CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > OpenFOAM > OpenFOAM Programming & Development

tractionDisplacement BC for solidDisplacementFoam with Body Forces

Register Blogs Members List Search Today's Posts Mark Forums Read

Like Tree4Likes
  • 3 Post By bigphil
  • 1 Post By bigphil

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 13, 2012, 21:39
Default tractionDisplacement BC for solidDisplacementFoam with Body Forces
  #1
Senior Member
 
Hisham's Avatar
 
Hisham Elsafti
Join Date: Apr 2011
Location: Braunschweig, Germany
Posts: 257
Blog Entries: 10
Rep Power: 17
Hisham is on a distinguished road
Hi Foamers,

I need to add body forces to the solidDisplacementFoam solver. So it goes something similar to:
Code:
fvVectorMatrix DEqn
                (
                    fvm::d2dt2(D)
                 ==
                    fvm::laplacian(2*mu + lambda, D, "laplacian(DD,D)")
                  + bodyForces  
                  + divSigmaExp
                );
Where the bodyForces vectorField represents accelerations (e.g. gravity). Nevertheless, I have not found a reference on how to add a term to gradient() in tractionDisplacement boundary condition. I mean that for example a term for strain resulting from thermal stresses is added to the gradient() in tractionDisplacementFvPatchVectorField.C like:
Code:
gradient() =
    (
        (traction_ + pressure_*n)/rho
      + twoMuLambda*fvPatchField<vector>::snGrad() - (n & sigmaD)
    )/twoMuLambda;

 if (thermalStress)
    {
        ...

        gradient() += n*threeKalpha*T/twoMuLambda;
    }
I really appreciate any ideas or directions to references (or even how to do it )

Best regards,
Hisham El Safti
Hisham is offline   Reply With Quote

Old   April 14, 2012, 02:40
Default
  #2
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by Hisham View Post
Hi Foamers,

I need to add body forces to the solidDisplacementFoam solver. So it goes something similar to:
Code:
fvVectorMatrix DEqn
                (
                    fvm::d2dt2(D)
                 ==
                    fvm::laplacian(2*mu + lambda, D, "laplacian(DD,D)")
                  + bodyForces  
                  + divSigmaExp
                );
Where the bodyForces vectorField represents accelerations (e.g. gravity). Nevertheless, I have not found a reference on how to add a term to gradient() in tractionDisplacement boundary condition. I mean that for example a term for strain resulting from thermal stresses is added to the gradient() in tractionDisplacementFvPatchVectorField.C like:
Code:
gradient() =
    (
        (traction_ + pressure_*n)/rho
      + twoMuLambda*fvPatchField<vector>::snGrad() - (n & sigmaD)
    )/twoMuLambda;

 if (thermalStress)
    {
        ...

        gradient() += n*threeKalpha*T/twoMuLambda;
    }
I really appreciate any ideas or directions to references (or even how to do it )

Best regards,
Hisham El Safti
Hi Hisham,

Body forces act on the volume of each cell and are source terms so they do not have boundary conditions.

So to add a body force term, just add 'rho*g' to the momentum equation, where g is a dimensionedVector -9.81 in the y direction.

Philip
bigphil is offline   Reply With Quote

Old   April 14, 2012, 06:24
Default
  #3
Senior Member
 
Hisham's Avatar
 
Hisham Elsafti
Join Date: Apr 2011
Location: Braunschweig, Germany
Posts: 257
Blog Entries: 10
Rep Power: 17
Hisham is on a distinguished road
Hi Philip

Quote:
Originally Posted by bigphil View Post

Body forces act on the volume of each cell and are source terms so they do not have boundary conditions.

So to add a body force term, just add 'rho*g' to the momentum equation, where g is a dimensionedVector -9.81 in the y direction.

Philip
I agree with you that body forces do not need a BC for themselves but don't they contribute to displacement gradient at the boundary? I know that the boundary values can be retrieved from cells next to it.

