API Opening each part file in an assembly. 2

[cadnutcase]

I am giving a shot at this API stuff and so far really like it but I am having a hard time with the following.

I want to open up each part file no matter how deep an a assembly file. Run a special macro that I have, and then close the file.

I am using the traverse assembly macro out of the help section, and I put a line in there for I want to open the part file (I think it is in the right place).

What am I missing here?

'Make All Assembly Components Visible Example (VB)
'This example shows how to make all assembly components visible.



'---------------------------------------

'

' Preconditions: An assembly document is open.

'

' Postconditions: Any hidden assembly components are made visible.

'

'---------------------------------------

Option Explicit

Dim swApp As SldWorks.SldWorks

Dim swPart As SldWorks.ModelDoc2

Dim swFeat As SldWorks.Feature

Dim Indent As Long





Sub TraverseComponent(swComp As SldWorks.Component2, nLevel As Long)

Dim vChildCompArr As Variant

Dim vChildComp As Variant

Dim swChildComp As SldWorks.Component2

Dim swCompConfig As SldWorks.Configuration

Dim sPadStr As String

Dim i As Long



For i = 0 To nLevel - 1

sPadStr = sPadStr + " "

Next i



vChildCompArr = swComp.GetChildren

For Each vChildComp In vChildCompArr

Set swChildComp = vChildComp

Debug.Print sPadStr & swChildComp.Name2 & " <" & swChildComp.ReferencedConfiguration & ">"

' Right here is where I want to open the part file and run my other macro

TraverseComponent swChildComp, nLevel + 1

Next

End Sub



Sub main()

Dim swApp As SldWorks.SldWorks

Dim swModel As SldWorks.ModelDoc2

Dim swAssy As SldWorks.AssemblyDoc

Dim swConf As SldWorks.Configuration

Dim swRootComp As SldWorks.Component2

Dim bRet As Boolean



Set swApp = Application.SldWorks

Set swModel = swApp.ActiveDoc

Set swConf = swModel.GetActiveConfiguration

Set swRootComp = swConf.GetRootComponent



Debug.Print "File = " & swModel.GetPathName



TraverseComponent swRootComp, 1

End Sub

 

[alexit]

Starting after this line:

vChildCompArr = swComp.GetChildren

Put this:

For Each vChildComp In vChildCompArr
Set swChildComp = vChildComp

swModDoc = swChildComp.GetModelDoc()

FileTyp = swModelDoc.GetType
strPrt = swModDoc.GetPathName

If FileTyp = swDocPART Then
Set Part = swApp.OpenDoc6(strPrt, swDocPART, swOpenDocOptions_Silent, "", longstatus, longwarnings)
End If

If FileTyp = swDocASSEMBLY Then
Set Part = swApp.OpenDoc6(strPrt, swDocASSEMBLY, swOpenDocOptions_Silent, "", longstatus, longwarnings)
End If


And erase everything until here:

' Right here is where I want to open the part file and run my other macro

TraverseComponent swChildComp, nLevel + 1

Next

End Sub

 

[cadnutcase]

Thanks alexit,

The only problem I got now is defining the new variables that you put in.

I am guessing the following:
dim swModDoc as sldworks.modeldoc2
dim filetyp as long
dim strPrt as long
dim part as object
dim longstatus as long
dim longwarnings as long
Dim swModelDoc As SldWorks.Component2

Thanks for the help

 

[cadnutcase]

I am having a problem with this line, but I am pretty sure it is the way I am defining it

swmoddoc = swChildComp.GetModelDoc()

 

[handleman]

How "open" do you need the files to be? If you open the assembly file each part file is opened in memory unless it is either suppressed or lightweight. You can then traverse through the collection of all open documents, making them visible if you need to. If what you want is to open all parts as if for editing, you can strip out a few lines from the macro at faq559-1231 and be done.

 

[fcsuper]

ditto to cadnutcase's issue here.

 

[cadnutcase]

Okay here is the whole problem.

I am trying to open each part file from one master assembly file and export specific cut list properties from each body to an excel spread sheet would be nice, text delimited file would be just as good.

It seems that the other macros that I am using the file has to be open and current to export the properties.

If somebody has a macro to do this already, I would gladly send them some beer money, I am tired of screwing around with this. Especially since it is something that I think Solidworks should do already.

