# Another conditions for connection

mekafime
Member

in Structures

Hi,

I have the next K-gap connection, when I use Cylindrical support in the diagonals the solver solves it without problems, but that condition is not real, when I use the real condition in the external face of the diagonal I restrict the movement so that it moves axially the solver has problems in the convergency. Please, What I can do?

screenshot 1: external face of the diagonal restricted to move axially

Screenshot 2: Cylindral support in all diagonal

## Comments

Hello Mekafime,

Please provide more information to get help on this model.

Regards,

Peter

Hi Peter,

Thanks for the additional information. You didn't request any Newton-Raphson Residuals under the Solution Information folder. You must always ask for 3 or more whenever you have convergence difficulties. I hoped you would know that from your previous experience.

You only had 1 element through the thickness. With a Cylindrical Support, that didn't matter, but with the end displacement it does. I have changed that to provide a minimum of 2 elements through the thickness in Mesh Details, Capture Proximity.

The mesher used 3 elements on the pipes.

I put in a Sweep Mesh Method, to limit it to 2 elements to reduce solve time.

This is running now.

Your forces would allow you to use 1/2 symmetry on the XY plane, which would cut the solution time in half.

Regards,

Peter

Hi Peter,

Thanks for your quick response. I activated that method but that marked the error in the diagonal (figure 1), I did not know because there, if there were no other elements nearby (connection) I did not think it was thick, a thousand apologies.

Hi Mekafime,

Here is what I found when I ran the model described above.

1) There was a warning message, which I read, but decided to ignore and let it run.

Maybe changing the contact stiffness would have let this model finish. I don't know.

2) The model failed to converge near the end with a highly distorted element error. I created a Named Selection to see where this element was. It was at the contact face.

So contact elements are holding the two element thick pipe to the elements on the rectangular tube.

I don't personally like having contact elements in the middle of a volume experiencing plasticity. Maybe other members can chime in here, but I prefer to have my contact elements away from the volume experiencing plasticity. What that means is you have to use Shared Topology to make a connection between the diagonal pipe and the center portion of the rectangular tube. Without any extra slicing, that will probably result in one or both bodies being meshed with tet elements. To avoid having the whole length of the tube meshed with tet elements, you can slice off the ends, which can have a swept mesh, and just leave the a minimum volume around the welded area to have tet elements as shown in my example below, which started out as a straight pipe with a diagonal strut, but failed under an end load.

Regards,

Peter

Hi Peter

Thanks for your time. How many divisions did you put to the thickness to avoid failure by Newton?

I put 2 and I used half with the symmetry

Hi Mekafime,

It failed to converge with a full model and 2 elements through the thickness.

I am rerunning it now with the contact stiffness factor of 0.1 to see if it converges.

Hi,

At the location of element distortion, please try using a large element, a coarse mesh (if the stress is not expected result at the location). Coarse mesh helps a little bit with distortion. Also a linear mesh - coarse at distorting location - and fine at region of interest may help. Try increasing substeps and number of equilibrium iterations.

Regards,

Ashish Khemka

Hi Mekafime,

Model failed to converge with contact stiffness at 0.1 and 2 elements through the wall thickness.

I remeshed with 3 elements through the thickness and the model again failed to converge.

Below are the Newton-Raphson Force Residual plots showing where the 3 element model had difficulty.

The interesting observation of this 3-element models compared with the 2-element through-thickness model is that the convergence problem has moved away from the contact area between the diagonal pipe and the rectangular tube and is now showing on the deformation in the rectangular tube itself.

I increased the rectangular tube to 4 elements through the thickness and to reduce the solution time, I used symmetry to cut the model in half. That model is running now. I also checked if the Iterative solver was the better choice for solution time and it was much faster at iterating than the Direct solver. On 12 cores, the solver takes about 5.2 minutes/iteration.

One question I had about the geometry was if the thicker wall in the corner was intentional?

To have a uniform wall thickness, either the inner corner radius should be smaller, or the outer corner radius should be larger.

Regards,

Peter

Hi Peter,

I used the ratio in 1.5*thickness (4.8 mm x 1.5 = 7.2 mm) and I extruded the thickness. I did not notice it

Hi Mekafime,

This is your corner dimensions:

Keep the 7.2 mm inner radius, but to maintain a constant wall thickness, the outer radius must be 7.2+4.8 = 12 mm.

This change may also improve the shape of your elements! The 4-element thick model is still running, but maybe it needs a new corner radius?

Regards,

Peter

Hi Peter,

I think that the model must converge like this first and then modify the radius.

I am testing other configurations

Hi Mekafime,

The half model with 4 elements through the thickness of the rectangular tube did not converge to the full (half) load.

I broke the load into 2 steps to use much smaller steps when the previous models got into trouble. Step 1 ramped the force up to 75000 N taking a minimum of 40 substeps, then Step 2 increased the force to the full half load of 85000 N and also took a minimum of 40 substeps. The convergence plot below shows the model getting into difficulty converging.

I stopped the solver after the bisection occurred. This represents 14.6 hours of computation on 12 cores.

The first N-R Residual Force Maximum is located under the compressive tube.

The second N-R Force Residual Maximum is on the Tube.

Since you are applying a force and not a displacement load, I plotted the Force-Displacement graph for a point on the end of the diagonal tube to look for evidence that the slope was approaching zero. It is not.

I believe smaller elements will help this model to converge, however, I don't want to wait 20+ hours for the computation to finish when a 6-element through-thickness mesh is created.

Since all the interesting behavior is at the intersection of the tubes, I recommend you create 4 planes and cut the rectangular tube and the pipes through at a 200 mm distance from the center. Then you can mesh the bodies near the center with six elements through the thickness, while the bodies away from the center can be meshed with two elements through the thickness. Use Bonded Contact to connect the outer bodies to the inner bodies. That way, the solver will take much less time to run.

If you want me to run that model, please make those changes and send me an archive. You might also change the corner radius to get a uniform wall thickness while you are at it.

Regards,

Peter

Hi Peter

very grateful for your time, I will make the respective modifications according to what you tell me and I will show the result