Boundary conditions for seabed response under wave action

bigphil · July 21, 2021, 08:27

The convergence seems ok to me. In this case, 5 residuals are written:

resD: initial residual from the D equation
resP: initial residual from the p equation
relResD: alternative residual calculated as the max normlaisied difference between D and the previous iteration of D
relResP: alternative residual calculated as the max normlaisied difference between p and the previous iteration of p
matRes: residual from the mechanical law; in this case it is always 0 so this law does not define a residual

The reason for the alternative residuals is that sometimes the equation initial residuals fail to show convergence even when the fields have stop changing (seems to be related to the choice of normalisation factor that is used), so solids4foam will assume convergence is achieved if any of the following conditions are met:

if resD and resP and relResD and relResP are less than the specified solution tolerance
if resD and resP are an order of magnitude less than the specified solution tolerance
if relResD and relResP are an order of magnitude less than the specified solution tolerance

In any case, you can always tighten the tolerance and see if the results change.

As regards the displacement field, are you looking at the same component in both COMSOL and OpenFOAM? I cannot see the name of the component on the COMSOL image.

And for the difference in rKprime, you can try change it and see what effect it has.

Philip

qi.yang@polimi.it · July 21, 2021, 08:59

Quote:

Originally Posted by bigphil

The convergence seems ok to me. In this case, 5 residuals are written:

resD: initial residual from the D equation
resP: initial residual from the p equation
relResD: alternative residual calculated as the max normlaisied difference between D and the previous iteration of D
relResP: alternative residual calculated as the max normlaisied difference between p and the previous iteration of p
matRes: residual from the mechanical law; in this case it is always 0 so this law does not define a residual

The reason for the alternative residuals is that sometimes the equation initial residuals fail to show convergence even when the fields have stop changing (seems to be related to the choice of normalisation factor that is used), so solids4foam will assume convergence is achieved if any of the following conditions are met:

if resD and resP and relResD and relResP are less than the specified solution tolerance
if resD and resP are an order of magnitude less than the specified solution tolerance
if relResD and relResP are an order of magnitude less than the specified solution tolerance

In any case, you can always tighten the tolerance and see if the results change.

As regards the displacement field, are you looking at the same component in both COMSOL and OpenFOAM? I cannot see the name of the component on the COMSOL image.

And for the difference in rKprime, you can try change it and see what effect it has.

Philip

Thanks. I realized no matter "all converged" or "relative converged", the solution does not change to a large degree. As a matter of fact, the displacement should be distributed as shown in the figures, at least qualitatively. Both of them are horizontal displacement. The strange thing is that displacement on the surface is greatly different from each other. Furthermore, I tried to make all equations and corresponding constants consistent then I did not find significant difference.

bigphil · July 21, 2021, 09:20

In COMSOL, the horizontal displacement at the surface (seabed surface) seems to be exactly zero. Is it possibly that the horizontal displacement on the surface is constrained to zero in COMSOL?

qi.yang@polimi.it · July 28, 2021, 06:48

Dear Prof.,

In order to consider the wave force exerted on the structure embedded on the seabed, it requires to implement a dynamic wave force on the structure thereby "timeVaryingTraction" boundary condition should be used, I think, which I found in Tangtian's source code and literature, like the similar condition used for implementing dynamic wave pressure on seabed by "timeVaryingAveragedValue". Thus, is it possible to add an additional boundary condition to achieve this goal? Thanks for your attention.

bigphil · July 28, 2021, 10:00

solidTraction can be optionally time-varying.
For example, it can be defined in any of the following ways:

Code:

myPatch
{
    type        solidTraction;
    traction    uniform (0 0 0);
    pressure    uniform 0;
    value       uniform (0 0 0);

or

Code:

myPatch
{
    type        solidTraction;
    tractionSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsTraction";
        outOfBounds    clamp;
    }
    pressure    uniform 0;
    value       uniform (0 0 0);

or

Code:

myPatch
{
    type        solidTraction;
    traction    uniform (0 0 0);
    pressureSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsPressure";
        outOfBounds    clamp;
    }
    value       uniform (0 0 0);

or

Code:

myPatch
{
    type        solidTraction;
    tractionSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsTraction";
        outOfBounds    clamp;
    }
    pressureSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsPressure";
        outOfBounds    clamp;
    }
    value       uniform (0 0 0);

where the timeVsTraction file looks like, for example:

Code:

(
    ( 0.   ( 0 0 0 ) )
    ( 1.5   ( 1e4 2e5 3e4 ) )
    ( 10.4  ( 4e4 5e4 5e5 ) )
)

and timeVsPressure like, for example:
the timeVsTraction file looks like, for example:

Code:

(
    ( 0.   0 )
    ( 1.5   -10.6e5 )
    ( 10.4  3e5 )
)

qi.yang@polimi.it · July 29, 2021, 10:43

Quote:

Originally Posted by bigphil

In COMSOL, the horizontal displacement at the surface (seabed surface) seems to be exactly zero. Is it possibly that the horizontal displacement on the surface is constrained to zero in COMSOL?

