Help with autochanging a number in a custom property (Macro)

Dim serialcount as long dim strSerial as string Dim FileName as string

serialcount = 1

for serialcount = 1 to 10 strserial = format (serialcount, "000000") filename = "Serial" & strserial & ".sldprt" msgbox filename next

Do you want to continue creating coppies of Serial.sldprt

I need to make 100 parts, serial # 000001 to #000100

I have a note on a model, that will be etched onto the plate (laser cut). I need this note to change on every part, then save that part as serial000001, serial000002, etc etc

Yes, i need to autogenerate 100 parts. There is a note on each part for the serial #. Im trying to make a macro that will open a default part (serial.sldprt), then change the note (note linked to a custom propoerty that is changed) then saves the part as "serial000001.sldprt". This macro would add 1 to the serial# and do the same for 000002,3,4,5,etc etc.

Any help would be appreciated. Thanks :)

CS wrote:

message

"Serial"

Serial000002.sldprt,

Dim swApp As Object Dim Part As Object Dim boolstatus As Boolean Dim longstatus As Long Dim Annotation As Object Dim Gtol As Object Dim DatumTag As Object Dim FeatureData As Object Dim Feature As Object Dim Component As Object

Sub main() Dim Errors As Long Dim Warnings As Long Dim serialcount as long Dim strSerial as string Dim FileName as string

serialcount = 1

for serialcount = 1 to 10

next

Set swApp = Application.SldWorks

Set Part = swApp.OpenDoc4("serial.SLDPRT", 1, 0, "", longstatus) Set Part = swApp.ActivateDoc("serial.SLDPRT")

for serialcount = 1 to 100 strserial = format (serialcount, "000000") filename = "Serial" & strserial & ".sldprt" retval = Part.DeleteCustomInfo2("", "Serial") retval = Part.AddCustomInfo3(EmptyStr, "Serial", 30, strSerial) Part.EditRebuild SaveOpts = swSaveAsOptions_Copy retval = Part.SaveAs4(filename , 0, SaveOpts, Errors, Warnings) next

swApp.CloseDoc "serial.SLDPRT" End Sub

This is written for 2004 and up mostly because of CONST's

Regards, Corey

Thanks Corey, that works great. I have a problem though, I cant seem to link text in a sketch to a custom property. This seems like a no brainer. I tried linking it like you would a note, but it doesnt have the option. I am using 2003 still, is that a new feature in 2004 or 2005?

I believe it is in 2005 I don't think it is available in 2004 I am still on 2004

Corey

I'm assuming your trying to add linked text to the either the calloutabove, calloutbelow, suffix, or prefix of a DIMENSION. This is not an option in SW2005 either. You can place a note in your part or assembly file but it is not linked to the sketch. It doesn't hide and show when you open and close a sketch. The visibility is controlled by your annotions options in the feature manager tree. I believe you could do this in SW2003 also.

Roland