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ENGINEERINGXYZ8-Gravel
8-Gravel
September 22, 2023
Question

How to Create Custom Parameters for Auto-naming in Creo Parametric?

  • September 22, 2023
  • 3 replies
  • 1767 views

Hello everyone,

I'm currently working on implementing an auto-naming system for parts and assemblies in Creo Parametric. My goal is to have the name generated based on a combination of a unique identifier and the type of part (Mechanical, Electrical, etc.). The idea is to have a function like this:

 

 

new_name = "PART_" + TYPE_SELECTION + "_" + UNIQUE_ID

 

 

For the TYPE_SELECTION, I want to create a dropdown list of options, and for UNIQUE_ID, I'm looking for a way to make it increment by 1 automatically each time a new part is created.

I was able to add basic parameters via Tools > Parameters, but I'm not quite sure how to make TYPE_SELECTION a list of predefined options or how to auto-increment UNIQUE_ID.

Does anyone have experience setting up something similar? Any guidance or tips would be greatly appreciated!

 

3 replies

M
MartinHanak24-Ruby III
24-Ruby III
September 22, 2023

Hi,

from my point of view auto-naming system for parts and assemblies is system which assign names to files. If you want to implement this functionality, you have to develop Toolkit application which calls generator and them creates part or assembly.

    P
    Pettersson15-Moonstone
    15-Moonstone
    September 26, 2023

    https://support.ptc.com/help/creo/creo_pma/r9.0/usascii/index.html#page/fundamentals/fundamentals/about_Restricted_Value_Parameters.html

     

    EDIT: That's just for parameters, though. To implement that as a naming scheme in Windchill, I think it's doable, but I've never done that myself. See this link:

     

    https://support.ptc.com/help/windchill/r12.1.2.0/en/index.html#page/Windchill_Help_Center/ProEWCInteg/ProEWCIntegCustObjNameNumberManageCustName.html#

    H
    Hidetaka1-Visitor
    1-Visitor
    September 27, 2023

    I have done it, but not actually use it.

    To make a drop down list of options, there are two methods.
    1. Using .lst file 

    Example:


    ND_ParamDefArr_K01 = {
    { Name = Maker
    Type = string
    Default = 'ミスミ'
    Enum = { 'ミスミ', 'SMC', 'キーエンス', 'CKD', 'IAI', 'オリエンタル', 'オムロン', 'コガネイ', 'THK', 'CSS', 'SUS', 'ユーザ入力'}
    }
    }


    2. Using user interface

    Hidetaka_0-1695791267250.png

    Hidetaka_1-1695791376960.png




    Automatic numbering can be achieved with Creo API, or automation script (eg. python).
    You should use what you are familiar with.

    In my case, I used Autohotkey.

     

    placeComponent(argument2)
    { ; this function take argument from command line to place a stock part to an assembly. User need to rename the part later. The method used here guarantee that even if the user forgots to rename, there will be no pairs of same name part.
    source := "O:\Free\FA_data\治具_creo\STD_\Sunpou**bleep**ei\" . argument2 . ".prt.1"
     
    FileReadLine, partNumber, D:\partNumber.txt, 1 
    newPartName := A_ComputerName . "_" . partNumber . ".prt.1" 
    wdir := getWorkingDirectory_v1()
    destination := wdir . newPartName
     
    FileCopy, %source%, %destination%, 1
    If ErrorLevel
    {
    Msgbox,64,, Error copying %source%, 1
    return
    }
    sendInput aa ; mapkey to assemble
    setClipBoard(newPartName)
    If (language = "japanese")
    title := "開く"
    else ; If (language = "english")
    title := "Open"
     
     
    Winwait, %title%,, 5 ; wait for the open window to appear
    WinActivate
    SendInput ^v ; paste part name to the search field
    SendInput {Enter}
     
    ; increase partNumber so that the next stock part will have a different name
    partNumber += 1
    file := FileOpen("D:\partNumber.txt", "w")
    file.write(partNumber)
    file.close()
     
    WinWaitNotActive, %title%,, 2
    containingFolder := getContainingFolder()
    if (wdir != containingFolder)
    {
    Msgbox,64, アセンブリは作業フォルダにありません, %newPartName%は作業フォルダ%wdir%に保存されていますが`n親アセンブリは%containingFolder%にあります。,20
    }
     
    return
    }




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