useless macro

Using solidworks 2006. Record a macro (part elongation). undo change
(recorded) or load assembly again (or even another assembly. Try to
invoke macro. no change to part. Seems to me this should work without
much ado. I am in the process of re-installing SW now. In the meantime,
any ideas as to how/why it is not working for me?

 

You have to understand that macro recordings are not one for one
keystroke recordings. Way back in SW95 they were, but no more. In
addition, not all GUI functionality is possible in a macro.

When you say part elongation what are you doing to elongate the part?

 

Recording a macro will capture the commands you issue, but you have to
remember that it's possible that it will only work again if ALL other
variables are kept the same the next time you run the macro. For
example, changing the length on a part should be easy, but may not work
if you change window size, view orientation, part name, etc. when you
run the macro the next time.

Recording macros are a great way to start an API project, and also
helpful if you can't figure out a certain command. I have never ever
simply recorded a macro without editing it heavily after the fact. Of
course this take a bit of API knowledge.

I always keep a "temp.swp" macro which I use to record new stuff to
(overwrites it all the time) so I can use the recorded code later.

 

TOP hit the issue right on the head. Not all commands are reproducible
in VBA. Most of the time, you have to replace the recorded one with a
valid call.

 

Taking a pin and enlongating the shaft by changing it's value. Tried
some examples of macros off the web, but they also did not work. I
don't mind programming (have a lot of VB and other expereince), prehaps
I have had better APIs to work from in past....

 

Dragon,

This might explain some things.

Option Explicit

'
******************************************************************************
' C:\DOCUME~1\KELLNERP\LOCALS~1\Temp\swx132\Macro1.swb - macro recorded
on 04/10/06 by kellnerp
'
' REQUIRES A NEW EMPTY PART BEING OPEN
'
'
******************************************************************************
Dim swApp As Object
Dim Part As Object
Dim boolstatus As Boolean
Dim longstatus As Long, longwarnings As Long
Dim FeatureData As Object
Dim Feature As Object
Dim Component As Object
Dim ANNOTATION As Object 'HAD TO ADD THIS LINE BECAUSE SW FORGOT, SEE
OPTION EXPLICIT

Sub main()

Set swApp = Application.SldWorks

Set Part = swApp.ActiveDoc
boolstatus = Part.Extension.SelectByID("Front", "PLANE", 0, 0, 0,
False, 0, Nothing)
boolstatus = Part.Extension.SelectByID("Front", "PLANE", 0, 0, 0,
False, 0, Nothing)
Part.InsertSketch2 True
Part.ClearSelection2 True
Part.CreateCircle 0, 0, 0, 0.01863896961691, -0.01974623513871, 0
Part.ClearSelection2 True
boolstatus = Part.Extension.SelectByID("Arc1", "SKETCHSEGMENT",
0.01974623513871, 0.01679352708058, 0, False, 0, Nothing)
Set ANNOTATION = Part.AddDimension2(0.0570242, 0.0544406, 0)
Part.ClearSelection2 True
boolstatus = Part.Extension.SelectByID("D1@",
"DIMENSION", 0.05739326287979, 0.05333328929987, 0, False, 0, Nothing)
Part.Parameter("D1@Sketch1").SystemValue = 0.0254
Part.ShowNamedView2 "*Trimetric", 8
Part.ClearSelection2 True
boolstatus = Part.Extension.SelectByID("D1@",
"DIMENSION", 0.05739326287979, 0.05333328929987, 0, False, 0, Nothing)
Part.FeatureManager.FeatureExtrusion True, False, False, 0, 0, 0.0762,
0.00254, False, False, False, False, 0.01745329251994,
0.01745329251994, False, False, False, False, 1, 1, 1
Part.SelectionManager.EnableContourSelection = 0
Part.ViewZoomtofit2
' OK HERE WE GO
' PICK PIN
boolstatus = Part.Extension.SelectByID("", "FACE", 0.007306839262867,
0.01038749729173, 0.04061127328708, False, 0, Nothing)
' ACTIVATE PIN CAUSING DIMS TO APPEAR
Part.ActivateSelectedFeature
boolstatus = Part.Extension.SelectByID("D1@",
"DIMENSION", 0.01309206995176, -0.003006131781169, 0.03323381468602,
False, 0, Nothing)
' CHANGE DIMENSION. OOPS, SW DOESN'T SHOW THIS IN THE MACRO, IT JUST
REBUILDS. SHOULD HAVE SHOWN PART.PARAMETER( ) LINE HERE.
Part.EditRebuild
Part.ClearSelection2 True
Part.ViewZoomtofit2
' LETS DO IT FOR REAL AND PUT IN THE CHANGE TO THE EXTRUDE DIM.
Part.Parameter("D1@Extrude1").SystemValue = 0.0254 * 5
Part.EditRebuild
End Sub

 

Heh - so true. The Macro recorder is really a POS, but once you trudge
your way through a few basic macros (RTFM), it's not hard to figure out
what to do to make the macros work.

Best advice would be to find someone with a macro similar to what you
need (that works of course), and use it as a basis for your program.

 

I would say that the macro recorder doesn't come up to customer
expectations. The vast majority of SW users don't know much about VB
and much less about object oriented programming. The API does not
capture many useful and important GUI commands. And, as in this
example, it misses something very simple. For all that it is much
better than, say , SolidEdge which has no macro recorder at all. And it
is helpful for getting started. For the average user something that
captured keystrokes would probably be more helpful, but on the whole
the macro/API has been quite usefull to me even with its steep learning
curve.

 

What exactly are you trying to create, I may already have one that does
it or is a good starting point.

 

I don't know what Dragon is trying to create.