Learning Forum

[mekafime]

Hi

The model below does not converge for a load of 170 kN on one diagonal and -170 kN on the other, however when under load at 130 kN and -130 kN respectively the model does converge. Please what would be the mistake?

Attached File in 2019 R3

[Aniket]

Ansys Employees can not download the files. But in general, increasing substeps should help you to converge this problem.

-Aniket

Guidelines on the Student Community

How to access ANSYS help links

[mekafime]

Hi Aniket

 

This is my configuration but I tried increase substeps and the results is the same.

 

[Aniket]

what error do you get in the solve.out file?

[mekafime]

 

[peteroznewman]

Element 24213 has become highly distorted. 

If you type a nonzero number into the Identify Element Violations field under the Solution Information folder details, then Mechanical will automatically create a Named Selection to show you that element.   If you left it zero, you can manually create a Named Selection using the Worksheet to show which element that is. Please reply with an image of that element.

One corrective action may be to improve the element shape, pre-distorting elements in that location in the meshing phase, so that as the load is applied, the deformation causes the element shape to improve as the load is applied.

Another corrective action may be to get rid of the bonded contact and replace it with bodies connected via shared topology. That might require some of the bodies to be meshed with Tet element, but those are very good at tolerating distortion.

 

[mekafime]

Hi Peter,

I suppose that the section change between elements is abrupt because there is no node that communicates them

 

I am using boolean to unite solidos and tet mesh, waiting results ...

 

[peteroznewman]

Here is one of the elements that became highly distorted.

These are quadratic elements which don't like their midside nodes getting too far out of line. One idea is to change to linear elements while also halving the element size. This will put a node much closer to the bonded contact edge of the other part and eliminate the midside node, making elements that are more tolerant of distortion.

Getting rid of bonded contact is a better idea when it comes to modeling plasticity. With some effort, the parts could be sliced to maintain hex elements and use shared topology instead of tet elements.

[mekafime]

Hi Peter,

I used boolean to unite in a only, and hex elements , but when I use topology the analysis failed because I avoid use topology.

The model analyzes successfully

For my thesis I am analyzing this type of tubular connection by varying the separation between the diagonals and I get the Force - Displacement curve as a response, with Force being the axial force acting on the compression diagonal and the Displacement the deformation of the upper flange face (horizontal element) by action of the diagonal compression.

The solids to analyze them with solidworks, as I mentioned only by varying the distance between diagonals and charged to the design modeler, thus having several 3D models and several Ansys files, from which I obtain my graph and gather the curves in Excel. For the model in ansys a mesh study was made.

My problem is that:

In the first curves there is a trend, however in the following this trend is broken and there are many variations.

The end of the curve is the break point (elongation at break 23%) for the type of material used in the analysis.

What can I do to standardize, or is that the result? I also planned to make the model in design modeler and parameterize it, but if it is the same….

Please waiting for your comments.

[peteroznewman]

Please reply with a more detailed description of Displacement, maybe with a sketch or image.  Why is Displacement important?

Also, attach a copy of your spreadsheet in a zip file so I can look at it more closely.

[mekafime]

Thanks Peter.

The node taken for displacement is (2 cm from the outer foot of the diagonal) :

The displacement is important because in a curve Force-Displacement , I can obtain the maximum force that I can apply to the diagonal depending on the width of the chord.

I include the model with the smallest and largest distancing.

 

[mekafime]

The files are in Ansys R3

[peteroznewman]

I ran each model you provided. Nice mesh.

What I asked for was the spreadsheet that had the Force-Displacement of all values of the parameter d.

The idea I had was to normalize Displacement by the parameter d.

Or maybe just plot data directly against the parameter d.

[mekafime]

Hi Peter,

Thanks for your time.

I add the spreadsheet of Force-Displacement. 

[mekafime]

Hi Peter,

I try to change the mesh, but ... nothing ! ... the result is the same all models they don´t follow a trend although some want to accomodate certain models move away from the trend.

[mekafime]

Hi Peter
Could you normalize the displacement?

Thanks you