goes here…
End If 'The list length matches the pattern size
End If 'This is a linear pattern feature
Loop 'through the features
Browse API Help
to see properties
Test Early, Test Often

Arrays and Collections
Array
Think of it as a bin system for values
Can be 1D, 2D or more
It’s a fixed size (you need to REDIM to change it)
Tough to move things around in
Collection
Think of it as a collection of stackable bins
Need another? Just add it!
Rearranging, sorting, searching…no prob, Bob!
Don’t know collections? Take the time to look them up!!
7
5
9
11
7
8
5
2
1
2
2
2
3
0
10
3
4
3
6
4
6
9
2
6

Numbering Sequence for Linear Pattern Instances
SEED = 0
(Row 1, Col 1)
5
10
15
20
(2, 1)=1
6
11
16
21
(3, 1)=2
7
12
17
22
(4, 1)=3
8
13
18
23
(5, 1)=4
9
14
19
24

Create the Skipped Instance Array
'Create a collection for the list of instances to be skipped
DimSkipColAs New System.Collections.Generic.List(OfInteger)
'Go through the characters in the string finding the O's and add that index
For Index As Integer = 0 TosInputList.Length - 1
IfsInputList.Substring(Index, 1).Equals _
("O", StringComparison.CurrentCultureIgnoreCase) Then
'add this to the list of excluded items
SkipCol.Add(Index)
End If 'we need to add this entry to the skipped list
Next Index 'move to the next character in the string
Substrings start at 0
String method .Equals
How can I remember that?!!? You don’t. Intellisense gives it to you!
The input list “XXOOXOXO”…
…results in the collection: (2,3,5,7)
0
1
2
3
4
5
6
7

Update the Feature and Error Handling
'pass the collection as an array to the LinearPatternFeatureData object
swFeatureData.SkippedItemArray = SkipCol.ToArray()
'Tell SolidWorks to update the LinearPattern with the new information
swFeature.ModifyDefinition(swFeatureData, swDoc, Nothing)
'Rebuild the model
swPart.ForceRebuild3(False)
Else'the input size doesn't match the pattern size
DIMsMessageAs String = "Pattern Size "& (iRows * iCols) &"doesn’t match input size "&sInputList.Length
System.Windows.Forms.MessageBox.Show(sMessage)
swPart.AddCustomInfo3("", "Code Errors", 30, sMessage)
End If'the input size matches the pattern size
One of many collection methods
These methods are subs, no returns
& joins strings and values
“I’m “ & iAge & “ years old”
= “I am 4257 years old”

The Amazing Disappearing Pattern Instance trick
Complete Code

Finished Code (Part 1 of 4)
''' <summary>
'''Sample Code #2 for SolidWorks World 2010: Demystifying the SolidWorks API
'''Razorleaf Corporation -- Paul Gimbel -- January 20, 2010
'''This macro removes instances within a linear pattern based on a string input of X's and O's stored in a custom property.
'''The code loops through all of the features of a part looking for linear patterns.
'''For each linear pattern that it finds, it compares the input string length to the pattern size.
'''If the string matches the pattern, the code builds the SkippedInstanceArray and updates the pattern.
'''See the Powerpoint Presentation (available from www.razorleaf.com) for complete documentation of the code
''' </summary>
DimswAppAsSolidWorks.Interop.sldworks.SldWorks
Public Sub main()
'Reads a list stored as a string from a custom property named "SkipList" (populated by DriveWorks)
'This list will contain an "X" if the pattern instance is to be there and an "O" (Letter Oh) if it is to be removed
'The list walks down a column, then starts at the next column, just as SolidWorks does
'When Skipping, the instances are numbered as such (Row,Col):
' (1,1) = 0, (2,1) = 1, (3,1) = 2
' For a 3x3 array, (1,2) = 3, (2,2) = 4 and so on.
'Get currently open document
DimswPartAs SolidWorks.Interop.sldworks.ModelDoc2 = CType(swApp.ActiveDoc, SolidWorks.Interop.sldworks.ModelDoc2)

