Separation Contact Fails to Converge for Shell Elements

[darrenlovesmusic]

Hi,

I'm running a test case for a separation and offset bonded contact that fails to converge.

I have tried the following based on several past forum posts: 

1. Maintaining contact activation distance as 1.2 x gap distance 

2. Maintaining contact activation distance as Sqrt(Mesh size^2 + Gap^2)

3. Changing ADAPTLNCONTACT

4. Changing SLINEMAXPENDIST 

5. Changing offset penetration distance to gap/2 

6. Changing SLINESLIDETYPE 

I'm using Nastran 2020 (linear static) and the gap for this application is 0.2 inch. What could be the problem? Also, I get some absurd values for displacement eg 10^8 in

Thank you. Model attached for those who may want to try. 

[darrenlovesmusic]

@John_Holtz do you have some suggestions for this problem? 

[John_Holtz]

Hi @darrenlovesmusic 

There is no constraint in the Y direction. So when you apply a load in the -Y direction, the model moves an "infinite" distance (4E8) in the Y direction. The analysis should not even solve, but somehow it finds enough stability to gives an approximately correct answer. 😁

When I add an artificial Ty constraint and delete the separation contact, the analysis run and looks reasonable. (I think a maximum activation distance of 0.25 is to small for a 0.2 gap and 0.5 mesh size.)

[darrenlovesmusic]

@John_Holtz  Thank you for taking a look. The structure is stable probably because one section is fixed in separate cylindrical co-ordinates. But my query is pertinent to the separation contact only. It can never reach convergence and I'm driven to my wits end. Is it to be treated as a nonlinear contact? I posted a simple geometry, but I have to analyze a huge safety platform on a pressure vessel. The solution blows up when even a single separation contact is used. 

[John_Holtz · Accepted solution]

Hi,

Just to clarify one item, I like to consider a model as unstable if it relies on separation contact to make it statically stable. Why? In general, what points are in contact is not known until the displacements are calculated, and the displacements cannot be calculated until which points are in contact is know. The solution becomes an iterative problem, and there are a number of factors during the iterative process that can go wrong.

So, perhaps your model is one of these:

• Before defining contact, the model runs correctly. Adding separation contact causes the analysis to not run properly. (Adding, not changing, a contact is the key here.)
• Before defining contact, the model runs correctly. Changing one of the existing contacts from bonded to separation contact causes the analysis to not run properly. (Most likely the model becomes unstable when the contact is changed.)
• Something else.

A nonlinear static analysis can solve better when separation contact is involved. Here are the steps that help to make the nonlinear analyis run as quickly as possible:

1. When changing the analysis type to nonlinear, set "Options > Large Displacements" to "Off". 
2. Edit the Nonlinear Setup and enter 1 for the "Number of increments".
3. In some cases, the nonlinear analysis will struggle to converge (going into subincrements) or fail to converge. In this case, edit the "Nonlinear Setup > Advanced Options" and set the "Initial Load increment" and "Minimum load increment" to a really small value (such as 1.0E-4), and set the "Maximum load increment" to a large value (such as 0.2). The analysis will apply a very small load (1E-4 times the applied load) to "bring the parts into contact", and then increase the load increment using larger and larger values (up to the maximum of 0.2 times the applied load) on each step. It may take 10-20 steps in total to solve.

•  

[darrenlovesmusic]

Thank you John. I think there are a few issues with separation contact and shell elements. For now, Ive decided to NOT use separation contact and find workarounds to transfer loads correctly.