Yes I have sent an enchanment request.
Yes I have complained to my VAR.
Yes I am going home for the night.

 

[handleman]

Sorry, I should have explained further. Any time you open an assembly all part files that are not suppressed or lightweight are opened automatically. Each open file is a ModelDoc2 object and has a True/False .Visible property. This is different from component visibility in the assembly. The Visible property is true on any file (part, assembly, or dwg) that has a graphics window and false on files that are open just because a visible file references it. I've stripped away lines of the macro I referenced above. I've marked where you can call your other macro.

Sub ActivateOpenFilesAndRunMyMacro()
Dim swDoc As SldWorks.ModelDoc2
Dim swAllDocs As EnumDocuments2
Dim FirstDoc As SldWorks.ModelDoc2
Dim dummy As Boolean
Dim NumDocsReturned As Long
Dim DocCount As Long
Dim i As Long
Dim sMsg As String
Dim swApp As SldWorks.SldWorks
Dim bDocWasVisible As Boolean

Set swApp = Application.SldWorks
Set swAllDocs = swApp.EnumDocuments2
Set FirstDoc = swApp.ActiveDoc

DocCount = 0
swAllDocs.Reset
swAllDocs.Next 1, swDoc, NumDocsReturned
While NumDocsReturned <> 0
    bDocWasVisible = swDoc.Visible
    swApp.ActivateDoc swDoc.GetPathName
'************************
'*Call your macro that works on the open, visible, active
'*document here
'************************
    swDoc.Visible = bDocWasVisible
    swAllDocs.Next 1, swDoc, NumDocsReturned
    DocCount = DocCount + 1
Wend

swApp.ActivateDoc FirstDoc.GetPathName
End Sub

 

[Stoker]

You may want to have a close look at Thread559-155921. This is a very similar situation in that it iterates through the child components of an assembly looking at properties. Be aware that iterating through child components will result in a child doc being returned once for every instance. If you do use the iteration approach you will be calling child parts more than once when there are multiple instances and will have to reject the duplicate entries as you step through the tree.

If you take the enum documents route of iterating through the open docs as Handleman suggested, be aware that it will look at all open documents. Therefore if you have other docs in addition to your assembly open they will be captured by the code. You should test for this if you want to make the routine bulletproof.

 

[handleman]

Good call by Stoker. Since you're putting together some sort of master cut list I'm guessing you'll want every instance counted. If that's the case, (mostly) ignore my posts.

 

[cadnutcase]

Actually I want it to look at every instance. Basically once I get a master cut list put together. I can sum all the like parts in excel, export that to a one-dimensional bin packing program, and I can let our purchasing department know how many randoms to buy.

I appreciate all the help from alexit, stoker and handleman. If I get this thing working and anybody is interested in it, I will post the final code.

cadnutcase

 

[RacingD98]

This is great.

Many a time I've gone through my assembly file opening up the parts one at a time so that I can work on them. A lot of the time I also will open the drawing file for each part. Is it possible to add a few lines of code to this macro to allow the assoiciate drawing file to open when the part file opens?

I always have my drawing files and part file in the same directory and the drawing file has the same file name as its
part file.

thanks in advance
racingd98

 

[handleman]

Are you talking about the macro I posted? If so, and you want all the files to be shown and not re-hidden, you will have to comment out the line

swDoc.Visible = bDocWasVisible

If, as you say, the drawing file is always in the same folder as the part file with the same name, you can definitely add a few lines to do that. You would probably use swDoc.GetPathName to get the path of the current part file, strip off the extension and replace with .slddrw, and open the file with OpenDoc6. Of course, you'd have to first test and see if that file exists. You can do that with standard VBA functions.

Be warned that opening a bunch of graphics windows will likely hurt your performance.

 

[RacingD98]

Yes, I forgot to post that I had already stripped that piece of code from what you posted. It works really good for opening the part files up and keeping them open. I guess when I get time to play I'll add the code (or at least try) for opening the drawing files. Most of my code writting is just dabbling and not real code work. i have a lot to learn.

thanks

 

[handleman]

Try this one, RacingD. I think the existence check may not be necessary if we check to see if OpenDoc6 succeeds in setting myDwgDoc to an object. No guarantees that this code even works, as I'm typing straight into my browser.