'Fetch the custom property list
DimsInputListAs String = swPart.GetCustomInfoValue("", "SkipList")
'If the list does not exist, exit out of the function. We do not need to run the macro.
If sInputList.Length < 1 Then Exit Sub
'Get the first feature in the part. NOTE!! THIS DOES NOT MEAN THE BASE EXTRUSION. There are reference features.
DimswFeatureAsSolidWorks.Interop.sldworks.Feature = swPart.FirstFeature()
'We know from our research that we'll need the LinearPatternFeatureData object, the feature type, and some indices.
'We'll declare them outside of the loop so that they only get declared once.
DimswFeatureDataAsSolidWorks.Interop.sldworks.LinearPatternFeatureData
DimsFeatureTypeAs String 'Type of feature to test to see if it's a linear pattern
DimiRowsAs Integer 'Number of rows in the pattern
DimiColsAs Integer 'Number of columns in the pattern
DimTempStringAs String = ""
Do While swFeatureIsNotNothing'loop through the features checking to see if the feature is a pattern
'Check to see if this is a pattern feature
sFeatureType = swFeature.GetTypeName2
IfsFeatureType = "LPattern" Then'we have a pattern to process
swFeatureData = swFeature.GetDefinition'get the feature information object
iRows = swFeatureData.D1TotalInstances 'get the information that we want
iCols = swFeatureData.D2TotalInstances
'Check to ensure that list matches pattern size
IfsInputList.Length = iRows * iColsThen'we're good to go

'Create a collection for the list of instances to be skipped
DimSkipColAs New System.Collections.Generic.List(OfInteger)
'Go through the collection finding the O's and add the index of that character to the collection
For Index As Integer = 0 TosInputList.Length - 1 'cycle through the characters in the string
IfsInputList.Substring(Index, 1).Equals("O", StringComparison.CurrentCultureIgnoreCase) Then
'add this to the list of excluded items
SkipCol.Add(Index)
TempString = TempString & CStr(Index)
End If 'we need to add this entry to the skipped list
Next Index 'move to the next character in the string
'Convert the collection into an array and pass it to the LinearPatternFeatureData object
swFeatureData.SkippedItemArray = SkipCol.ToArray()
'Tell SolidWorks to update the LinearPattern with the new information
swFeature.ModifyDefinition(pFeatureData, pPart, Nothing)
Else'the input size doesn't match the pattern size
'During testing you can have it pop up a message box
'System.Windows.Forms.MessageBox.Show _
' ("Pattern Size (" & iRows * iCols & ") does not match input size (" & Len(sInputList) & ")")
'During Production, have it write the error to a custom property
swPart.AddCustomInfo3("", "Code Errors", 30, "Pattern Size (" & iRows * iCols & ") does not match input size (" & sInputList.Length & ")")

End If 'there are the correct number of entries in the list
End If 'this is a pattern feature
'Go fetch the next feature
swFeature = swFeature.GetNextFeature
Loop'while pFeatureIsNot Nothing
End Sub 'main
End Class 'PARTIAL SolidWorksMacro

PROGRAMMING Best Practices
What Not To Wear: SolidWorks API Edition

Programming Tips For SolidWorks
DOCUMENT THE $#^@ OUT OF EVERYTHING!!!
Anything after an apostrophe in VB (‘) or (//) in C# is a comment…use them!!
Intellisense…good. Typing…bad.
If you don’t see the option that you need, something’s wrong.
Test for Errors
Don’t run code if you don’t have to
Runtime errors make you look like a doofus
Compile and Test Often
Programmatic sanity checks
Insert Test Code (Debug.Print, msgbox, extraneous IF’s you can comment out)
Use Debug Tools
Step Into, Step Over, Watches, Breakpoints, Immediate window, Stack trace, …
Errors/Warnings window at the bottom IS YOUR FRIEND!!

Documenting Your Code - Comments
VB will ignore anything after an apostrophe (‘)
C# will ignore anything after two forward slashes (//)
The editor will turn all comments green
Turn your code into complete sentences
IfswSensor.SensorType = swSensorDimensionThen‘find the dimension
Else‘we need to see if this is a mass property sensor
End If ‘this is a dimension sensor
Keep track of the end of nested loops and if statements (don’t miss them!)
End If ‘the width is over the threshold value
End If ‘the width is greater than the length
Create section headers (Visual Studio has tools for this as well)
‘Set all of the hole wizard feature parameters

Early Binding and Fully Qualifying – Great Practices
Option Explicit in VBA (implicit in VB.NET and C#.NET)
DIMswFeatureAs Object
Perfectly legal (with IMPORTS), but sloppy
DIMswFeatureAsSolidWorks.Interop.sldWorks.Feature = swPart.GetFirstFeature
Better documented
Will catch more errors
Enables Intellisense

