User login

You are here

Error

Hi friends
I have two errors in my simulating ,with this massage:

2 nodes are missing degree of freedoms. The MPC/Equation/kinematic coupling constraints can not be formed. The nodes have been identified in node set ErrNodeMissingDofConstrDef.

Analysis Input File Processor exited with an error.

I checked all constraints in those two nodes, and I am sure that I created these constraints like others, but I cannot understand what is the problem?
Also there is a warning:

Boundary conditions are specified on inactive dof of 2 nodes. The nodes have been identified in node set WarnNodeBCInactiveDof.

How I could solve these problems?
Could someone guide me?
I upload my CAE and JNL files in the following address:
http://www.4shared.com/rar/xiz-nVkl/mymodeling.html

Thanks

If there are several constraints, and some of those constrained nodes are involved in multiple constraints and/or boundary conditions, then you should look carefully into how constraints are being defined. Abaqus removes some of the constrained dofs, and therefore anything coming after that (e.g. constraints, load, bc) will not be felt. This is what I think is happening in your model. Check manual for what dofs will be removed in a constraint definition, and then organize your constraints/bc accordingly such that no eliminated dofs are involved in later definition.

------

The world started with 0, is progressing with 0, but doesn't want 0.

Hi Akumar !

Thanks for your guide

Now I have another question

How I could check manual for what dofs will be removed in a constraint in a constraint definition?

and then how I could organize my constraints accordingly such that no eliminated dofs are involved in later defination?

brunda's picture

For example, your constraint equation says that

X displacement of node 1 - X displacement of node 2 =0

then you are removing the X displacement of node 1 and you cannot use another equation of the  form X displacement of Node 1 - X displacement of Node 3 = 0.

Instead X displacement of Node 3 - X displacement of Node 1 can be used. 

 

In your .dat file, the degrees of freedom that have vanished for error nodes will be mentioned.

Well, there is no method that I know of other than what Brunda has just mentioned.You have to do it manually. Almost always, in any constraints (MPC, EQUATION, COUPLING, KINEMATIC COUPLING, RIGID BODY, etc.), the dofs of slave nodes that are involved in the constraint definition will be eliminated. Also, it will be done in the order they are encountered.

 In some cases the elemination (or condensation) will be done before any system matrix assembly. In other case, it is done during the matrix assembly. Therefore, it's all dependent on how these have been defined.

Some guidelines:

  1. If some nodes are participating in two or more constraints, then try to chain them; i.e. if A, B, and C are linked as A is tied to B, and B is rigidly connected to C, then define B->Ref Node=A, Node B, Ref Node=C.
  2. Pay extra attention to which node or node set are you going to define as slave. Usually choose slave node/sets which are not going to participate anywhere either in other MPC or Boundary/Load.
  3. Try to put all constraint definitions at one place in the input file, this makes tracking easier.

If I come across any technique where abaqus can printout which dofs are removed, I will definately share it here.

------

The world started with 0, is progressing with 0, but doesn't want 0.


Is there anybody who know what do these warning and error mean?


Solver problem. Zero pivot when processing
D.O.F. 6 of 1 nodes. The nodes have been identified in node set
WarnNodeSolvProbZeroPiv_6_1_1_1_1.


And when I define a load and submit the job, Analysis exited with
this error:


Too many attempts made for this
incrementAbaqus/Standard Analysis exited with an error - Please see the message
file for possible error messages if the file exists.


How I could solve them ?


Thanks


Zero pivot means there is rigid body motion in your system or in other words the system matrix is singular. Abaqus will try to resolve zero pivot but if it is genuine then abaqus can not, and you'll have to fix it...since there is only 1 dof of 1 node, the task is quite easy. Open odb file, and check which node it is (abaqus has created a node set for this)...and then you can check your input file or model to find out what is causing singular matrix or rigid boyd motion.

------

The world started with 0, is progressing with 0, but doesn't want 0.


Thanks for your quick reply A.Kumar


My model is a simple 3D truss, I modeled many kind of these
structures, but this is the first time which I have this error, one of respective
node is locating along one of elements and the other one is locating in a pin
joint, so there isn’t anything that  causing
singular matrix or rigid body motion


By this description what do you think about this error?


By definition, tursses can not carry moment and shear, and therefore no rotational dof in truss element. Since the singularity came on dof 6, then it is quite obvious that somehow through constraints, rotaional degree of freedom is being activated. And since trusses don't have bending or shear stiffness, your rotation dof stiffness = 0.

Check your model again, it must be some small thing that is causing the problem. Specially check around the node where zero pivot is being reported by abaqus.

By the way, are you using connector element to create a pin joint between two nodes?

------

The world started with 0, is progressing with 0, but doesn't want 0.

Thanks a lot, I solved my problem!

Subscribe to Comments for "Error"

Recent comments

More comments

Syndicate

Subscribe to Syndicate