ipc Connection Error

Arun asks..

hi pls help me..am doing 3d modelling and analysis...am started a case 4 days before...now 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
abaqus_no_hardware_acceleration=ON
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.

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 www.abaqusguru.blogspot.com/#askGuru. 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
FOR COMMENTS/CRITICISMS/SUGGESTIONS : Use comments box.

Regards
Abaqus Guru

Buckling

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

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.

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.

About this Blog

Hello,

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.

Regards,
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.