I checked the boundary condition at the surface again, there is no constraint for displacement there, in which only wave pressure is applied. In addition to the PDE model, I created a multiphase model combined with solid mechanics and Darcy's law, which is nearly the same as the solids4Foam model implemented in OpenFOAM and I also did not prescribe a boundary condition for the seabed surface regarding displacement. As you can see, the horizontal displacement is different from the one calculated by openfoam.

qi.yang@polimi.it · July 30, 2021, 05:53

Quote:

Originally Posted by bigphil

solidTraction can be optionally time-varying.
For example, it can be defined in any of the following ways:

Code:

myPatch
{
    type        solidTraction;
    traction    uniform (0 0 0);
    pressure    uniform 0;
    value       uniform (0 0 0);

or

Code:

myPatch
{
    type        solidTraction;
    tractionSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsTraction";
        outOfBounds    clamp;
    }
    pressure    uniform 0;
    value       uniform (0 0 0);

or

Code:

myPatch
{
    type        solidTraction;
    traction    uniform (0 0 0);
    pressureSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsPressure";
        outOfBounds    clamp;
    }
    value       uniform (0 0 0);

or

Code:

myPatch
{
    type        solidTraction;
    tractionSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsTraction";
        outOfBounds    clamp;
    }
    pressureSeries
    {
        "file|fileName"    "$FOAM_CASE/constant/timeVsPressure";
        outOfBounds    clamp;
    }
    value       uniform (0 0 0);

where the timeVsTraction file looks like, for example:

Code:

(
    ( 0.   ( 0 0 0 ) )
    ( 1.5   ( 1e4 2e5 3e4 ) )
    ( 10.4  ( 4e4 5e4 5e5 ) )
)

and timeVsPressure like, for example:
the timeVsTraction file looks like, for example:

Code:

(
    ( 0.   0 )
    ( 1.5   -10.6e5 )
    ( 10.4  3e5 )
)

Thanks. I definitely got the idea. Now I am going to simulate a suction anchor with an external skirt (double bucket). According to the tutorial of suctioncassion, I built my geometry. But I am not pretty sure if it is correct since if I apply the traction on the structure-soil boundary, the inner and outer parts are separated without contact, which results in adding force two times on structure? Another question, once we add a force on structure, the load point is essential, as different locations lead to different torque?

bigphil · August 4, 2021, 10:33

If the structure is represented by a slender cavity, and you apply a traction to both sides of the cavity then yes each side will contribute to the force. In that case, you should just calculate the traction such that the total load will be correct.

Quote:

Another question, once we add a force on structure, the load point is essential, as different locations lead to different torque?

Sorry, I don't understand your question.

qi.yang@polimi.it · August 4, 2021, 10:47

Quote:

Originally Posted by bigphil

If the structure is represented by a slender cavity, and you apply a traction to both sides of the cavity then yes each side will contribute to the force. In that case, you should just calculate the traction such that the total load will be correct.

Sorry, I don't understand your question.

Thanks. In fact, the pressure force acts on the upper pile induced by wave, which could be applied traction on the interface of soil-structure, right? Imagine if the loading positions on the pile are different (e.g. F1, F2), resulting in different results since the torque is different due to the distance. I am confused that after I get the pressure exerted on the upper pile, how can I transform this force to the lower double-anchor part, coupling with soil?

bigphil · August 4, 2021, 11:22

OK I understand now.

In that case, you will need to set a traction distribution that balances the F1 and F2 loads as well as balances any moments that are generated.
There are probably many ways to do this, so starting with the easiest would make sense e.g. uniform traction.

