RIKS - Load Vs. Displacement Curve

Rahul asks..
I want to plot load versus displacement curve from the static riks analysis I have performed for my Buckling problem. Is it possible that abaqus generates such curve or I have to use arc lengths to estimate "load applied" at each increment. please help me out

Answer :
There is no direct way to do this.

You can make a XY data of LPF ( Load Proportinality Factor) from History Output. Then create another XY data for load by mutliplying this LPF with the load magnitude you have defined. This XY Data will now be your Load Data.

Extract XY Data for the displacement you require. Now you have XY data for Load and Displacement.

Goto Create->XY Data-> Operate on XY Data.

Use the combine() function to combine these two data. The resultant will be the load vs. displacement curve.

Reversing Plot Axes, Multiple plots

Vijay asks...
I have plotted a plot true distance along path on x-axis and Stress on y-axis.But I want In reverse i.e. stress on x-axis and distance on y-axis. I have seen options but I could not found out how to interchange axes? could you help me in that?
Another was I want 3 different plots on same graph in abaqus.Is there any procedure to get that one?

Answer :
Well, the solution is not that straighforward.

If you are OK with visulaizing the curves in a spread sheet, then you can write the XY Data to a text file with the option
Report->XY Data.

This will write the data in a text file. You can import the file in MSExcel or any other spreadsheets. There you can plot in any way that you want.

If you specifically want to plot Stress in X axis and Distance in Y Axis, then follow the steps mentioned above. In the spreadsheet, exchange the columns, so that Stress is in first column and Displacement in second column. Retain only this XY Data and delete all other text from the file and save this spreadsheet as CSV ( Comma Seperated Values).

From Abaqus, do the following :
Tools->XYData->Create->ASCII File
Select the CSV File you have created and save it as a XY Data. Plotting that will give you the curve required.


Plotting Multiple curves is very easy in Abaqus. Extract the required XY Data. Then
Tools->XYData->Manager
Select the required Data and Click Plot

NODE SET IS NOT ACTIVE IN THE MODEL

Shyam asks..
I am trying to solve a problem for charpy test where a hammer stricts a specimen supported on two anvils. while running the problem, encountered with errors as follows. plz guide me
*A BOUNDARY CONDITION HAS BEEN SPECIFIED ON NODE SET ASSEMBLY__PICKEDSET21 BUT THIS NODE SET IS NOT ACTIVE IN THE MODEL
*Error in job finpractice: The surface ASSEMBLY_SURF-2 has not been defined.


Answer :
This is a typical modelling error. It can be caused by a variety of reasons. There is too little information for me to ascertain the real cause for the problem. Neverthless, you can do the following to check for errors.

In the .dat file, search for that ASSEMBLY__PICKEDSET21 or ASSEMBLY_SURF-2 to see where it is used. After finding out which BC or load that is used, goto CAE and try to edit that Load or BC. In my guess, when you try to edit, you will get an message saying that, the references no longer exist. Reselect the references again and then you should be able to run the job.

Good Luck

Averaging Regions

issares asks..
I have simulated an explicit simulation. when the simulation has completed i used "fieldoutputs report" to save some results (section thickness (STH)) for all unique node in text file. The problem is the results in this file was "automatically" seperated in some different averaging region.
If anyone got an idea please help me
I want to know how can i save a fieldoutputs report without this many averaging region in the text file.

Answer :
By default, Abaqus Viewer Averages the results inside the ODB Regions. So if you have different section defintions in the model, each region with different section properties is considered as a different ODB Region and will be averaged seperately.

To avoid this, you can change the default Averaging Region to all that is in the model.

In Viewer,

Results->Options->Computation->Averaging->Average Element output at Nodes->Use Region Boundaries->DisplayGroups->Specify->ALL

Transformation of Results to Cylindrical Co-ordinate System

Bharadwaj asks...

Is der any way that i can out put stress values in Cylindrical coordiantes instead of rectangular cartesian coordiantes

Answer :
YES! You can.

1. Create a Cartesian Co-ordinate system in visualisation Mode.
2. Result->Options->Transformation->UserDefined. There you choose the Co-Ordnate System you just now created.

Please note that only the Components of the Stress Tensor ( like S11, S22, etc.) will be transformed to the new co-ordinate system. The Invariants like Von-Mises etc. cannot be changed as they are scalar quantities.