1 (edited by pavlo 2019-05-15 17:25:00)

Topic: Convergence problem

Hello!

I have a problem with convergence. I found a node with maximum residual force and compared it with internal force in the same node. The absolute values are equal (only sign is opposite). I assume that this node is the problematic one which leads to convergency problem. The values are relatively small respectively to the problem size and I would just ignore it but I am afraid to miss the point of failure while convergency problem would signal about exhausting of member capacity.

How can I eliminate this problem?

Which reason can cause such problem?

MODEL

Re: Convergence problem

screenshot of results

Re: Convergence problem

Dear Pavlo,
1. I assume you have already read Troubleshooting, 2.1.19 Problems reaching convergence and understanding ATENA convergence parameters.

2. Have you already tried to allow more iterations or change the step length to reach full convergence (errors below the 1% tolerances)?

Regards.

Re: Convergence problem

Dear Dobromil,

1. I already divided self weight application into 20 steps and I have 6 steps non-converged of 20. Iteration limit is set to 500.
Relative error for Criteria 2 exceeds 5% (see screenshot). What I didn't try is to use initial stiffness for iterations. But I am amfaid I cannot use this approach to find an ultimate force for my structure.

2. As I wrote above, iteration limit is 500 and iterations do not tend to converge so I don't think it is reasonable to increase number of iterations more than 500. I would allow even 5% tolerance for forces but the fact that I have convergency problem in such unexpected place means that I cannot rely on results of the calculation. I'd like to find the root of the problem and eliminate it to meet convergency problem while achieving ultimate capacity and failure rather than while facing some numerical problems...

Could you please check what exactly is the problem with that node?

Re: Convergence problem

Reagarding using Elastic predictor and update stiffness each step. As I understand this approach cannot be used to solve problem from zero to failure. It is only to pass problematic steps. The point is that almost all steps are not converged so this way is not applicable to my case, am I right?

Re: Convergence problem

Dear Pavlo, of course you can try with the Modified Newton-Raphson (Elastic Stiffness, Each Step) from the beginning.

7 (edited by pavlo 2019-05-13 14:26:20)

Re: Convergence problem

Dear Dobromil,

I modified the model with shells and frames instead of all solids. However, I get the same problem in the same place even with ISOBEAM (see Fugure1 from link below). The point is that stresses in rebars in this joint are very low (15-20 MPa), and in concrete also very low: compression <3.5 MPa, tension 1.7 MPa while FT=2 MPa).
Regading this issue I have several questions:

1. I assume that the problem comes from the fact that crack occurs exactly at Master-Slave connection. Reaction between wto contacts should be equal to zero but it is always more than zero. Therefore, relative error is very high. Does it mean that I should always avoid Master slave where crack is assumed?

2. Elements in beams are not always bricks. Some of them are skewed. Is it OK? (see Figure 2)

3. Beams elements are connecred with MS contact (see Figure 2). Is this correct? Is there a need to make mesh consistent?

4. Beams are connected to walls and slabs with MS as well. Is this approach correct? (Figure 3)

5. Would you please review my model and advice what can be a problem with convergency in problematic node? (AtenaCalculation.rar - last nonconverged step results only, FT4_v10.gid.rar - GiD model without results)

https://drive.google.com/open?id=14VRRZ … TBEMcdGk2c

Re: Convergence problem

Dear Pavlo,
briefly looking at the screenshots, the mesh for the 2 short connections in the IsoBeam seems problematic - even the 3 elements in the opposite single connection beam are on the edge for beam elements already - note the assumptions are that the cross section dimensions are small compared to element length. Usually, element length comparable to cross section dimension can still work reasonably, but the 2 short beams are clearly over the edge.

I would recommend to change the mesh settings such that the elements generated in the beams have length comparable with the larger dimension of the cross section (height). Then, also the skewing is going to be less extreme.

Regards.

Re: Convergence problem

Dear Dobromil,

I changed the mesh. It seems normal now. However, I still have the same problem!

I kindly ask you to review my questions again and give your comments. Many thanks in advance.

1. I found that M-S connections was not a root of the problem. I changed mesh to compatible in problematic joint and got the same results. However, please comments whether it is possible to use MS condition while connecting incompatible mesh frame-to-frame and shell-to-frame.

2. Resolved

3. Beams elements are connecred with MS contact (see Figure 2 from message #7). Is this correct? Is there a need to make mesh consistent?

4. Beams are connected to walls and slabs with MS as well. Is this approach correct? (Figure 3 from message #7)

5. Would you please review my model and advice what can be a problem with convergency in problematic nodes? (FT4_v12.gid.rar - GiD model without results). Please note that in problematic beams stresses in rebars are very low (less than 250 MPa) and failure should not occur (see FT4_v12.avi from the link below).

6. Cracks in shells and frames are shown through the full height of the element (see CRACKS.PNG from the link below). It looks totally enormous from structural point of view. Is there a modeling mistake or is it a symbolic representation of ATENA?

https://drive.google.com/open?id=13xNmg … 4Drw1bUqw4

Re: Convergence problem

Dear pavlo,
the solution setting in FT4_v12.gid do not make much sense - increased Residual Error tolerance (to 5%), and I see you are using Tangent predictor together with stiffness matrix update in each step, which does not make any sense? The 2 usual settings are
A. Full Newton-Raphson = Tangent + Each Iteration
or
B. Modified N-R = Elastic + Each Step.

Ad 6.: The cracks are drawn in Elements, however, it is also possible to show them in each Integration Point (without the averaging to get 1 per element).

Ad 3, 4: mesh compatibility between beams/shells and volume elements does not bring any advantage. Similarly for connecting the side surfaces of shells/beams to head/tail surfaces of these.

Regards.

Re: Convergence problem

Dear Dobromil,

Here are my replies:

3,4 - OK, it is really good because compatible mesh preparation in GiD takes too much efforts.

6. Still crack pattern looks almost same on bottom and top surfaces while there should be no cracks at bottom surface. Please watch the video : https://drive.google.com/open?id=1cQ1y7 … w8stjl3CfN

Regarding solution method. I couldn't find Modified N-R in GiD 14 (script 16595). Does it mean that only Full N-R and Arc-Length are only available for GiD users?

Re: Convergence problem

Dear Pavlo,
ad 6.: it does not make much sense to project the cracks in IPs on element surfaces (I think it is not possible in Egr 3D...). Switch to Wireframe, show the IPs, then display the cracks in IPs.


Ad solution methods: I guess you are searching for a button choosing Full or Modified NR? The situation is that you select

A. Tangent stiffness, After Iteration - and this corresponds to the Full Newton-Raphson

or

B.  Elastic stiffness, After Step - and this is the Modified Newton-Raphson.

In both cases, you of course choose Newton-Raphson (and not Arc Length).

Regards.