You can print out the total force and total torque/moment on a patch using the solidForces and solidTorque function objects (place at the bottom of the controlDict inside a function dict/list)*:

Code:

forcesPatch1
{
    type   solidForces;
    historyPatch PATCH_NAME;
}
torquePatch1
{
    type   solidTorque;
    historyPatch PATCH_NAME;
    pointOnAxis "(0 0 0)";
    axisDirection "(0 1 0)";
}

* note: I only realised I never pushed the solidTorque functionObject so I have pushed it now (commit: 0f916163).

qi.yang@polimi.it · August 4, 2021, 11:42

Quote:

Originally Posted by bigphil

OK I understand now.

In that case, you will need to set a traction distribution that balances the F1 and F2 loads as well as balances any moments that are generated.
There are probably many ways to do this, so starting with the easiest would make sense e.g. uniform traction.

You can print out the total force and total torque/moment on a patch using the solidForces and solidTorque function objects (place at the bottom of the controlDict inside a function dict/list)*:

Code:

forcesPatch1
{
    type   solidForces;
    historyPatch PATCH_NAME;
}
torquePatch1
{
    type   solidTorque;
    historyPatch PATCH_NAME;
    pointOnAxis "(0 0 0)";
    axisDirection "(0 1 0)";
}

* note: I only realised I never pushed the solidTorque functionObject so I have pushed it now (commit: 0f916163).

Frankly, I did this step but I don't know how to apply those on the lower anchor part. When I simulate the anchor-soil interaction, the upper pipe was removed. Thus, where I can apply the force and moment? As you did in that tutorial, just import the force and torque on soil-structure interface?

bigphil · August 4, 2021, 11:46

Yes you will need to calculate the traction magnitude (and optionally the distribution) externally. The force and torque are then implicitly defined by the traction.

qi.yang@polimi.it · August 27, 2021, 07:05

Dear Prof.,

I found the porepressure was unchanged no matter which mechanistic model I selected. In the plot, poro M-C and poro linear Elastic models were considered. However, they are totally the same. In fact, the porepressure should be accumulated with time if elastoplastic M-C model was applied. What is your opinion on this issue?

bigphil · August 27, 2021, 07:29

Quote:

Originally Posted by qi.yang@polimi.it

Dear Prof.,

I found the porepressure was unchanged no matter which mechanistic model I selected. In the plot, poro M-C and poro linear Elastic models were considered. However, they are totally the same. In fact, the porepressure should be accumulated with time if elastoplastic M-C model was applied. What is your opinion on this issue?

That suggest that no plasticity is occurring i.e. if the stress are below the yield stress then elastoplastic and elastic laws are equivalent.

What are the Mohr-Coulomb parameters you used i.e. what is the approximate yield stress? The current pressures (a few hundred Pascals) may be far below this yield threshold. And so the results would be as expected.

qi.yang@polimi.it · August 31, 2021, 08:02

Quote:

Originally Posted by bigphil

That suggest that no plasticity is occurring i.e. if the stress are below the yield stress then elastoplastic and elastic laws are equivalent.

What are the Mohr-Coulomb parameters you used i.e. what is the approximate yield stress? The current pressures (a few hundred Pascals) may be far below this yield threshold. And so the results would be as expected.

Hi, Prof. Thanks. You are correct. After I reduced the cohesion, the soil was yielded. However, the pore pressure is so weird. I would like to know in the current model whether the yield and hardening law are considered. If so, where can I see and modify the relevant parameters? For example, elliptic cap parameters or hardening-related parameters.

bigphil · August 31, 2021, 08:23

This particular implementation of Mohr-Coulomb takes the following parameters:

Code:

        frictionAngle   frictionAngle [0 0 0 0 0 0 0] 30;
        dilationAngle   dilationAngle [0 0 0 0 0 0 0] 0;
        cohesion        cohesion [1 -1 -2 0 0 0 0] 1e5;

as described in https://onlinelibrary.wiley.com/doi/....1002/nag.2361.

qi.yang@polimi.it · August 31, 2021, 11:07

Quote:

Originally Posted by bigphil

This particular implementation of Mohr-Coulomb takes the following parameters:

Code:

        frictionAngle   frictionAngle [0 0 0 0 0 0 0] 30;
        dilationAngle   dilationAngle [0 0 0 0 0 0 0] 0;
        cohesion        cohesion [1 -1 -2 0 0 0 0] 1e5;

as described in https://onlinelibrary.wiley.com/doi/....1002/nag.2361.

I realized that in Tang's thesis, the cyclic poro-elasto-plasticity model was used to investiggate the accumulation of pore pressure in the seabed, instead of the current one I am using (poroElasticM-C). Is this possible reason that I could not obtain the expected results as shown in her thesis?

