API: inserting a component from a file

Hello,

I was experimenting a bit with the api (using VB), trying to insert a
component to an assembly & then mate it to another component.
But it got all a bit confusing as I found there are seemingly various ways.
(& I'm quite a newbie to it)

The simplest way I thought to be was using ".addcomponent4 ( compName,
configName, x, y, z)"
but this method requires a part already to be loaded into memory & that's
where I got stuck.

I tried opening it with ".OpenDoc6" & it's various options, but then I get
the particular part opened in a part document.
Is there a way to "load" a component without actually opening it in a
separate document then ?

Could anybody lighten me up a bit on this, or on which method is actually
best used to insert a component from a file ?

TIA & best regards,
JM

 

Try using AssemblyDoc.AddComponents, which adds multiple components. There
is no mention in the API documentation that this function needs the parts to
be loaded first. Furthermore, I just tried it out and it works for me
without the parts being loaded first. There is an example in the API
documentation - Add Components Example (VB) - that you can modify.

 

open the part with OpenDoc6 and make sure you use
swOpenDocOptions_Silent option. then insert it into your assembly with
addcomponent4. after that close the doc with ModelDoc2::Close.

hope this helps

 

Hi Paul, thanks for your answer.
I had been looking at this example before, but its realy 'general', more
like a description then an example.
E.g. where does "txtCompCount.Text" come from ?
I' try to strip the example leaving the bare necessities.

Best regards
JM

 

Hi Sean, thanks for your suggestion,
I tried that option, but it doesn't seem to behave 'silently'
As a matter of fact, the part to be inserted does get opened in a window &
gets focus before it gets inserted into the assembly. Unless I'm looking
over something....

Best regards
JM

 

If it helps, here is my stripped version:
---------------------------------------------
Dim swApp As Object
Dim Part As Object
Dim title As String
Dim compNames(0) As String
Dim compXforms(15) As Double
Dim vcompNames As Variant
Dim vcompXforms As Variant
Dim vcomponents As Variant

Sub main()

compNames(0) = "D:\temp\block.SLDPRT"
' The first 9 elements are the 3x3 rotational sub-matrix
' Set these to the identity rotation.
compXforms(0) = 1
compXforms(1) = 0
compXforms(2) = 0
compXforms(3) = 0
compXforms(4) = 1
compXforms(5) = 0
compXforms(6) = 0
compXforms(7) = 0
compXforms(8) = 1
' The next 3 elements are the translation vector
' Set these to the zero translation
compXforms(9) = 0
compXforms(10) = 0
compXforms(11) = 0
' The next element is the scaling factor.
' Set this to one.
compXforms(12) = 1
' The next 3 elements are unused.
' Set these to zero to be on the safe side.
compXforms(13) = 0
compXforms(14) = 0
compXforms(15) = 0
vcompNames = compNames
vcompXforms = compXforms

Set swApp = Application.SldWorks

Set Part = swApp.NewDocument("D:\Program Files\SolidWorks
2001Plus\data\templates\Assembly.asmdot", 0, 0#, 0#)
title = Part.GetTitle
Set Part = swApp.ActivateDoc(title)

vcomponents = Part.AddComponents((vcompNames), (vcompXforms))

End Sub
----------------------------------------

Paul Delhanty
Cadcambridge Ltd
SolidWorks Research Partner
http://www.cadcambridge.net

 

you are asking for somthing that you can not do.

 

If it helps, here is my stripped version:

Hi Paul,
This works perfectly, thanks very much !!

JM

 

Actually, you can accomplish what you want to do. Open the document
using the OpenDoc6 method. Then after opening, use the ModelDoc
object that was returned by the opendoc method and set the "Visible"
property to false. Then you can activate the assembly document again
and then insert the component. So something like this may work:

Dim AssyDoc as ModelDoc2
Dim PartDoc as ModelDoc2
Dim swApp as sldworks.sldworks
Dim NewComp as component2

Set swapp = CreateObject("SolidWorks.Application")

'Get the current doc which should be the assy
Set AssyDoc = swapp.ActiveDoc

'Open the part document to insert into the assy. This should return a
pointer
'to the new part
Set PartDoc = swApp.OpenDoc6(<insert your parameters here>)

'Hide the part doc
PartDoc.visible = False

'Make the assy the active document
swapp.ActivateDoc2 AssyDoc.GetTitle, ....

'Insert the part into the assy
Set NewComp = Assydoc.AddComponent4(<insert your parameters here>)

'close the part document
PartDoc.close

I hope this helps ....

Steve

 

Hi Steve, thanks, but this way the part document still pops up before u turn
off its visibility.
however I did find a way:

"void SldWorks.DocumentVisible ( visible, type)"
"This method is a flag that allows you to display or hide documents as they
are loaded."

Setting this flag to false (for part documents) before using the opendoc6
(don't forget closing the part & setting the flag back to true afterwards
ofcourse)

best regards,
JM