How do you drive a Creo Parametric Part (.prt) parameters/attributes from file using a text file? Pro Program? Something else?

I've only ever done this using trail files or mapkeys to modify existing part. I usually use VBA/Excel to generate the files. Pro/Program doesn't do this though some sort of Excel analysis might.

What is the workflow you expect to use if you had an ideal situation?

Hi,

yes, you can use Pro/PROGRAM.

Pro/PROGRAM example:

VERSION 2.0

REVNUM 86

LISTING FOR PART PRT0001

INPUT

VYSKA NUMBER

END INPUT

RELATIONS

D3=VYSKA

END RELATIONS

... and so on ...

When you regenerate a part, you use Read File command and enter file name (unfortunatelly you cannot browse folders...).

Example of myfile.txt contents

VYSKA=123

MH

We use Automation Gateway as well to handle parameters in models. It is easy to use, but it is not for free.

Hi  Lawrence Scheeler,

I think I can help you on this because that's the thing I am currently doing for my company.

Use Excel VBA and Mapkey in Creo, see example below:

Sub writeParameters()

Dim filePath, filePath1 As String, textData As String, fileNo As Integer

Dim FromPath, ToPath As String

Dim dataP01, dataP02, dataP03, dataP04, dsgDate, Ldate As String

Dim FSO As Object

Dim wbCnfgr As Workbook

      filePath = "full path and name of the text file which you write parameters to"   (Eg, "C:\AutoDesign\AutoDsg_D\A999-2740\03 CADFiles\15-X\xxx.txt")

     dataP01 = Range("A1")+ "=" +Range("B1")      '(A1=parameter name ,   B1= parameter value on your worksheet)

     dataP02 = Range("A2")+ "=" +Range("B2")

     dataP03 = Range("A3")+ "=" +Range("B3")

     dataP04 = Range("A4")+ "=" +Range("B4")

  Ldate = Date

  dsgDate = "/*Designed by ...on " + Ldate

fileNo = FreeFile 'Get first free file number

Open filePath For Append As #fileNo

Print #fileNo, dsgDate

Print #fileNo, dataP01

Print #fileNo, dataP02

Print #fileNo, dataP03

Print #fileNo, dataP04

Close #fileNo

'End If

End Sub

And in Creo you just create a makey to import the text file to your relation.

Two thoughts.  First, we have done something similar in the past to what KC Ai‌ is suggesting.  We created a bunch of feature parameters inside a stable (but never looked) in feature (one of the datum planes at the top of the model tree.)  We then created a mapkey to automatically browse to a folder and wait for us to pick a file, and then copy the contents of the file into this feature as feature relations.  Relations were added to the other features in the model so they referenced these feature parameters.  It was easy enough to build an Excel file that could directly generate the exact relations statements needed (we would copy them to a text file before importing.)

A second idea might be to use Nitro-CELL.  There is a free version available.  Definitely worth taking a look at.

Here's the method we have been using for the past 10 years:

Microsoft Excel drives our 3D models. Basicly its a combination of the solutions by Martin Hanak (CREO side) and Changxing Lin (EXCEL side)

EXCEL

1) Create an Excel spreadsheet to calculate the values of the parameters which drive your part/assembly. Make the Excel spreadsheet as fancy as you like.

2) Use one sheet of that Excel spreadsheet to hold all the parameters (name of parameter in column A, value in column B)

3) Create an (ActiveX) button and write a small Excel VBA macro which will export all the parameters and their values to a text-file.

We use the exact same text-file over and over again, overwriting the contents when we generate something new. For example: "c:\temp\my_creo_parameters.txt"

CREO

1) Use INPUT parameters

Each PART and ASSEMBLY are driven by INPUT parameters. You can use STRING, YES_NO and NUMBER.

2) Use EXECUTE statements

Use the EXECUTE statement in your assembly to drive the INPUT parameters of any PART and/or sub ASSEMBLY

3) Use Mapkeys

As soon as a part or assembly contains INPUT parameters, you will get the option to use "Read file" when regenerating that part/assembly. Create a mapkey that will do "Edit" --> "Regenerate"--> "Read File" --> "c:\temp\my_creo_parameters.txt". You can also assign a mapkey to a button.

FINAL WORKFLOW

1) Open the Excel spreadsheet, configure your design, hit the button in Excel to generate the "my_creo_parameters.txt"

2) Open your design (part/assemby) in CREO, hit the button which executes the mapkey to read the values from "my_creo_parameters.txt"

P.s. If you are wondering how many parameters you can use...our biggest model uses 1264 input parameters at top-level.

HTH

Although not as detailed an answer as some of the previous ones, please take a look into External Analysis.  I have used it in the past to successfully read in customers' pre-existing algorithms/calculation results.  I usually modify the program to produce repeatable output (csv works well), then read the results into a part/assembly, pulling out whatever its needed. The results are fairly easily accessed from the analysis feature.  Depending on your needs, the analysis feature can exist anywhere in the model tree where you can hopefully avoid multiple regenerations.