API - BOM Tables and Formatting

Hi,

I need some help.

My SW API skills are just short of being dangerous to anyone standing
in a 20 ft. radius. I believe this will be an easy question to answer


I have a 3rd party application that generates a script to create and
populate the revision block.

The problem:

1. This program generates a table with really thick lines. There is no
specific code that sets the table line thicknesses.
2. I looked at the SW api help and see that there is a command
TableAnnotation::GridLineWeight which I can set. SW does not provide a
sample call that demonstrates how a) I should activate this table and
b) how to modify the actual thickness (i.e. do I use normal, thick,
thick2) or numbers?

Request:

Can someone supply me with several lines of code (example) that shows
me how to actually call and set the table properties.

Or point me to a reference site where applicable examples exist?

Given enought time I think I could figure it out - however, larger
fires (deadlines) are getting in my way of obtaining "quality" time.


Len

Thank you in advance

 

To get hold of TableAnnotation objects call BomFeature.GetTableAnnotations,
which returns an array of TableAnnotation.

TableAnnotation::GridLineWeight takes a long, that is a whole number.
Experimentation suggests that valid numbers seem to be 0 to 7 inclusive.
You could start with this macro that I hacked out from the "Export BOMs to
XML Example (VB)" in the SolidWorks API help.

=============================
Option Explicit

Sub ProcessBomFeature( _
swBomFeat As SldWorks.BomFeature, _
lineWeight As Long)

Dim swFeat As SldWorks.Feature
Dim vTableArr As Variant
Dim vTable As Variant
Dim swTable As SldWorks.TableAnnotation
Set swFeat = swBomFeat.GetFeature

vTableArr = swBomFeat.GetTableAnnotations

For Each vTable In vTableArr

Set swTable = vTable

swTable.GridLineWeight = lineWeight
Next vTable

End Sub

Sub main()

Dim swApp As SldWorks.SldWorks
Dim swModel As SldWorks.ModelDoc2
Dim swDraw As SldWorks.DrawingDoc
Dim swSheet As SldWorks.Sheet
Dim swFeat As SldWorks.Feature
Dim swBomFeat As SldWorks.BomFeature
Dim nNumSheet As Long
Dim nRetval As Long
Dim i As Long
Dim bRet As Boolean

Set swApp = Application.SldWorks
Set swModel = swApp.ActiveDoc
Set swDraw = swModel

Set swFeat = swModel.FirstFeature

Do While Not swFeat Is Nothing

If "BomFeat" = swFeat.GetTypeName Then

Set swBomFeat = swFeat.GetSpecificFeature2
' lineWeight values
ProcessBomFeature swBomFeat, 1

End If
Set swFeat = swFeat.GetNextFeature
Loop
End Sub

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

 

Paul,

Thank you for the help.

Len