I also have some other explicit terms that come from another variable (pore fluid velocity). They are all explicit terms (as the case of the "T" term in the DEqn in solidDisplacementFoam.C)
Code:
 if (thermalStress)
                {
                    const volScalarField& T = Tptr();
                    DEqn += fvc::grad(threeKalpha*T);
                }
So is the existence of a "T"-term added to the gradient() [at D's tractionDisplacement BC] due to the existence of a "T" BC or because "T" contributes to the displacement gradient?

Best regards,
Hisham
Hisham is offline   Reply With Quote

Old   April 14, 2012, 06:49
Default
  #4
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Hi Hisham,

The reason there is a T-term in the boundary condition is because T appears in the constitutive equation i.e. Hooke's law for a thermal elastic solid is:
sigma =2*mu*e +lambda*I*tr(e) - (2*mu + 3*lambda)*alpha*(T - Tref)*I

Therefore the traction on a boundary face is Trac = n . sigma, and then you sub in Hooke's law and rearrange this equation to get the equivalent (implicit) gradient on the boundary, which is what you set in the traction BC. So the traction BC will contain a T-term. But it will not contain any body force contributions.

If you add rho*g to the momentum equation then it will work, I ran a quick test case and everything is fine on the traction boundaries.

Philip
bigphil is offline   Reply With Quote

Old   April 14, 2012, 07:03
Default
  #5
Senior Member
 
Hisham's Avatar
 
Hisham Elsafti
Join Date: Apr 2011
Location: Braunschweig, Germany
Posts: 257
Blog Entries: 10
Rep Power: 17
Hisham is on a distinguished road
Hi Philip

Thanks a lot for your help! Now it is clear to me

Best regards
Hisham
Hisham is offline   Reply With Quote

Old   April 29, 2013, 13:26
Default
  #6
Member
 
Samer
Join Date: Jan 2013
Posts: 31
Rep Power: 13
SamerAli is on a distinguished road
Hi Philip

using the same methodology, if simulation fluid-structure interaction problem, and i want to transfer the temperature computed at the wall of a solid, as boundary condition for the fluid part (where there is a common patch between fluid and solid) ??

Best regards
SamerAli is offline   Reply With Quote

Old   April 30, 2013, 16:27
Default
  #7
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by SamerAli View Post
Hi Philip

using the same methodology, if simulation fluid-structure interaction problem, and i want to transfer the temperature computed at the wall of a solid, as boundary condition for the fluid part (where there is a common patch between fluid and solid) ??

Best regards
Hi Samer,

yes you can follow the same Dirichlet-Neumann coupling procedure to couple the temperature between the regions.

Philip
bigphil is offline   Reply With Quote

Old   November 17, 2017, 09:27
Default
  #8
Member
 
Join Date: Sep 2016
Posts: 63
Rep Power: 9
sitajeje is on a distinguished road
Hello Philip,

Thank you very much first of all for your solvers in solidMechanics incorporated in foam-extend!

I want to do a stress analysis of a fan with a certain rotation speed. The material remain elastic and I assume Newtonian properties. I wonder which solver can implement the centrifugal force please? I am new for your solvers. I checked through your solvers, but did't figure it out.

Thank you very much in advance!

Best regards,
sitajeje
sitajeje is offline   Reply With Quote

Old   January 9, 2018, 13:20
Default
  #9
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by sitajeje View Post
Hello Philip,

Thank you very much first of all for your solvers in solidMechanics incorporated in foam-extend!

I want to do a stress analysis of a fan with a certain rotation speed. The material remain elastic and I assume Newtonian properties. I wonder which solver can implement the centrifugal force please? I am new for your solvers. I checked through your solvers, but did't figure it out.

Thank you very much in advance!

