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.

Friday, October 31, 2008

ipc Connection Error

Arun asks..

hi pls help doing 3d modelling and started a case 4 days it shows job s running...but i cant monitor that...if i give the monitor,abaqus ifself automatically closing..y i did nt know... GUI detected for error while waiting for the ipc connection to close....abaqus error:abaqus\CAE kernal excited with an error...

Answer :
I have a feeling that this has nothing to do with the solver itself. I guess there would not be any error messages in the .sta file. But if you find error messages there, please let me know.

Did you change any of your system configuration recently. Anything to do with the graphic card? If so probably it has something to do with Hardware Accleration

Try setting
in your abaqus_v6.env file and rerun the simulation.

Sign up for Site updates... Email Subscription

Vijay Kumar said..
Thank you very much for adding RSS feed.I have seen in another blog there "sign up for site updates" facility is available.There I have given my email id.When new article was posted in that blog I will get the information about that.Like that can you add that facility to this blog also.That is very useful for the most........

Response :

The "Sign Up for Site Updates" Feature is now available in this blog. Thanks Vijay again for the sugestion.

Using subroutines without fortran compiler

Abhijit aks..
I am doing a heat transfer analysis using ABAQUS. I am using a subroutine FILM but my computer does not have a FORTRAN compiler. So, I think I can not run this job on my computer.
Can you give me some suggestion: how get away with FORTRAN compiler and still use the subroutine. Otherwise is there any other way where I can get it for free.

Answer :
There are several options that you can try..

1. You can download the Intel Visual Fortran Compiler for trial and run for 30 days. Make the object file using abaqus make. Use the object file in future. Also note that before that you need to have Microsoft Visual Studio pre installed. You can also download a free trial version of it.
Intel Visual Fortran Trial Version Download Page

2. Try installing the free fortran compilers like GNU
GNU Fortran Homepage
I dont know for sure if it would work seamlessly, because it is not supported by Abaqus. But it is worth a try.

3. Compile the Fortran Program in an another abaqus machine with fortran, using abaqus make. And try to use that with your simulation.

Good luck!!

Tie Constraint over many surfaces

Bharath asks...
Im doing a quater model aluminium specimen which has counter sunk hole . SO
i basically divided it into 4 parts like 1 with counter sunk and den the st
shank and 2 more additional peices attached to it. what i hve done is used
tie constraint for all to make node equivalnce ..but der is problem with tie
constraint it gves me warning says nodes on the lave surface have more than
one tie constraint so it is automatically removing one tie constraint ...

is der any other way for me to do this node equivalnce with using tie
constraint or and i cannot use partition because of geometry too ...
and lastly im not getting the mpc constraint in abaqus 6.7.3 which i used
to get in the 6.6.3.

Answer :
Try modelling such that there is one master surface which ties to several other slave surfaces. Or if a slave surface of constraint-1 comes into constraint-2 with another surface, then define the slave surface from constraint-1 as master surface in constraint-2. Basically avoid modelling a slave surface being driven by more than one Master Surface.

MPCs can be accesed in 6.7-3 using the keyword *MPC. This is not supported in CAE.

Choosing Elements

Jason asks..
Would you please instruct us how to choose the type of solid elements in large deformation analysis? For example,linear or quadratic, reduced integration or not ?

Answer :
The choice of the elements, depend on the type of problem and the material. I will try to give brief guidelines.

1. In General, the Quadratic meshes give more accurate results than the Linear meshes. But the quadratic elements should NOT be used for the faces coming in contact. This will produce unrealistic jump in Contact Pressure values. In that case, better to refine the mesh and use linear elements

2. Many non-linear problems use nearly incompressible materials. Usage of Fully Integrated Elements in this case will lead to volumetric locking and therefore excessive stiffness. Usage of Reduced Integration elements ( e.g. C3D8R) will relax it and provide more realistic results. But, one should be careful with the effect of Hour glassing when using Linear Reduced Integration Elements

3. Hour glassing is the phenomena of elements distorting in such a way that there is no change in Strain Energy. It behaves like a rigid body mode. One should be concerned with hour glassing effect only in Linear Reduced Integration elements. In Quadratic Reduced Integration Elements, Hour glassing doesn't propagate and therefore has no big effect. Most of the times, hour glassing can be controlled by using enhanced hour glass stiffness option. When using hour glass stiffness one must keep an eye on the artificial energy created in the system and make sure it is low.

Monday, October 27, 2008

Ask Guru Form and my messup with Comments

Yesterday I thought of streamlining the blog a bit. As the first step, I have created a sort of form, through which the questions could be asked. The form is reachable at Clicking the "Ask Guru" button will lead you to the same page. Please use this form to submit your questions.

