Disclaimer

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.

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.

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 gatech.edu as video

Abaqus Tutorial Slideshow at gatech.edu 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.

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	originalodb=odb-file-name
	restartodb=odb-file-name [copyoriginal] [history] [compressresult]

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 odbjoin.py. 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

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.

Disclaimer
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.

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.

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
abq663


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.

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.