Wednesday, November 12, 2008


There are some queries asking if this blog is officialy related to Abaqus. To make things clear and to avoid confusion, I decided to write this post.

Abaqus is a trademark owned by Abaqus Inc. This blog is in no way affilated to Abaqus, and therefore UNOFFICIAL.

The blog is intended to discuss the various problems faced by users like me and to get different perspectives to the problem. Often one is struck with a single viewpoint and finds it difficult to solve the problem. The blog is intended to get more viewpoints. The original plan was to start a forum, but I started this blog, because it is easier.

As I mentioned in About Blog, this page is not merely for writing about Abaqus Software, but also about Science in General.

If you have any thoughts about the whole blog, do feel free to comment.

Monday, November 10, 2008

Difference in Results Between Various Versions and OSs

Julian Hallai asks...
I have been running jobs in different machines with different OS and different abaqus versions. The same input file gives reasonably different outputs. The machines were:
1) IBM Unix Machine with abaqus 6.3
2) Linux Machine with abaqus 6.7
3) Windows Machine with abaqus 6.7
So I got different results with the same version of abaqus in two different machines (with different OS) and also different results with different versions in Unix/Linux.

This doesn't happen to all input files. It has happened to about 50% of the cases (total 20 jobs).

I should also write that the material's engineering stress-strain curve has one part that's softening.

Any thoughts on that?

Thank you so much

Answer :
From Version 6.3 to 6.7 Abaqus has changed a lot, especially in the contact formulation. Please check if the input files, which exhibit remarkable difference between versions, have some specific contact definitions. These contact definitions often exhibit such differences between the versions. Material model implementation is another area where discrepancies may occur. But it is very difficult to ascertain that without looking into the exact case.

Non-Convergence of the input file between versions is very common and people at Abaqus themselves accept this and suggest to read the documentation before using any keyword. The release notes in documentation for every version are a good source of reference to check what all had been changed in the new version.

Difference in results from one OS to another for the same version is defintely a bug. You should contact abaqus support to notify the bug.

Saturday, November 8, 2008

Assembling parts from Different Models

Basavaraj asks..
i have imported two inp files in abaqus now i want to assemble
how to do assemble two different inp files in abaqus GUI?

Answer :
What do you mean by assembling? Do you want to assemble the parts from the input files together?
In CAE ( Version 6.8), after you have imported the inp files, you will get 2 models. Then goto
Model->Copy Objects...
There you can copy different objects ( in your case, the orphan mesh parts, sections, materials etc..) in a single model. Then you can assemble the parts together.

Beam Elements with Solid Elements

Jason asks....
Can we use beam element and solid element in one model ? And how to deal with the joint section ?

Answer :
Yes, it is possible to use beam elements with solid elements. If modelled so, the nodes at which the beam and solid elements join, will have additional DOFs. ( e.g. 6 DOFs if 3D Beams are used. Please note that normally nodes of solid elements will have only 3 DOFs)

Abaqus Online Tutorials

In addition to the basic tutorials found in at simulia website, I found the following resources helpful for abaqus beginners.

Abaqus Tutorial Slideshow at as video

Abaqus Tutorial Slideshow at as PPT

Abaqus Tutorial at Brown University

Chapter 11 of "A First Course in Finite Elements" by Jacob Fish, Ted Belytschko ( Google books)

The above mentioned book from another website

Another tutorial from iMechanica

Please note that I have collected all this information just by googling. The links are credited to the respective authors. If some links are not working, please try other links or you google yourself.

Thursday, November 6, 2008

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.

Wednesday, November 5, 2008

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
Select the required Data and Click Plot


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
*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

Tuesday, November 4, 2008

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.

Sunday, November 2, 2008

Ask Guru Button is back!

Hello All,
after a small hiccup, the 'Ask Guru' Button is again functional. Please post your questions about Abaqus Software by clicking on that button.

I have answered all the questions till now asked. People who asked questions, please check out the blog for answers and do write your comments.


AskGuru Functionality - Temporarily Out of Order

Hello All,
I was trying to change some settings in the Blog and have done something wrong. Now the 'Ask Guru' Fucntionality is temporarily not availble. I will fix it as soon as possible and will inform you people.

Thanks for your understanding :)

Saturday, November 1, 2008

Combine Restart Odb Files

Anonymous asks..
I am running an analysis splitted into 10 restart analyses (ABAQUS/Standard). Now the problem is I am not creating .fil file for the analysis. Is it possible to combine all the odb files into 1 single ouputfile??? is it possible thru command line or do I need to go to python scripting???

Answer :
Starting from Abaqus 6.6 a execution procedure called restartjoin can be used to join different odb files from restart analysis. The syntax is

abaqus restartjoin

Prior to Abaqus 6.6, this execution procedure was not available. But almost the same functionality can be availed by using example programs odbjoin.c and I use here almost the same functionality because it seems that merging of history output is not the same between the execution procedure and the example programs.

To use C program, follow these steps. ( For python program also the steps are similar, only that you dont need to compile the program and should make use of abaqus python command)

Fetch the program
abq651 fetch job=odbJoin.C

Compile the program
abq651 make job=odbJoin.C

Use the compiled binary
abq651 odbJoin -writeOdb destination.odb -readOdbs restart.odb

The above command will join the restart.odb to Destination.odb

Modelling Fluid Viscosity in Fluid Cavity

Rahul asks...
I am modeling a fluid cavity in abaqus. I need to model fluid viscosity. How can it be done?

Answer :
Fluid Cavity as such does not have Viscosity as a parameter. But if fluid is flowing from one Cavity to another then you need to use *FLUID EXCHANGE. In this keyword you can define the Bulk Viscosity.

The following is the input file implementation of it.


viscous resistance coefficient, hydrodynamic resistance coefficient

Biased Meshing

Vijay asks..
I created a 3-D fixed beam(i.e. fixed at one end and free at other end) in Abaqus CAE.I want to mesh that one. But actually what I want is I want to use finer mesh for half of the beam( i.e. from fixed end) than the other half(i.e. free end)
how can we do that one?

Answer :
You can use Local Biased seed for the edges.
In Mesh Module -> Seed -> Edge Biased.

Abaqus Tutorials and Documentation

One of the questions that I am often asked by someone who is just starting to use Abaqus, is where they can find Online Tutorials, so that they can learn on their own.

The answer simply is google. I mean try googling. There are humpty number of sites, especially educational institutions, which host Abaqus Tutorials.

I just name few sites that I found by googling.

Abaqus Official Webpage itself has an assortment of Tutorials to get oneself started. You can find them at the following link.
Abaqus Academic Tutorials at Simulia Website

Another nice place to start, in my opinion, is the Tutorials section of the Abaqus Documentation. It is very comprehensive and ofcourse official. And for more complicated problems, there are these Example Users Manual and Verificiation Users Manual.

Abaqus Documentation comes along with the Abaqus Software and is copyrighted. But surprisingly, I found the documentaion online in some sites. HLRS Stuttgart was one such site with the documentation for many versions available. Very recently, public access to that site was denied.

With a little more effort and tweaking, I found the documentation on Scientific Computing and Visualisation Institute of Boston University. May be they also will deny access to the Documentation soon. For reasons of copyright problems, I refrain from posting those links.

Good luck and have fun using Abaqus.

Please note that Abaqus Documentation is copyrighted and I have found these links just by googling. I have nothing to do with the posting of these documents online and therefore cannot be held responsible for any misuse of these documents.