Error Trapping
End Users do NOT take errors well
Small errors can snowball
TRY…CATCH
OnErrorGotoerrhandler
errhandler:
Iferr.number > 0 Then‘we have an error, deal with it
msgbox(“You have a problem with ” & err.description)
EndIf‘we have an error
ALWAYS test for objects
IfswFeatureIsNotNOTHINGThen‘we have a feature, go
Watch for data types and illegal values (negatives, zeroes, “artichoke”, etc.)
Look for anything that will make your code or SolidWorks barf

Go Hungarian!
Hungarian Notation places the data type at the front of the variable name
Examples:
Dim iCounter as Integer
Dim bResult as Boolean
Dim dLength as Double
Dim swApp as SolidWorks.Interop.SldWorks.SldWorks
(here “sw” indicates it’s a SolidWorks object)
Microsoft (and Bob) now recommends against it – The Sherpa recommends it!!
But Visual Studio Intellisense tells you the data type, it’s redundant
VBA doesn’t have that feature
Neither does my printer
What if the data type changes!??!!?
Find/Replace – It’s 5 clicks
If you always declare your variables, it’s documented
So I have to scroll to the top every time?
Violent objection?
Don’t use it.
Arguments Against HN

Code You Should Know
Loops (DO, WHILE, FOR, FOR EACH)
IF…THEN…ELSEIF…ELSE (with AND, OR, NOT)
SELECT CASE
WITH Blocks
Msgbox
String Manipulation (.Length , .Remove, .Substring, .Trim, …)
CHR()
Collections and Arrays
Exit Sub (-5 Style Points, but it’s cheap and easy)
Err Object
Math (ABS, Trig, SQRT, Int)
File I/O (Write, Print, Input, LineInput, Open Append/Output, Close)
DB Access (ODBC, ADODB, DAO)

What Else can the API do?
API and Beyooooooooooond

API Areas
APIs exist for tons of SolidWorks Modules
Automating Design Validation - Tomorrow @ 1:30
Integrate with other programs
Automating With Excel – Wednesday @ 1:30
MathCAD or custom calculation engines
Read from/Write to your ERP or other system
Allow less-sophisticated users to use advanced features
Build an interface for non-SolidWorks users that drives SolidWorks
Cut mouse clicks out of your day
Automate iterative processes
Build the model, run a test, use results to rebuild, run a test, again…

Macro Features - How Will YOU Use Them?
Two Steps: 1) Write the macro, 2) Write a macro to insert the macro
Macro feature appears in the SolidWorks Feature Manager™
Macro is executed based on its position in the Feature Manager™
Code is contained in an SWP file or a registered application* on your machine
*For the advanced: code must be in an exposed COM DLL or executable
Everyone must have access to this code to be able to use it
Your code contains 2-4 functions
What to do when the macro feature is created (optional)
What to do when the macro feature is rebuilt (mandatory)
What to do when the macro feature is edited (mandatory)
Can feature be deleted, suppressed or edited (VBA = optional, COM = mandatory)
If you use multiple (older) versions of SolidWorks and wish to use Macro Features, check out the API Help article on Macro Features and Strong Name Versioning

Questions? Comments? Suggestions? Amusing Pet Stories?
If you have questions you would like to discuss, please find me
Now…At any time during the conference…or After the conference
Presentation available on www.razorleaf.com
Free newsletter with tech tips, industry insiders, free code, and more…
Catch me in my upcoming tour dates!!
Tuesday @ 1:30 – Automating Design Validation with the SolidWorks API
Wednesday @ 1:30 – Automating Your Designs with Excel and the SW API
The
Sherpa
Paul Gimbel
Business Process Sherpa
paul.gimbel@razorleaf.com
www.razorleaf.com
TheProcesSherpa on Twitter

SURVEY TIME!!!
Paul Gimbel, Razorleaf Corporation
paul.gimbel@razorleaf.com
@TheProcesSherpa on Twitter
PLEASE PLEASEPLEASE fill out your survey
It takes practically no time at all
I HONESTLY want your feedback and I do apply it
Let’s see if the SolidWorks folks read these:
PLEASE PLEASEPLEASE fill out your survey
It takes practically no time at all
I HONESTLY want your feedback and I DO apply it
Let’s see if the SolidWorks folks read these:
In the comments section, PLEASE end with:
“Wow, he was right. These burritos are quite tasty!”

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Demystifying The Solid Works Api

by Razorleaf Corporation on Feb 01, 2010

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Demystifying The Solid Works Api — Presentation Transcript