Sub ActivateOpenFilesAndRunMyMacro()
Dim swDoc As SldWorks.ModelDoc2
Dim swAllDocs As EnumDocuments2
Dim FirstDoc As SldWorks.ModelDoc2
Dim dummy As Boolean
Dim NumDocsReturned As Long
Dim DocCount As Long
Dim i As Long
Dim sMsg As String
Dim swApp As SldWorks.SldWorks
Dim bDocWasVisible As Boolean
Dim OpenWarnings as Long
Dim OpenErrors as Long
Dim DwgPath as String
Dim myDwgDoc as SldWorks.ModelDoc2

Set swApp = Application.SldWorks
Set swAllDocs = swApp.EnumDocuments2
Set FirstDoc = swApp.ActiveDoc

DocCount = 0
swAllDocs.Reset
swAllDocs.Next 1, swDoc, NumDocsReturned
While NumDocsReturned <> 0
    bDocWasVisible = swDoc.Visible
    swApp.ActivateDoc swDoc.GetPathName
    DwgPath = swDoc.GetPathName
    If LCase(Right(DwgPath,3)) <> "drw" Then
        DwgPath = Left(DwgPath, Len(DwgPath-3)) & "drw")
        Set myDwgDoc = swApp.OpenDoc6(DwgPath, swDocDwg, swOpenDocOptions_Silent, "", OpenErrors, OpenWarnings)
        If Not myDwgDoc Is Nothing Then
            swApp.ActivateDoc myDwgDoc.GetPathName
            set myDwgDoc = Nothing
        End If
    End If
    swAllDocs.Next 1, swDoc, NumDocsReturned
    DocCount = DocCount + 1
Wend

swApp.ActivateDoc FirstDoc.GetPathName
End Sub

 

[RacingD98]

Handleman, thanks for your help. I tried your code but unfortunately, it fails on:

DwgPath = Left(DwgPath, Len(DwgPath-3)) & "drw")

I did change it to read:

DwgPath = (Left(DwgPath, Len(DwgPath - 3)) & "drw")

But it continues to fail on the -3 part, I think.

RacingD98

 

[handleman]

Oops, misplaced parenthesis. Should read:

DwgPath = Left(DwgPath, Len(DwgPath)-3) & "drw"

Sorry!

 

[handleman]

Found another problem this morning when I tried to run it. In the OpenDoc6 line swDocDwg should be swDocDRAWING, as below. This macro now works as is on my m/c.

Sub ShowAllOpenFiles()
Dim swDoc As SldWorks.ModelDoc2
Dim swAllDocs As EnumDocuments2
Dim FirstDoc As SldWorks.ModelDoc2
Dim dummy As Boolean
Dim NumDocsReturned As Long
Dim DocCount As Long
Dim i As Long
Dim sMsg As String
Dim swApp As SldWorks.SldWorks
Dim bDocWasVisible As Boolean
Dim OpenWarnings As Long
Dim OpenErrors As Long
Dim DwgPath As String
Dim myDwgDoc As SldWorks.ModelDoc2

Set swApp = Application.SldWorks
Set swAllDocs = swApp.EnumDocuments2
Set FirstDoc = swApp.ActiveDoc

DocCount = 0
swAllDocs.Reset
swAllDocs.Next 1, swDoc, NumDocsReturned
While NumDocsReturned <> 0
    bDocWasVisible = swDoc.Visible
    swApp.ActivateDoc swDoc.GetPathName
    DwgPath = swDoc.GetPathName
    If (LCase(Right(DwgPath, 3)) <> "drw") And (DwgPath <> "") Then
        DwgPath = Left(DwgPath, Len(DwgPath) - 3) & "drw"
        Set myDwgDoc = swApp.OpenDoc6(DwgPath, swDocDRAWING, swOpenDocOptions_Silent, "", OpenErrors, OpenWarnings)
        If Not myDwgDoc Is Nothing Then
            swApp.ActivateDoc myDwgDoc.GetPathName
            Set myDwgDoc = Nothing
        End If
    End If
    swAllDocs.Next 1, swDoc, NumDocsReturned
    DocCount = DocCount + 1
Wend

swApp.ActivateDoc FirstDoc.GetPathName
End Sub

 

[RacingD98]

Handleman,

oooooooooohhhhhhhh, so sweet.

thanks a ton, this will save me so much time.

thanks again, RacingD