## General Mechanical

#### increase the value of the criterion

• Riccardo Petrelli
Subscriber

I'm doing a nonlinear analysis, every time I find this value which is much smaller than the convergence force, is it possible to increase it without making them do many iterations?  thank you

• Riccardo Petrelli
Subscriber

• peteroznewman
Subscriber

It is possible to increase the Force Criterion value, but you should first look for the reason why the Force Convergence line is not dropping below the Criterion line and take corrective action first.

Under the Solution branch click on the Solution Information folder. In the Details window is a line that says Newton-Raphson Residuals. The default is 0 but type in a number such as 3 or 4. This will cause 3 or 4 plots to be saved under the Solution Information folder which show the residual force imbalance in the mesh for the last 3 or 4 iterations. Look at the plots and zoom in on the location with the Maximum value. This location needs smaller, better quality elements. If you remesh to achieve that, the convergence will often be achieved.  Sometimes these plots will have the Max value in the same place, but other times the Max value will jump around to different locations.

Here is an article on convergence.

In your reply, please paste an image of the plot around the location of the Max value of the Newton-Raphson Residual for the current mesh and another image to show the improved mesh and let us know if the model now converges. Improving the mesh is how you get an accuracte solution. Relaxing the Force Criterion means you are accepting less accuracy in the solution.

Here is a thread on how to change the Criterion.

• Riccardo Petrelli
Subscriber

I want to drop the stress strain curve in my lattice structure, simulating failure. So I created this script to do it. Is this the right procedure? Or is there an easier way? thank you

i want reprodu

• Riccardo Petrelli
Subscriber

this is my material

• Riccardo Petrelli
Subscriber

The sudden increase in value is due to the elimination of the element that exceeds a certain stress and strain threshold (actually with the command estif 0.5 I am lowering its stiffness). I am attaching my script.

total_steps=20
subst_int=10
subst_max=18
subst_min=10
neqit, 120 !numero massimo di iterazioni di default è impostato su 15

*do,i,1,total_steps
/gopr
time_step=i/total_steps
time,time_step
nsubst,subst_int,subst_max,subst_min
outres,all,all
esel,all
solve
finish

/post1
set,last

esel,all
etable,stress,s,eqv
esel,s,etab,stress,ARG1
!    *get,stress_ecount%i%,elem,0,count
cm,kill_stress%i%,elem
cmsel,s,kill_stress%i%,elem
!    *get,stress_ecount%i%,elem,0,count

esel,all
etable,strain,epto,eqv
esel,s,etab,strain,ARG2
!    *get,strain_ecount%i%,elem,0,count
cm,kill_strain%i%,elem
cmsel,s,kill_strain%i%,elem
!    *get,strain_ecount%i%,elem,0,count

allsel
cmwrite,kill_list,cm
parsav,all
finish

/solu
antype,,restart
parres
!    *status
/input,kill_list,cm
*do,k,1,i
estif, 0.5 !moltiplica la matrice di rigidezza di 0.5
ekill,kill_stress%k%
ekill,kill_strain%k%
!      *status
*enddo
*enddo
finish

my value for stress eq is 1750 and strain 0,032

note that the number of steps is not the one written in the script, because I don’t remember it for this case.

• Bill Bulat
Ansys Employee

You can use the CNVTOL command to adjust convergence criteria:

You can also use NCNV,0 to tell MAPDL to continue solving even if the convergence criteria are not satisfied after the maximum number equilibrium iterations have been reached.