PHP Code:


			
[B]3.2.1 Critical state two-surface cyclic plasticity model
The adopted critical state two-surface cyclic plasticity model can effectively
reproduce cyclic stress-strain behaviors considering several important soil
features, such as phase transformation, critical state and peak failure, etc.
It involves more complicated formulations and a considerable amount of extra model parameters, compared to the previously discussed Mohr Coulomb
model. However, that is always the rule: the more soil features to predict,
the more complex soil constitutive model one tend to need.[/B]

Could we add the same mechanistic model similar to this one?https://bitbucket.org/tiantang/minig...PlastBiotFoam/

bigphil · September 1, 2021, 06:41

Quote:

Originally Posted by qi.yang@polimi.it

Could we add the same mechanistic model similar to this one?https://bitbucket.org/tiantang/minig...PlastBiotFoam/

Yes, it is possible to add this plasticity model.

The steps are:

Create a copy of an exisiting similar law, e.g.

Code:

$> cd solids4foam-release/src/solids4FoamModels/materialModels/mechanicalModel/mechanicalLaws/linearGeometryLaws 
$> cp -r poroAnisotropicBiotElastic poroTwoSurfaceBiot
$> cd poroTwoSurfaceBiot
$> mv poroAnisotropicBiotElastic.H poroTwoSurfaceBiot.H
$> mv poroAnisotropicBiotElastic.C poroTwoSurfaceBiot.C
$> sed -i "s/poroAnisotropicBiotElastic/poroTwoSurfaceBiot/g"

Add the new law to Make/options of solids4FoamModels and check it compiles:
Code:
```
$> wmake libso
```
Add to code from the twoSurfacePlasticity.H file to the correct function of the mechanical law (this should set the "sigma" stress tensor); and add any fields that need to be stored to the H file adn the constructor of the C file. In addition, you will need to read the material parameters within the constructor.
Compile it:
Code:
```
$> wmake libso
```

If this all works then you will be able to use it in a case.

Alternatively, feel free to add it as a feature request here: https://bitbucket.org/philip_cardiff...ew&status=open. Eventually I will get to it.

Philip

qi.yang@polimi.it · September 1, 2021, 07:04

Quote:

Originally Posted by bigphil

Yes, it is possible to add this plasticity model.

The steps are:

Create a copy of an exisiting similar law, e.g.

Code:

$> cd solids4foam-release/src/solids4FoamModels/materialModels/mechanicalModel/mechanicalLaws/linearGeometryLaws 
$> cp -r poroAnisotropicBiotElastic poroTwoSurfaceBiot
$> cd poroTwoSurfaceBiot
$> mv poroAnisotropicBiotElastic.H poroTwoSurfaceBiot.H
$> mv poroAnisotropicBiotElastic.C poroTwoSurfaceBiot.C
$> sed -i "s/poroAnisotropicBiotElastic/poroTwoSurfaceBiot/g"

Add the new law to Make/options of solids4FoamModels and check it compiles:
Code:
```
$> wmake libso
```
Add to code from the twoSurfacePlasticity.H file to the correct function of the mechanical law (this should set the "sigma" stress tensor); and add any fields that need to be stored to the H file adn the constructor of the C file. In addition, you will need to read the material parameters within the constructor.
Compile it:
Code:
```
$> wmake libso
```

If this all works then you will be able to use it in a case.

Alternatively, feel free to add it as a feature request here: https://bitbucket.org/philip_cardiff...ew&status=open. Eventually I will get to it.

Philip

Thanks a lot, Prof. Since those two codes were implemented in two versions of openfoam, I am not sure whether I can successfully compile it but I will make a try. Could you please also try to add it in parallel when you are available? Really thank you. In addition, I entered that request page and it said that I have no permission to access.

bigphil · September 1, 2021, 07:54

To add a feature request via an "issue", go to the public solids4foam bitbucket repository: https://bitbucket.org/philip_cardiff...se/src/master/. The click on "issues" on the left and create a new one.