Best regards,
sitajeje
Hi sitajeje,

To include a body force, you just need to add this term to the momentum equation in the solver. For example, in elasticSolidFoam the momentum equation would become (on line 93 of elasticSolidFoam.C):
Code:
            fvVectorMatrix UEqn
            (
             	rho*fvm::d2dt2(U)
          ==	fvm::laplacian(2*muf + lambdaf, U, "laplacian(DU,U)")
              + divSigmaExp
              + rho*g
              + rho*magSqr(v)/r      // centrifugal force per unit volume
            );
where you would need to define your velocity volVectorField "v" and the radial distance field "r". You could read these fields from the case.

Philip
bigphil is offline   Reply With Quote

Old   January 9, 2018, 13:38
Default
  #10
Member
 
Join Date: Sep 2016
Posts: 63
Rep Power: 9
sitajeje is on a distinguished road
Thank you very much Philip!

I get it done by myself, and my programming is improved a little. Thank you all the same!

I have another question please, and I cannot figure it out until now. It would be very helpful if you could give me a suggestion. I wonder how to map the pressure field of the fan blades from results of pimpleDyMFoam to solidDisplacementFoam please? I did mapFields, but "p" is mapped to "p", and didn't effect. How can I map "p" to the "p" in the "tractionDisplacement" boundary condition in the "D" file please? I want to calculate the stress induced by the aerodynamic pressure.

Thank you very much in advance!

Best regards,
sitajeje
sitajeje is offline   Reply With Quote

Old   January 25, 2018, 07:41
Default
  #11
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Hi sitajeje,

mapFields is used to map from one domain to another domain that overlaps the original domain in some way e.g. see cavityClipped case in the documentation; however, it does not map (as far as I know) from a patch on one domain to a patch on another domain, where the patches overlap but the domains do not.

So in this case, you need to use the functionality provided by classes like patchToPatchInterpolation or GGIInterpolation (foam-extend) or AMIInterpolation (Foundation and ESI forks).

If you send me a PM with your email, I have some code that may work for you.

Philip
bigphil is offline   Reply With Quote

Old   February 15, 2018, 15:19
Default
  #12
New Member
 
Florida
Join Date: Feb 2018
Location: Florida
Posts: 12
Rep Power: 8
shinjanghosh is on a distinguished road
Quote:
Originally Posted by bigphil View Post
Hi sitajeje,

To include a body force, you just need to add this term to the momentum equation in the solver. For example, in elasticSolidFoam the momentum equation would become (on line 93 of elasticSolidFoam.C):
Code:
            fvVectorMatrix UEqn
            (
             	rho*fvm::d2dt2(U)
          ==	fvm::laplacian(2*muf + lambdaf, U, "laplacian(DU,U)")
              + divSigmaExp
              + rho*g
              + rho*magSqr(v)/r      // centrifugal force per unit volume
            );
where you would need to define your velocity volVectorField "v" and the radial distance field "r". You could read these fields from the case.

Philip
Hello Philip,
I was trying to introduce the body force as a centrifugal force per unit volume in a beam like the example you gave. However I am having trouble introducing the radius vector by reading it from the mesh(which is the z coordinate of the cell center of each cell in my mesh). Please help. Thanks.
shinjanghosh is offline   Reply With Quote

Old   February 16, 2018, 04:44
Default
  #13
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Hello shinjanghosh,

What is your problem? You will need to give more information if you want someone to help you.

Also, looking back on the body force term I suggested above, the dimensions are wrong: it should be a vector not a scalar; the following makes more sense:
Code:
        + rho*(magSqr(v)/mag(R))*(R/mag(R))
where R is the radial volVectorField, which could be calculated as:
Code:
// Points on the axis
const vector pointOnAxis1(0, 0, 0);
const vector pointOnAxis2(1, 0, 0);

// Axis unit direction vector
const vector axisDir = (pointOnAxis1 - pointOnAxis2)/mag(pointOnAxis1 - pointOnAxis2);

// Radial vector field: it only has a component in the radial direction
const volVectorField R
(
    "R",
    (I - sqr(axisDir)) & (mesh.C() - pointOnAxis1)
)
Philip
bigphil is offline   Reply With Quote

Old   February 16, 2018, 13:51
Default
  #14
New Member
 
Florida
Join Date: Feb 2018
Location: Florida
Posts: 12
Rep Power: 8
shinjanghosh is on a distinguished road
Hello Philip,

Thanks for the reply. Sorry for the inconvenience.

