Learning Forum

[Renir Reis Damasceno Neto]

Hello guys,

I'm having issues in converging the following static structural analysis. Could you please help me to identify where the error should be?

There are 3 components: 1 spherical head inside 1 smaller cup inside 1 bigger cup.
The spherical head is a perfect sphere, but the cups are not perfect shapes (they have multiple radius).

I want to simulate a sitting force, to pressfit the 3 components together.

The two contact pairs are the following:
   1. Frictional 0,05 between head and small cup
       Small distance between them (0,42 mm)
       Interference treatment: adjust to touch

   2. Frictional 0,2 between small cup and big cup.
       Small distance between them (1,1mm) (though there are some points with small penetration = 0,07mm)
       Interference treatment: Add Offset, Ramped Effects

Mesh (Figure 2)
   Default with adaptative size = 6
   Refinement around the small cup antirotative tabs

Static Structural (Figure 3)
   Fixed support in the outer face of the bigger cup.
   Weak springs on.
   2000N applied against the spherical head, simulating the sitting force.

I tried adding substeps and slowly increasing the force, but with no luck.

Thank you in advance for any ideas!

[Akshay Maniyar]

Hi,

What is the error message you are getting when it is failing? Make sure that you have selected the contact and target side correctly while defining the contact. Please check the below Ansys video for more details.

https://www.youtube.com/watch?v=yUhTaTwM-c4

Can you try using the detection method as combined and the normal stiffness factor as 0.1? Also, please check the Newton-Raphson residual plot for finding the problematic region.

Thank you,

Akshay Maniyar

How to access Ansys help links

Guidelines for Posting on Ansys Learning Forum

 

[Renir Reis Damasceno Neto]

 

Hi Akshay, thanks for your reply!

Please find below some new results considering your suggestions. I’ve reached convergence, but I’m not sure about the physical representation of those changes.

 

1. I’ve checked the contact/target selection and it’s well defined (also I’ve tried switching it with no success).

2. The solution fails after a few iterations, there are three warnings:

•    One or more bodies may be underconstrained and experiencing rigid body motion. Weak springs have been added to attain a solution.  Refer to Troubleshooting in the Help System for more details. (in the beginning of the simulation)
•    Contact status has experienced an abrupt change.  Check results carefully for possible contact separation. (around 4th iteration with no convergence)
•    One or more contact pairs exceeds contact small sliding assumption, check your results carefully.  Consider using Large Deflection or turning off Small Sliding on the offending contact pair(s).  You may select the first offending pair via RMB on this warning in the Messages window.  Additionally, you can use the “Number With Too Much Sliding” Contact Results Tracker to locate any additional pairs.

 

3. I’ve selected the normal stifness factor as 0,1 for both contacts, but I couldn’t find the detection method as combined.

 

New simulations run:

A: Applying normal stifness factor as 0,1, the Newton-Raphson residual plot shows residual force in the contact inner surface of the outer bigger shell:

B: Since the previous simulation showed residual force in the outer shell border, I’ve tried refining it. The residual force is low, but still present, still missing the convergence.

C: Finally, it’s reached convergence, adding the normal stiffness factor 0,1 and Detection Method as on Gauss point.

The question is: Do those changes in the model affect phisically the model? Are there any other changes that could be applied instead to reach convergence but still have a good physical representation?

In this case is very important to simulate the interactions between the components. Just for you to know it’s a real case in which the antirotative tabs (at the outside border of the small cup) have broken in use.

 

 

 

[Akshay Maniyar]

Hi,

According to the warning messages, weak springs are created as some of the parts are not properly constrained. Ensure that the reaction in weak springs is significantly smaller than the applied force and that all parts are properly constrained. You can also try to switch off the small sliding option under contact settings if you are expecting large sliding. 

Also, Is large deformation ON? If not, then please try to switch it ON and try to run the model. Always turn it on, unless the model is truly for small strains, small deformations, small rotations, and small sliding. 

Thank you,

Akshay Maniyar

How to access Ansys help links

Guidelines for Posting on Ansys Learning Forum