1.Initially you have to create a node set (example: "output nodes") 

2.Now, create a display group(DG)

Tools -> Display group -> Nodes -> Node Set -> output nodes and save the DG.

3. To extract the data click on Tools -> query -> Probe values-> Field output (spatial displacement U1/U2/U3) -> ok. Click on Display group and select the group that you have created in the previous step.

4. Click on 'Write to File'. Now the displacement values for the required nodes will be extracted as a report file (.rpt).

Hope this helps.

Thanks, Mr. Narayanan.

But, this method is not very useful here. For my case, the number of frames is 40 and I need all dof displacements (U1, U2, U3, UR1, UR2, UR3) for all the node at all the frames. I think by the method you mentioned, I need to make report 40*6 times!

There are some other conventional methods that you can get all dof displacements of all the nodes at a specific frame:

create XY data> ODB field output> unique nodal> U1, U2, U3, UR1, UR2, UR3> Node set (target nodes)> save.

[Here, you get all dofs for all the frames you like. But for my case it is impossible, as the data are too many.]

And then: report> XY data, .rpt will be created.

Hello,

Try to get the divide the nodes into 2 or 3 set of nodal sets and get the displacement data for all nodes in for sets using create XY data> ODB field output> unique nodal> all> nodal set. 

I usually do it this way. Hope this helps. 

Thank you for the idea Mr Maroju and the trick seems effective.  Then, I divided the original set to some subsets. However, still the PC cannot handle reading the data even for one subset separately, although it is already more than 5 times easier to it!

Do you know any other way or trick?

How many nodes do you have in a node set? Do you need all the displacements from U1 to UR3? If not necessary you can also reduce the field outputs. 

You can also assign physical memory to the job before you run the simulation. 

You can extract the .odb file and check it in a workstation with high performance. That might help you. 

Thanks again for going to the point.

There are about 6300 nodes in each subset. As the field outputs, I need all the displacements from U1 to UR3 for all the frames.

I would like to try allocating physical memory to this job first. Would you please guide me with it?

If this doesn’t work, I go for running the job on a super computer.

Once you create the job file that is write input file. Go to the abaqus job directory.

Then shift+right click > open command prompt here. Use folloeing command

Abaqus job= input file cpus=(max no cpus u have) memory = (max that u can ) interactive. 

The job runs in non gui module but is faster than gui.

Going back to the initial question, the issue is about post processing of the numerical analysis, not the analysis itself (running the job). I mean in running the job in gui module gives results and no problem with it. However, when I want to get displacement data, it takes too long by gui (as described earlier).

How to resolve this issue? Can I get the data that I want (after finishing the job) by assigning physical memory to the job?

How do I extract stress at surface sets not node sets using abaqus python script?

If it is allowed, one can reduce the number of increments from 40 to lets say, 10. This can reduce the data number to again one fourth.

Also when you request XY data from ODB field output, it is possible to access 'Active Steps/Frames' and select only the interesting frames to generate the data and save them; consequently reducing the data points.

Cheers!

Shafiq

Mr. Mohammadmahdi Davoudi

I am getting the same problem, in extracting nodal output data, like you, How did you solve it? Please share me your exprience.

Thanks in advance for your time.

Try to display only the elements/nodes you want to export and then use the Report - Field output option. This should only write the information of the displayed elements/nodes to a report file.

click on xy data, choose unique nodal and select the parameter you want to get the results for (displacement, reaction; etc.), click on elements/nodes, click on add selection, pick the node you want from the viewport and press plot, after you can export these data to excel.

Dear Mohammadmahdi & Abdurehman,

it's actually quite simple, however you need to do a programming work in matlab or other tool of your preference. You can look in the Abaqus manual for the keyword *Node print if you need to know more details. The steps that I used to do is like this:

1. create a set that contains your nodes or elements that you want to include. Let's call it MD.

2. if you are working from the CAE then create the job and write the .inp file.

3. edit manually your .inp file using notepad. Just before the end of the step ("*End Step" in your .inp file), add the command below:

*Node print, nset=MD

U1

you can change U1 to other dof. You can repeat the command as many as you like for other dof or other set.

4. Assuming the .inp file location is not changed, you can save it on your notepad then click submit from CAE job module. Or you can run it from Abaqus command. The results will be printed in the .dat file of your job.

5. Now you just need to create a script in matlab with textscan, for loops, strcmpi etc. to read all the output. Just remember that the .dat text file contains strings so you might need to have some workaround in your matlab code to search for the outputs and to separate the numbers from the whitespace.

Assuming that you are working with such big data, you would or should be using matlab anyway (instead, say, office) and thus, you can combine the script with your plotting or post processing script.

I hope this helps.

Mit freundlichen Grüßen,

Ashwin Narayanan Hi Mr. Ashwin Narayanan, thanks for sharing! It is useful to extract field output data (e.g. U3) from a display group in Abaqus. May I ask, do you know how to use python script to extract the same data (U3 and node coordinate)? As I have many frames and I need all the displacement data at all frames. Thanks in advance.

Mohammadmahdi Davoudi Dear Mohammadmahdi Davoudi,

Have you solved the problem now? I have a similar problem in my case. I need to extract U3 displacement and node coordinate for all the nodes at target sets (e.g. at the surface of the model) at all the frames. Do you maybe have a suggestion?

Sincerely,

Nan

Hi Nan,

If you want to use Python script to extract bulk or repetitive field output data from Abaqus. I suggest you use Macro manager on Abaqus to record the extraction process in the .py file and later modify it to your purpose. While using the Macro manager record, you can do the U3 displacement and node coordinate extraction using XY report for one node. Later, you can browse and open the Macro file in Python and edit the number of nodes to the desired value on the code. Finally, when you run the python script from 'run script' on Abacus CAE or command prompt, you should get the report file for all required nodes.

I hope this will solve your problem.

I do have a problem with giving CSV data as input. My problem is a complex loading condition in which the model is shrinking with respect to time and other parameters (continuum simulation of component sintering). Can anyone please give me suggestions for solving this problem?

Thanks in advance