My problem :

Calculation of solid stresses in a hollow beam with a circular cross section(basically a pipe with a finite wall thickness) which rotates at a rpm of 3600.

the length of the pipe is along the 'z-axis' and it's axis of rotation is the x axis.

I figured out the boundary conditions (fixed end cantilever beam) and did a simple end load condition simulation solution (without any rotation) using solidDisplacementFoam. Then I started having problems adding the body forces inside the vector equation when I decided to include the rotation. I tried hard-coding the body force in the solver itself like you suggested in one of your previous replies.

Here's where I had issues :

1.) Reading the cell-center values for calculation of 'R' vector. In my case it is the z component of the cell center.

2.) Specifying it as a vector.


Thanks,
Shinjan
shinjanghosh is offline   Reply With Quote

Old   February 19, 2018, 07:23
Default
  #15
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Hi Shinjan,

As the x-axis is your axis of rotation, the updated code I suggested in my previous post should work for you.

If you have issues with compilation of running, you can post them here.

Philip
bigphil is offline   Reply With Quote

Old   February 19, 2018, 13:09
Default
  #16
New Member
 
Florida
Join Date: Feb 2018
Location: Florida
Posts: 12
Rep Power: 8
shinjanghosh is on a distinguished road
Hey Philip,

The compilation didn't give any errrors, but I encountered the following errors while running the solver :



----------------------------------------------------------------------------------------------
--> FOAM FATAL ERROR:
LHS and RHS of - have different dimensions
dimensions : [0 1 0 0 0 0 0] - [0 0 0 0 0 0 0]


From function Foam::dimensionSet Foam:perator-(const Foam::dimensionSet&, const Foam::dimensionSet&)
in file dimensionSet/dimensionSet.C at line 521.

FOAM aborting

Generating stack trace...
--------------------------------------------------------------------------------------------------

From what I understood, It has to be a dimension mismatch regarding subtracting a vector which is dimensionless, from one which has length as it's dimension.

I think the error came from here :

const volVectorField R
(
"R",
(I - sqr(axisDir)) & (mesh.C() - pointOnAxis1)
);
shinjanghosh is offline   Reply With Quote

Old   February 20, 2018, 06:56
Default
  #17
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Hi Shinjan,

The pointOnAxis1, pointOnAxis2 and aixsDir should be dimensionedVector instead of vector: try make the changes below:
Code:
// Points on the axis
const dimensionedVector pointOnAxis1("pointOnAxis1", dimLength, vector(0, 0, 0));
const dimensionedVector pointOnAxis2("pointOnAxis2", dimLength, vector(1, 0, 0));

// Axis unit direction vector
const dimensionedVector axisDir = (pointOnAxis1 - pointOnAxis2)/mag(pointOnAxis1 - pointOnAxis2);

// Radial vector field: it only has a component in the radial direction
const volVectorField R
(
    "R",
    (I - sqr(axisDir)) & (mesh.C() - pointOnAxis1)
)
Philip
bigphil is offline   Reply With Quote

Old   March 27, 2018, 13:28
Default
  #18
New Member
 
Dmitry
Join Date: Dec 2016
Location: Leoben, Austria
Posts: 1
Rep Power: 0
parnumeric is on a distinguished road
Quote:
Originally Posted by bigphil View Post
Hi sitajeje,

mapFields is used to map from one domain to another domain that overlaps the original domain in some way e.g. see cavityClipped case in the documentation; however, it does not map (as far as I know) from a patch on one domain to a patch on another domain, where the patches overlap but the domains do not.

