Model not converging after radii added

[RichardOliver4462]

I have a model which will have an internal pressure added, the original model was received with no radii and made from flat plates. I applied an internal pressure and ran as both a linear static and non-linear static with no problems. This showed high stresses at the edges of the flat plates so I added 30mm radii all around. Materials were re-assigned and loads added - model still runs fine as linear static but get an error when trying non-linear static as follows:

WARNING: E5078: SOLUTION HAS DIVERGED

WARNING: E5075: BISCETING CURRENT LOAD INCREMENT

This is a simple model and therefore am surprised it 'falls over'

[John_Holtz]

Hi Richard,

It is hard to know what is causing the problem. It could be that the radii have changed the mesh, which created distorted elements, which is causing a convergence issue. Are you able to provide the model? (If an assembly, you would need to zip/compress the parts and assembly files together.) You can either attach it to a reply, or send it to me in a private message.

[RichardOliver4462]

Hi John,



Please find model attached, if I suppress the radii that have been added it
will run as a non-linear static - but not with the radii.]



Many thanks,



Richard Oliver

[John_Holtz]

Hi Richard,

When you say the model is attached, do you mean the model is attached or that you intended to attach it but forgot?

Note that if you are having problems with uploading attachments, you might need to use a different browser. I recall problems in the past, but cannot remember if it was due to the browser or corporate policies.

[RichardOliver4462]

I replied to the email in Outlook and attached the file - I see though this
posts it on the forums, without the attachment.



What is your email address so I can send the file.



Thanks

[John_Holtz · Accepted solution]

Hi Richard,

Here is what I see in the model that has the radii. There are a few spots where the edges include a very small radius of curvature. When a "large" element is placed around it, the element can have a poor quality shape. Instead of being a "4 sided element", it looks like a 5 sided element with a "backward" angle on the one side.

It is easier to see where this occurs in the model if you download the attached two images and cycle through them with a photo viewer. (See "model - poor quad.png" and "model - poor quad.png" attached. You may need to view the forum post on the internet to access the attachments.)

When I made the following changes, the nonlinear analysis solved without a problem:

1. Under the "Advanced Mesh Settings" ("Mesh > Mesh Settings > Settings"), I unchecked the box "Project Midside Nodes". When unchecked, the midside nodes will be exactly halfway between the corner nodes instead of following the curvature of the edges and surface.
2. I used a mesh size of 10 mm.

The maximum stress was 674 MPa. How does that compare to the analysis without the radii?

For everyone's education, one reason to perform a nonlinear analysis is because it includes effects such as the stiffness changing as the model deforms. Linear analysis ignores this effect (which is valid if the displacements are small) and will calculate larger and larger displacements as you increase the load. The linear analysis gave a maximum displacement of 35 mm (on a model that is 1.3 m long). The nonlinear analysis gave a displacement of 9.4 mm. That is quite a difference!

[RichardOliver4462]

Thanks John I have this working now.

If I remove the radii and run as a linear static model then non-linear I get 1355MPa stress / 38mm displacement and 895MPa / 10mm displacement respectively.

Indeed the use of the non-linear analysis in a model of this type does make a big difference.