Convergence Norm INF,L1 and L2 1

[Dave442]

Hi all,

I was wondering if somebody could briefly explain the difference between the three types of Convergence norms employed in ANSYS.

As far as I can tell from reading the CNVTOL documentation:

INF norm causes the solution to iterate until the magnitude of the out-of-balance load vector falls below the magnitude of the maximum value within this vector?

The L2 norm causes the solution to iterate until the magnitude of the out-of-balance load vector falls below the magnitude of the SRSS of all values within this vector?

The L1 norm causes the solution to....????

If anyone could explain the L1 norm to me and correct my explanation of the other two where required I would really appreciate it!

Thanks!!
Dave

 

[kan123]

Section 15.13.2 of the Theory manual in ANSYS 12.1 explains the 3 different norms. Convergence is achieved when the "norm" (a scalar representation of the out-of-balance vector) is below a reference value you have selected (TOL x REF).
INF Norm = Max out-of-balance quantity
L1 Norm = Sum of the absolute value of all of the out-of-balance quantities
L2 Norm = SRSS of all of the out-of-balance quantities

So you see that L1 could be a pretty tight criterion to satisfy, so be careful how you choose TOL and REF. The default of L2 is usually a pretty good place to start for structural solutions. Once you have a solution that seems to converge OK, you can experiment with other settings.

INF Norm might be good when you're doing a nonlinear thermal solution. You can define convergence as being when all nodes have changed less than some particular value (for example, 0.001°C) from the previous interation.

 

[Dave442]

Hi Kan,

Thanks very much for your reply. I understand the NORMs better now.

I have been trying to figure out the CNVTOL command:

CNVTOL,Lab,VALUE,TOLER,NORM,MINREF

With SOLCONTROL,OFF ANSYS seems to iterate until the specified out-of-balance norm falls below either a program controlled VALUE or a TOLER*MINREF value; whichever is largest. i.e:

CNVTOL,F,calculated,0.001,L2,1.0

What exactly is the program controlled value? Also, if I wished to input the CNVTOL command to describe these default settings, how can I set the VALUE option to "calculated"?

Many thanks for your time, it is most appreciated.

Regards,
Dave

 

[kan123]

If you are doing a structural analysis with convergence based on force, then the program-calculated reference value is the magnitude of the applied force vector. This is the default. If you want a force balance within 0.1% using the L2 Norm, then the command is:
CNVTOL,F,,0.001,2 (don't need the 2, it's the default also).

 

[Dave442]

Hi Kan,

Thanks again for your explanation. What you have said makes sense to me, however, here is my problem.

I have a nonlinear structural analysis which converges ok when the only solution controls that I specify are:

ANTYPE,0 !!Define a Static Analysis
NLGEOM,1 !!Activate Large Displacements
AUTOTS,1 !!Activate Auto Time Stepping
NSUBST,100,1000,20 !!Set Number of Substeps

However, when I add the following line to set the convergence tolerance with default values:

CNVTOL,F,,0.001,2 !!Convergence Criteria

The actual solution that is carried out is different to the previous one. Looking at the monitor file it appears that many more iterations are carried out at most load sub-steps.

Also, looking at the solver output I can see that the force convergence value at almost every iteration is set as 0.1E-04. In my previous solution (without the CNVTOL command) the force convergence value varied each iteration.

Am I missing something here??

Thanks again!
Dave

 

[Dave442]

Its OK, I figured it out. I hadn't entered the command properly.

Many thanks Kan for the advice, much appreciated!

Kind Regards,
Dave!