Learning Forum

[sypniewski]

Welcome, I'm a mechanical engineering student doing a simulation of a kind of push rod. The push rod is inside of an aluminum body that a min 0,1 mm distance from the face of this body. I create the model using surface to interpret of body. So i got in model with 10 surfaces and 1 solid body component of push rode:

I use structural steel NL (from ANSYS ENgineering Data) for push rode, and structural steel for surfaces (they are only for boundary and what contact pressure is). I make 0,4 mm thickness for each surface and bottom offset type. 
Contacts were generated automatically i changed the setting for frictionless type and target shell face as bottom, the details of contact and showing contact and target:

I generate general a mesh on the body using 1mm element size with capture curvature and capture proximity.  For surfaces, I make 2 different face sizing, first with 1 mm element size and second with 5mm element size. 
The mesh looks like:

Boundary condition are specified:
A - Force of component Fz = -100N
B - Fixed support at all faces 
C - fixed support on hole 
 

in the analysis setting i switch on Large deflection in this case is there auto time stepping: program controlled  i tried another option givingg around 150/200 initial steps but this does not help. 

In solution i got no convconvergent force 

I got this kind of warnings and error:

Could someone help how to deal with this kind of situation? I tried changing the mesh and some behaviour, and nothing helped.
Thank in advance!

[Dennis Chen]

 

I wish we can just upload archive files so it’s easier to provide quick advice.    But since I can’t actually run and troubleshoot myself, here’s a few steps I am hoping will help

1) turn on shell thickness effect in the contact pair

2) run contact tool (right click connection and add contact tool) – check initial penetration, if there are any, check geometry and resolve it

3) in the contact setting, change formulation to pure penalty (more sensitive to FKN, may or may not matter)

4) change normal stiffness to value and change the value to 0.1, also change update frequency to per iteration - aggressive in the setting below it. 

5) under solution information, change newton raphson residual from 0 to 4 (this generates some contours that allow you to troubleshoot from non-convergence occured)

Hope this helps.

 

[sypniewski]

I will try to use your advices and tell you if it helps. Also, I share a link with the archove of the simulation if you would like to check on your own.

link: https://drive.google.com/file/d/1lE8NXBaoHRWkU-3s8vWF3BKCoxxVfRsg/view?usp=sharing

[Erik Kostson]

 

To add to the above points – see here for some more advice:

https://edrmedeso.com/article/tech-tips-how-to-use-displacement-control-to-assist-convergence-in-ansys-mechanical/

(adjust to touch is also good and can help with convergence)

All the best

Erik