July 21, 2021, 08:27		#21
bigphil Super Moderator Philip Cardiff Join Date: Mar 2009 Location: Dublin, Ireland Posts: 1,093 Rep Power: 34	The convergence seems ok to me. In this case, 5 residuals are written: resD: initial residual from the D equation resP: initial residual from the p equation relResD: alternative residual calculated as the max normlaisied difference between D and the previous iteration of D relResP: alternative residual calculated as the max normlaisied difference between p and the previous iteration of p matRes: residual from the mechanical law; in this case it is always 0 so this law does not define a residual The reason for the alternative residuals is that sometimes the equation initial residuals fail to show convergence even when the fields have stop changing (seems to be related to the choice of normalisation factor that is used), so solids4foam will assume convergence is achieved if any of the following conditions are met: if resD and resP and relResD and relResP are less than the specified solution tolerance if resD and resP are an order of magnitude less than the specified solution tolerance if relResD and relResP are an order of magnitude less than the specified solution tolerance In any case, you can always tighten the tolerance and see if the results change. As regards the displacement field, are you looking at the same component in both COMSOL and OpenFOAM? I cannot see the name of the component on the COMSOL image. And for the difference in rKprime, you can try change it and see what effect it has. Philip

August 4, 2021, 11:22		#30
bigphil Super Moderator Philip Cardiff Join Date: Mar 2009 Location: Dublin, Ireland Posts: 1,093 Rep Power: 34	OK I understand now. In that case, you will need to set a traction distribution that balances the F1 and F2 loads as well as balances any moments that are generated. There are probably many ways to do this, so starting with the easiest would make sense e.g. uniform traction. You can print out the total force and total torque/moment on a patch using the solidForces and solidTorque function objects (place at the bottom of the controlDict inside a function dict/list): Code: forcesPatch1 { type solidForces; historyPatch PATCH_NAME; } torquePatch1 { type solidTorque; historyPatch PATCH_NAME; pointOnAxis "(0 0 0)"; axisDirection "(0 1 0)"; } note: I only realised I never pushed the solidTorque functionObject so I have pushed it now (commit: 0f916163).

August 31, 2021, 08:23		#36
bigphil Super Moderator Philip Cardiff Join Date: Mar 2009 Location: Dublin, Ireland Posts: 1,093 Rep Power: 34	This particular implementation of Mohr-Coulomb takes the following parameters: Code: frictionAngle frictionAngle [0 0 0 0 0 0 0] 30; dilationAngle dilationAngle [0 0 0 0 0 0 0] 0; cohesion cohesion [1 -1 -2 0 0 0 0] 1e5; as described in https://onlinelibrary.wiley.com/doi/....1002/nag.2361.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
CGNS Boundary conditions using SU2	denzell	SU2	3	July 9, 2018 06:58
Wrong multiphase flow at rotating interface	Sanyo	CFX	14	February 7, 2017 18:19
Basic Nozzle-Expander Design	karmavatar	CFX	20	March 20, 2016 09:44
Question about heat transfer coefficient setting for CFX	Anna Tian	CFX	1	June 16, 2013 07:28
Low Mixing time Problem	Mavier	CFX	5	April 29, 2013 01:00

July 21, 2021, 09:20		#23
bigphil Super Moderator Philip Cardiff Join Date: Mar 2009 Location: Dublin, Ireland Posts: 1,093 Rep Power: 34	In COMSOL, the horizontal displacement at the surface (seabed surface) seems to be exactly zero. Is it possibly that the horizontal displacement on the surface is constrained to zero in COMSOL?

July 28, 2021, 06:48		#24
qi.yang@polimi.it Senior Member kimy Join Date: Mar 2019 Location: https://t.me/pump_upp Posts: 164 Rep Power: 7	Dear Prof., In order to consider the wave force exerted on the structure embedded on the seabed, it requires to implement a dynamic wave force on the structure thereby "timeVaryingTraction" boundary condition should be used, I think, which I found in Tangtian's source code and literature, like the similar condition used for implementing dynamic wave pressure on seabed by "timeVaryingAveragedValue". Thus, is it possible to add an additional boundary condition to achieve this goal? Thanks for your attention.

August 4, 2021, 11:46		#32
bigphil Super Moderator Philip Cardiff Join Date: Mar 2009 Location: Dublin, Ireland Posts: 1,093 Rep Power: 34	Yes you will need to calculate the traction magnitude (and optionally the distribution) externally. The force and torque are then implicitly defined by the traction.

September 1, 2021, 07:54		#40
bigphil Super Moderator Philip Cardiff Join Date: Mar 2009 Location: Dublin, Ireland Posts: 1,093 Rep Power: 34	To add a feature request via an "issue", go to the public solids4foam bitbucket repository: https://bitbucket.org/philip_cardiff...se/src/master/. The click on "issues" on the left and create a new one.