abaqus ElementConnectivity: extract deformed coordinates

[Jam3s]

Hello,
I red a lot of posts on this forum and I found them very useful , but now I have a problem that I can't solve so I hope that somebody can help me.
I would to extract the deformed coordinates of my job on a file that I'll use to create a new geometry without stress and strain; I found a script (odbElementConnectivity.py) already developed in Abaqus but when I run it, the software give me an error: "Error: you must supply the name of an odb on the command line". I opened the script and I tried to change the path in odbPath, but nothing happens.
Has somebody already used this script and can give me any suggestions?
Thanks in advance,

Jam3s

 

[akabarten]

Hello,

The script (odbElementConnectivity.p) you are talking about is this script from Abaqus documentation (9.5.9 An example of reading node and element information from an output database) ?
The script read only initial nodes coordinates so you will not get deform mesh.

If you want to get deform mesh with script you need modified it. You have to read displacement for all nodes from selected step/frame and next add it to initial mesh configuration.

There is also another option. You can import odb file to Abaqus/CAE (File->Import->Model, choose odb type file, next select deform configuration and choose step/frame).

Regards
akaBarten

 

[Jam3s]

Hi akaBarten,
thanks for your reply. The script I'm talking about is the script that you said: evidently I don't understand the description of the script that I've found.
If I can, I ask you other details about this.
First, if I don't change anything, how does it work? And when I run it, why does the software return me that error?
Second, how could I change the script to extract deformed coordinates?
I'll try also the second option that you said me, but I'm searching for something automatic and I suppose that this option is manual.

Regards,
Jam3s

 

[akabarten]

Hello Jam3s,

>>> if I don't change anything, how does it work? And when I run it, why does the software return me that error?

I run the script without any changes and it work fine.
Put the script and odb file in the same directory next open command line, go to that directory and use command:
abaqus python odbElementConnectivity.py name_of_odbfile.odb

>>>I suppose that this option is manual

Almost all processes which you are doing in Abaqus/CAE you can do with python methods. The true is that after you confirm any command in CAE the software run python command in background to perform a task. All python syntax used during your interaction with model in CAE you will find in the file "abaqus.rpy". Just open it in any text editor. The file is save in current directory. When you import deformed mesh from odb CAE run python command "PartFromOdb". So you are able to make a python script to automatic importing deformed mesh. The script with PartFromOdb command has one disadvantage, to run it you need run also abaqus/CAE (but it could be also be run without GUI).

>>> how could I change the script to extract deformed coordinates?

It is possible but this script will be much more complicated then previous one (with PartFromOdb). But it can be run without CAE. You need just write similar function to PartFromOdb. The function need to:
1. open odb file
2. read and save initial nodes coordinate (example you have in file odbElementConnectivity.py)
3. read and save nodes displacement from selected step/frame (9.5.6 Reading field output data)
4. for each node add his initial configuration and displacement
5. write new nodes definition in appropriate format to ASCII file
6. read elements connectivity and also write them to a file in appropriate format

As you can see the task is not so simple. If it is your first python script you should read all chapter "Abaqus Scripting User's Manual".

Regards
akaBarten

 

[corus]

Surely there's no need for python scripts, just use the *anneal keyword which will remove all the stresses for the next step.

corus

 

[Jam3s]

Thanks for the replies,
I've tried all the methods that you suggest to me and the solution of my problem is the *anneal keyword; this is a simply function that execute what I want, but it's guaranteed that I'll try to write also a phyton: first I must study the chapter "Abaqus Scripting User's Manual".
And, akaBarten, what do you know about Abaqus PDE tool? Is the file that it generates already a phyton script?

Regards,
Jam3s

 

[akabarten]

Hello,

PDE tool dose not generate any python scripts. It is just a simple text editor which can be use to write and run python scripts. It has one useful feature. During a script execution PDE can show which line/loop/module is execute so with this tool is quite simple to debug a script. Unfortunately from my experience PDE is not stable. It crash very often during writing a script.

Regards
akaBarten

 

[Jam3s]

Good, now I understand also Abqaus PDE. You are very helpful and competent and I thank you very much.

I have another problem: I explain my question to you and, if you can't answer, I will start a new topic.
I need to model nitinol; in literature I've found a lot of parameters that describe nitinol and I've extract some of them that I think they are sufficient for my purpose. In Abaqus/CAE, under Materials, I've found the possibility to develop a user-defined material where you can put a list of parameters: I wonder what is the order with which I should put them there.
Reading Abaqus documentation and similar topic, I understand that I should use a VUMAT routine (I'm working in explicit): in this case, how can I put these parameters (they are temperatures, Young's moduli, startind and ending stress for both two condition, austenite and martensite: lastly, I need something simple) in a VUMAT routine?

Regards,
Jam3s

 

[akabarten]

Hello,

I am afraid I can not help you with VMAT subroutine. I have never use subroutines. But I am sure that you can find help from others eng-tips users.

Regards
akaBarten