So in this case, you need to use the functionality provided by classes like patchToPatchInterpolation or GGIInterpolation (foam-extend) or AMIInterpolation (Foundation and ESI forks).

If you send me a PM with your email, I have some code that may work for you.

Philip
Hello Philip, hi sitajeje and Foamers,

I'm also as sitajeje interested in mapping "p" from one region (calculated in fluid) to another (solid). I'm doing a steady-state heat transfer simulation using one of multiregion solvers (I've modified one from chtMultiRegionSimpleFoam for my purpose) and now I'm interested in stresses in the solid region. I've copied the last time step of the solid region from my multiregion simulation, added a "D" file and I wanted to simply run a one-region simulation on it using the "solidDisplacementFoam" solver. My question is how I correctly set pressure in the "tractionDisplacement" boundary condition which is, from my understanding, the pressure field on the interface between the fluid and solid regions in my previous simulation. However, the boundary condition for "p" in fluid was set as "type zeroGradient" (initially I expected to see a non-uniform list which I wanted to simply copy in the "D file" for the pressure field instead of "uniform 0").

I'm wondering whether Philip's answer (using patchToPatchInterpolation or GGIInterpolation or AMIInterpolation) is the right direction for me or there is a simpler solution. I'm using OpenFOAM 2.4.0.

Best regards,
Dmitry
parnumeric is offline   Reply With Quote

Old   March 29, 2018, 04:32
Default
  #19
Super Moderator
 
bigphil's Avatar
 
Philip Cardiff
Join Date: Mar 2009
Location: Dublin, Ireland
Posts: 1,089
Rep Power: 34
bigphil will become famous soon enoughbigphil will become famous soon enough
Quote:
Originally Posted by parnumeric View Post
Hello Philip, hi sitajeje and Foamers,

I'm also as sitajeje interested in mapping "p" from one region (calculated in fluid) to another (solid). I'm doing a steady-state heat transfer simulation using one of multiregion solvers (I've modified one from chtMultiRegionSimpleFoam for my purpose) and now I'm interested in stresses in the solid region. I've copied the last time step of the solid region from my multiregion simulation, added a "D" file and I wanted to simply run a one-region simulation on it using the "solidDisplacementFoam" solver. My question is how I correctly set pressure in the "tractionDisplacement" boundary condition which is, from my understanding, the pressure field on the interface between the fluid and solid regions in my previous simulation. However, the boundary condition for "p" in fluid was set as "type zeroGradient" (initially I expected to see a non-uniform list which I wanted to simply copy in the "D file" for the pressure field instead of "uniform 0").

I'm wondering whether Philip's answer (using patchToPatchInterpolation or GGIInterpolation or AMIInterpolation) is the right direction for me or there is a simpler solution. I'm using OpenFOAM 2.4.0.

Best regards,
Dmitry
Hi Dmitry,

From my understanding of your case, it should be possible to explicitly interpolate fields using patchToPatchInterpolation/GGIInterpolation/AMIInterpolation.

However, be careful with "pressure" in the tractionDisplacement specification: here pressure is the surface normal component of the wall traction vector, this is not the same (in general) as the hydrostatic pressure (i.e. "p" in the fluid solver). So you should reconstruct the total stress/traction vector on the fluid side and interpolate this across to the solid side (tractionDisplacement).

Philip
parnumeric likes this.
bigphil is offline   Reply With Quote

Reply

Tags
bodyforces, soliddisplacementfoam, tractiondisplacement

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
DPM body force to express electric forces adam14qin FLUENT 24 August 1, 2013 13:34
Body forces on hovering airfoil sanmysterio Main CFD Forum 1 July 13, 2010 03:14
Fan modelling using body forces Fred Siemens 2 June 13, 2007 08:56
strong body forces Ankan Main CFD Forum 0 August 2, 2005 02:13
Body Forces Thomas P. Abraham Main CFD Forum 1 April 21, 1999 21:24


All times are GMT -4. The time now is 19:37.