While this new functionality was being added, I have messed up a little bit with the comments functionality in the blog and therefore yesterday writing comments was not possible . I havbe figured that out only lately and have now fixed it. I apologise if anyone had tried writing a comment and couldnot then do it. I am quite new to blogging and I am learning all this publishing and HTML stuff only now. So please bear up with me when something is not working. If something is not working or if you have some suggestions, please let me know through comments, or you can also scrap in my orkut account.

One such sugestion was from Vijay Kumar to add RSS feed. Thank you Vijay for the suggestion and you can now find that RSS subscription facility is now added. More suggestions are welcome.

And some final words about the present organisation.
FOR QUESTIONS : Use AskGuru Form

Abaqus Guru

Sunday, October 26, 2008


Rahul asks...
".... how to predict "critical buckling loads" for hollow cylindrical shaft under torsion?"

Answer :
To predict bucking, the *BUCKLE keyword can be used. In this procedure bucking is predicted using Eigenvalues. And therefore eigenvalues are extracted in this procedure.

A General Static Analysis can be used prior to the *BUCKLE procedure to prescribe the preloads . The *BUCKLE Analysis will take the end state of the previous analysis as the base state.

A *STATIC,RIKS analysis can be performed to ramp the load till the point of buckling and also to perform post buckling analysis. This RIKS analysis delivers the Load Proportionality Factor (LPF) as a solution. So it is enough to only give a reference load ( lets say Unit Load ) and the LPF at the time of bucking will then be buckling load.

For further information, please refer to :

Abaqus Analysis Users Manual
Section 6.2.3 Eigenvalue buckling prediction
Section 6.2.4 Unstable collapse and postbuckling analysis

Thursday, October 23, 2008

Extrapolation of results from Integration points to nodes.

In Abaqus the direct solution variables like displacement, temperature etc. are calculated directly at nodes. But the quantities like stress etc are calculated at so called material integration points. These points do not lie on the nodes but rather at an offset inside the element from the nodes.

In Abaqus Viewer you can request such results at integration points or at the nodes. When requested at nodes, the Viewer follows the following steps to extrapolate the results to nodes.

  1. The tensor components are extrapolated from the integration points to the nodes.
  2. For each element surrounding a node, the invariants are independently calculated using the corresponding unaveraged, extrapolated values.
  3. The independent values of the invariant are then averaged to get a single value at the node.
As an example, lets consider the Stress tensor output. The above steps will then become:
  1. S11, S22, S12, etc. are extrapolated from integration point to nodes.
  2. For each element sorrounding the node, the invariants of stres tensor, MISES, TRESC, PRESS, INV3, are calculated seperately.
  3. Then these independent values are averaged based on the threshold value set.

Tuesday, October 21, 2008

Running an Abaqus Job

The Abaqus CAE is a great tool that is improving continously. But most of the time, it hides from the user, what it exactly does and the breed that grow up using only CAE almost doesnot understand that the CAE is just a front end for the various options that can be accesed also by issuing commands.

Although volumes can be written about mimicing the CAE operations using command line or INP file, in this post I will just concenterate on the Job Submission, which is one of the simplest thing to explain. Given the fact that I am brand new to blogging, that is my obvious choice!!

Before we begin, some preliminaries. In this post, I use abaqus as the command to invoke the solver. In general that should invoke the most current version of the solver installed in your machine. If you want to invoke a particular version of the solver, for whatever reasons, then use the approriate command.

e.g. to invoke abaqus release 6.6-3 use the following

To start a job with default parameters :

abaqus job=input-file-name

This will set parameters by reading the abaqus environment file ( e.g. abaqus_v6.env) and then runs the job.

To do a datacheck of the model :

abaqus job=input-file-name datacheck =yes

To start the job with 2 cpus :

abaqus job=input-file-name cpus=2

To start the job with particular standard memory :

abaqus job=input-file-name standard_memory = '4000mb'

Note that starting from abaqus release 6.8-1 the default memory setting is 90% of the physical memory and the standard_memory parameter is no longer valid.

Sunday, October 19, 2008

About this Blog


In this Blog, I plan to share my experience and the understanding of the Abaqus Software. I plan to use the blog as a sort of forum to initiate discussions and thereby to expand the horizons of knowledge about Abaqus software in particular and Science in general.

The postings that I make are by no means the only allowed topics. Please feel free to comment on my posts and suggest new topics or ask questions on this blog.

Lets together expand the horizon of our knowledge.

Abaqus Guru

Difference between Static and Dynamic Analysis

Question : When to use Static and when to use Dynamic Analysis ?

Answer : A problem is dynamic when the inertial forces from Structural accelerations are both :

  • significant and
  • vary rapidly in time
Inertial forces are proportional to structure's mass and acceleration. If the loads acting on the structure vary slowly enough the inertial forces will be small and the response can be considered quasis-static.

Some times we have large inertial loads but can do static analysis because the loads vary slowly with time. e.g. Gravity loading.