hi,

with the information you provided I can suggest a change in the mesh size. As you know, discretization is the first source in errors. Secondly, its the choice of interpolation functions. Using higher order functions reduces errors.

I could help more if I knew more about your case. As you mentioned longitudinal steel, if I understand correct, you may have large geometric deflections, lateral torsional buckling or issues relating to boundary conditions.

Thank you very much...I will try another time and tell if its OK...

You are welcome.

Let me share an experience. There was a struggling convergence problem for me in ANSYS recently. After studying graphical solution tracking which shows absolute convergence norm vs. iteration, I found out the number of equation iterations are taken as default by software (which is 15 to 26 iterations), so I increased this number and I noticed convergence. Besides, in some points exceeding yielding stress and entering plasticity in different parts can hinder the solve and show convergence issue. These might be due to geometrical characteristics.

Best

currently, i am working in ansys apdl for concrete encased steel plate beam. i am also having same problem. Solution not converge at some load step. before solving i got two model and one load error. because i am using solid 65 for concrete, solid 45 for bearing plate and solid 185 for steel its 8 noded element. but i am using tetrahedral element for both steel and concrete.

how to rectify that error..

Hi @Velrajkumar

if you are modeling concrete using SOLID65 legacy element with CONC material model then there will be high probability of solution non convergence if cracking and crushing are activated. Also this element is highly sensitive to the mesh size used, you can deactivate cracking and crushing of the element by setting them values of (-1) and then solve just to see if this is the reason behind non convergence. In general it's tricky to get SOLID65 element to converge with both cracking and crushing activated, the load (displacement controlled) should be applied at a very slow rate with a very fine mesh. You can try the newly developed Microplane model using SOLID185 with damage elasticity/plasticity or with CPT215 coupled damage plasticity.

There are 2 ways of inputting the micro-plane model, as the Release Notes explain for ansys Version 19:

"The micro-plane material model is now available in two forms: an elastic micro-plane model with damage, and a new coupled damage-plasticity micro-plane

A) The Elastic/plastic Micro-plane model with damage is supported by the element Solid185. A snippet example

ET,MATID,185 ! Define elements as SOLID185

MP,EX,MATID,29100 ! Define Elasticity Modulus

MP,NUXY,MATID,0.2 ! Define Poisson's ratio

TB,MPLANE,MATID,,6 ! Define the microplane model parameters

tbdata,1,0.75,0.75,0.208,6.109e-05,0.512,98 !k0,k1,k2,α_mic, β_mic, beta_mic

B) The Coupled Damage-plasticity Micro-plane model is supported by the element CPT215. This model was presented on the paper by Zreid and Kaliske (2014, 2016, 2018)

(Link to the 2018 paper: https://dl.acm.org/citation.cfm?id=3296167)

A snippet example

! Material Properties

ET,1,215 ! Define elements as CPT215 (Coupled damage plasticity) (Change Number 1 with Matid (material ID) if using workbench)

KEYO,1,18,2 ! Activate extra degrees of freedom

! Parameter values

E = 40300

nu = 0.2

dens = 2.4e-09

fuc = 36.5

fbc = 41.975

fut = 2.56

Rt = 1

D = 4e4

sigVc = -40

R = 2

c = 1500

m = 2.5

gamt0 = 0

gamc0 = 2e-6

betat = .4e4

betac = .25e4

! Define elastic properties of material

MP,EX,1,E ! Define Elasticity Modulus (enter a value for E)- (Change Number 1 with Matid (material ID) if using workbench)

MP,NUXY,1,nu ! Define Poisson's ratio

MP,DENS,1,dens ! Define material Density

! Define microplane model properties

TB,MPLA,1,,,DPC ! Define Drunker-Prager

TBDATA,1,fuc,fbc,fut,Rt,D,sigVc

TBDATA,7,R,gamt0,gamc0,betat,betac

TB,MPLA,1,,,NLOCAL

TBDATA,1,c,m