Hello,

Can anyone help me to resolve the below issue.

I am facing Convergence issues with Solid185 elements.

i have tried to solve using time steps 5,5,20.but still facing issues.

Regards,

Velu A.

- 85 Views
- Last Post 03 July 2018
- Topic Is Solved

velu.annadurai
posted this
26 June 2018

Hello,

Can anyone help me to resolve the below issue.

I am facing Convergence issues with Solid185 elements.

i have tried to solve using time steps 5,5,20.but still facing issues.

Regards,

Velu A.

peteroznewman
posted this
26 June 2018
- Last edited 26 June 2018

Hello Velu,

I assume you have frictional contact in this model.

Did you insert a Contact Tool into the Connections branch of the Outline? Please do that and reply with an attachment for the Initial Contact Results.

Also, take a screen snapshot of the Solution folder Force Convergence Plot. Does it converge on the initial substep and later fail to converge, or does it fail to converge on the very first substep? That is important to know.

Have you turned on the Newton Raphson Force Residual Plots under the Solution Information folder. Those are very useful to show where the convergence problem is.

Finally, you can adjust the Contact Stiffness to help convergence. Sandeep's post provided a link to a good article on convergence issues.

Regards,

Peter

velu.annadurai
posted this
27 June 2018

Hello Peter,

Good day!!

Thank you for your view.

From the initial step itself it's not converging.

below are the references.

peteroznewman
posted this
27 June 2018
- Last edited 27 June 2018

Hello Velu,

I can see that the solver is trying to apply the entire load in the first substep (Time = 1). We can see that it cut the substep in half 3 times or a factor of 8.

Under Analysis Settings, Step Controls, change the Auto Time Stepping from Program Controlled to On the for Initial Substeps, type 10. That means it will apply 1/10th of the load during the first substep. You can see that in the last bisection, that it almost converged with 8 substeps or 1/8th the load. With 10 substeps, it should converge, but if it doesn't you can type 20 for the Initial Substeps. You can leave Minimum Substeps to 1. The Maximum Substeps must be larger than the Initial and I generally use 100 for that.

Regards,

Peter

akhemka
posted this
28 June 2018

As indicated above by Peter, try increasing the substeps - which will apply the load more gradually. On as safe side try increasing equilibrium iterations - neqit,100. Default is 25/26.

velu.annadurai
posted this
03 July 2018

Hello Peter,

Good day!

Increased sub-step but it didn't get converged.

pls advice.

peteroznewman
posted this
03 July 2018
- Last edited 03 July 2018

Hello Venu,

Click on Static Structural and insert a Command object. In the text window that opens, type NEQIT,100 as akhemka suggested. If you used Initial Substeps of 10, change that to 20.

Click on the Solution Information folder and in the details window, type 6 for the Number of Newton Raphson Force Residual Plots. Then click Solve. A plot will be created for the last 6 attempts to converge. The location of the maximum value on those plots shows you where the solver has the largest residual force, which may be larger than the convergence criterion. The corrective action can be to use smaller element size in the area of maximum N-R Force Residual. Sandeep's post provided a link to a good article on convergence issues.

velu.annadurai
posted this
03 July 2018

Hello Peter,

Thanks a lot for your advice which is really awesome.

- peteroznewman 107
- abenhadj 88
- SandeepMedikonda 83
- kkanade 67
- rwoolhou 66
- Aniket 38
- seeta gunti 30
- mazab17 30
- sk_cheah 23
- tsiriaks 18

Indu is a new member in the forum

lakshmidnair99 has been awarded the Your Question Solved badge

AgTKl has been awarded the Your Question Solved badge

EFP91 is a new member in the forum

brw205 is a new member in the forum