Learning Forum

[mashetty]

I have a exported temperature values of transient thermal analysis of a meshed geometry in excel format.  The head of the data looks as follows:

Node Number    X Location (mm)    Y Location (mm)    Z Location (mm)     Temperature
1    4    1    4    68.33297644
2    3    1    4    59.2816483
3    2    1    4    63.87420006
4    1    1    4    97.20906453

Now I have added an extra column of hardness values for the material from experiments.Now,the excel file contains columns as follows:

Node Number    X Location (mm)    Y Location (mm)    Z Location (mm)     Temperature  Hardness
1    4    1    4    68.33297644    0.122
2    3    1    4    59.2816483      0.866
3    2    1    4    63.87420006    0.455
4    1    1    4    97.20906453    0.655

Hardness (This is an example value, I want to use different values)
I want to import these hardness values into ANSYS(in text form) Mechanical and use them to represent intensity, similar to how stress contours work.

Is it possible to use APDL commands to achieve this?

[mjmiddle]

Native methods:

Are you trying to use these hardness values as an input to analysis? Or are you just trying to make a contour display of them? If you just want a contour display, you can import the data with "External Data." You can select the quantity type as anything, such as temperature, just to get a contour display. The contour will read a wrong title, thinking they are temperature values, but you can gnore that. And you won't want to solve with this load. An APDL command could use *vread and *vput to replace the data into an uninteresting result quantity, then you can use a User Defined Result in Mechanical to specify that result quantity from the result file. The title will still read as a different result quantity than you know it is.

Or you can just replace the temperature data column with the hardness data in your CSV file. In a User Defined Result, you can set the "Source" to "Import File."

Of course, this will also read a wrong title, but you'll ge the contours you want. This method will only accept a file that contains the exact titles and columns and format (tab delimited) you would get when you export a result to a text file. But you can replace the data in the temperature column.

Any native method you choose is going to be non-ideal, because you'll have to accept the wrong title above the result legend. 

Another option may be to use some other contour plotting software with scripting to read in a grid and plot values such as python matplotlib.

Or if you want to script the behavior entirely, and have the correct result title, you can do that with a "python result" or a result created in an ACT extension.

In Ansys help, go to "Mechanical Application > Mechanical Users' Guide > Using Results > Python Result."
https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v241/en/wb_sim/ds_python_result.html

To get started with ACT extensions, there is an Introduction to ACT in Mechanical in the Ansys Learning Hub:

https://www.ansys.com/services/ansys-learning-hub

[mashetty]

Thanks for your response. I am not trying to use hardness values as an input but would like to show the contours on the geometry that describe the intensity plot on the 3D geometry. I have tried the method mentioned above in your discussion. I created a user-defined result and imported a file using the source in the definition; however, I am getting an error as follows:

 

 

I then tried using the file exported from ANSYS without any changes in the temperature column, but it still does not work.

[mjmiddle]

Are you opening the file in Excel and doing any work to it? You can open in NotePad to and try changing some values since NotePad does writes out pretty much the same format as it read, which means same encoding (UTF-8) and same end-of-line characters. If you open in Excel and edit, you should be able to write as a tab delimited text file.

It must be tab delimited. Pretty much, it must be the exact format you would get when you right click on a result to "Export > Export Text File."

Also, it will be required to have "File > Options > Mechanical > Export", "Include Node Numbers" = Yes and "Include Node Locations" = No.

It will require 1 title row and it looks for the key text "Node Number." You can change the title of the exported quantity to anything (but not "Node Number"), and it must be tab delimited:

 

Node Number    hello

1    8.0404e-004

2    1.1004e-003

3    1.1004e-003

 

"Mechanical Application > Mechanical User's Guide > Results > User Defined Results > Application > Limitations for Imported Files"

https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v242/en/wb_sim/ds_user_defined_app.html

 

 

[mashetty]

Thanks a lot for your response.