weldments in 2004

has anyone tried this. you can generate a model very fast. There seems to be
some stablity issues though.
but from what i see here, it is painful to add custom property info and
creating cutlist seems to be worse the time saved in creating it is eatin up
creating cutlist and adding properties

maybe i am missing something but help me out if you have experienced
aynthing
similar

RH

 

okay i am still playing with this, here is my situation
i have a large fuselage frame, plane

115 items
60 itmes are tubes or all the same profile ø5/8 x .035 but the length is
different

once a cutlist is created, i need to add specific cutlist properties. but it
seems this needs to be done a per cutlist , so one item at a time.

has one seen anyhting like this so it can be done any other way.

the properties like material, size and description etc should be , maybe at
the profile stage , not at the cutlist so no i have 60 profiles all the same
but the length differs but seems i have to add all the propeties one at a
time per cutlist so 60 times


any help on this matter will be appreciated

ryan

 

Well I have since found out something

You can add properties to sketch profiles. So you can add material,
description, size etc.

But my problem is I have to redo all my profiles since it will not pick up
the new properties in that profile so setup your properties first not
afterwards I guess it doesn't look back to it to see if there are changes,
dam.



115 members to redefine

 

Ryan,

When you created the library feature of the tube (just the sketch of the OD
& ID) you can add the custom properties under the 'custom' tab for the
library feature (they must be the same properties as those used by your
weldment cut list template). Then when you create the 'cut list item' in
the weldment you will find that these properties have been added - weldments
will then automatically add the length (custom property is Length).

The above will only work if you are selecting the library feature from the
weldment selection list and you select a line for it to extrude the library
feature along - it does not work for a library feature created the previous
way (i.e. a feature on a base feature).

If you have a library part with multiple configurations that you want to
convert into weldment library features you can try the macro below (it was
created by Shane Parker at Intercad - my VAR). Please note that it needs a
tweak as it is still leaving the configuration information which makes for
large file sizes. Just remember to put your custom property information in
the custom tab and not the configuration tab and it will populate your cut
list.

Merry

'
****************************************************************************
**
' C:\DOCUME~1\Shane\LOCALS~1\Temp\swx568\Macro1.swb - macro recorded on
08/27/03 by Shane
'
****************************************************************************
**
Sub main()

Dim swApp As SldWorks.SldWorks
Dim Part As SldWorks.ModelDoc2
Dim longstatus As Long
Dim longwarnings As Long
Dim boolstatus As Boolean

Dim FullPath As String
Dim PathOnly As String
Dim vPath As Variant
Dim TemplateName As String
Dim vTemplateName As Variant
Dim NameOnly As String
Dim ConfigName As String
Dim ConfigList As Variant
Dim ThisConfig As Variant
Dim Skname As String

Set swApp = Application.SldWorks

UserForm1.CommonDialog1.Filter = "*.prtdot|*.prtdot"
UserForm1.CommonDialog1.ShowOpen
FullPath = UserForm1.CommonDialog1.FileName
vPath = Split(FullPath, "\")
TemplateName = vPath(UBound(vPath))
PathOnly = Left(FullPath, Len(FullPath) - Len(TemplateName))
vTemplateName = Split(TemplateName, ".")
NameOnly = vTemplateName(0)

Set Part = swApp.OpenDoc6(FullPath, 1, 0, "", longstatus, longwarnings)
Part.SaveAs2 PathOnly + NameOnly + ".sldprt", 0, False,
Falseyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyyy
Skname = InputBox("Sketch Name: ", "Name of sketch to use in lib
feature", "Sketch1")
ConfigList = Part.GetConfigurationNames

For Each ThisConfig In ConfigList
ConfigName = ThisConfig

Part.ShowConfiguration2 ConfigName

boolstatus = Part.Extension.SelectByID(Skname, "SKETCH", 0, 0, 0,
False, 0, Nothing)

Part.SaveAs2 PathOnly + ConfigName + ".SLDLFP", 0, True, False

Set Part = swApp.OpenDoc6(FullPath, 1, 0, "", longstatus,
longwarnings)
Next ThisConfig

End Sub