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


Reply to
Ryan Hay- SDSI
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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


Reply to
Ryan Hay- SDSI

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
Reply to
Ryan Hay- SDSI


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

Reply to
Merry Owen

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