i think the following link will help you

https://www.sharcnet.ca/Software/Ansys/16.2.3/en-us/help/ans_adv/Hlp_G_ADV6.html

FEM, as you might already know, solves essentially the equation [u] =[K]-1[F]. where u, K and F represent Displacement, Stiffness and Load.

K is the so called Stiffness Matrix composed of the stiffness of each individual element. Element birth and death is simply setting these individual stiffness to zero by setting the Young's Modulus to 0. Well not exactly to zero.. it multiplies the Young's modulus with a factor of 10-6. So numerically speaking...0.

I usually simulate solder joints and quite often I need to include the soldering step where the joining material (in my case solder and your case.. whatever you are using to weld) is a liquid and offers no structural stiffness. So this is an ideal application for element birth and death.

A simple way to implement this is by creating a named selection of the weld.. say well .. 'Weld'

/prep7

estif,1e-8

cmsel,s,weld

ekill,all

allsel

/solu

and when you are done

cmsel,s,weld

ealive,all

allsel

Be careful about the reference temperatures you provide for your killed element or you might run into convergence issues. If this is the case, thats a topic for another question.

Hope this helps.

Thank you Allen

@ Allen George

can you please explain the reference temperature?

i am simulating a fillet weld and i have a problem with temperature distribution.

when I kill weld metal in both sides before welding, during the first pass because of the dead element on the other side, almost no heat transfer to the other side.

this happen when i choose 25 for reference temperature,but when i don't put any reference temperature temperature transfer but the minimum temperature is so high.

There is a small catch here, which I fail to understand.

Its ok that when we kill the elements, they offer no structural stiffness, load or boundary conditions.

But after solving the FE equation, it will be found that some non-zero displacements, strains and stresses appear for those killed elements.

So what is the logic behind this? Are these displacements fictitious?

In an incremental FE analysis, we need to carry forward the displacements of one load step to solve the next load step.

So, my question is, what do we do with these fictitious displacements in this case?

Maybe you can read the paper "Article Node dynamic relaxation method: Principle and application