SimLab CFD Analysis: Solution doesn't converge

Alberto Sardi

Hi,

I'm new in SimLab 2023. 

I would like to know why my solution does not converge.

My problem is a simple cube placed inside a square section tube with air flowing through it and analyzed with laminar flow.
I followed these steps:
1) creation of the fluid via the "Domain" ribbon;
2) Creation of the cavity in the fluid, due to the presence of the cube, via the Connect Combine ribbon;
3) Surface Mesh of all bodies;
4) CFD mesh of the fluid body, designating the surfaces on which not to create the Boundary Layer and designating the solid bodies;
5) Designation of Inlet, Outlet and Wall with the corresponding ribbons;
6) Designation of the boundary conditions of velocity, pressure and temperature;
7) Update on Results.
The solution converges only for the velocity and pressure parameters, but the temperature does not converge.
Can someone help me?

Thank you in advance.

 

Marc_21384

Alberto Sardi said:

Hi Marc,

attached you find the SimLab file.

Yes, this is the problem, adding on the outer surface also the insulating.

I solved the thermal flow introducing Interface Surface between air and the other solid parts.

Does it make sense?

Hi Alberto,

Yes, that makes sense. My recommendation would be, you're already using parasolid (CAD). You can use the boolean tool to combine them all, just make sure you have "Create connected bodies" option enabled. Then you can do your surface mesh, select the mesh created and do right click -> unmerge, this will give you back your original assembly. Now you can continue with the rest without using Interface Surface.

The boolean tool will make sure you have shared faces/mesh between your bodies, which is the best way to work with. Hopefully this helps out.

Have a great week,

Marc

acupro

Can you attach the input (.inp) and Log (.Log) files from the run?  What are your thermal boundary conditions?  Assume you have defined a temperature at the inlet - but what do you have on the boundaries of the tube, and on the cube boundaries (or solid)?

Marc_21384

Hi Alberto,

On your Wall BC have you assigned a correct convective value?

acupro

Marc_21384 said:

Hi Alberto,

On your Wall BC have you assigned a correct convective value?

Kind of the same questions I had.  If there's nothing in the model to cause any temperature differences/gradients - it will essentially just be a constant temperature solution.  Is there a heat source or surface heat flux on the internal box?  Is there some temperature or flux condition on the outer tube walls?  Etc.

Alberto Sardi

acupro_21778 said:

Can you attach the input (.inp) and Log (.Log) files from the run?  What are your thermal boundary conditions?  Assume you have defined a temperature at the inlet - but what do you have on the boundaries of the tube, and on the cube boundaries (or solid)?

Hi acupro,

attached you find the file log. 

Thermal boundary conditions are:

1-"Heat source" on the cube, and I assinged it like a "Heat source on each body";

2-"Inlet" has both velocity (0.26 m/s) and temperature (0°C).

 

On the boundaries of tube and cube I put only "Wall", selecting corrisponding surfaces and for the "Wall velocity" i chose the type "Match Mesh Velocity" and for "Thermal" I chose the type "None".

Alberto Sardi

Marc_21384 said:

Hi Alberto,

On your Wall BC have you assigned a correct convective value?

Hi Marc,

on the Wall ribbon I chose in "Thermal" section the type "None" and for "Wall Velocity" I chose the type "Match Mesh Velocity".

 

Wall BC was assigned to inner surfaces of the tube and for the outer surfaces of the cube.

A "Heat Source" was assigned to the cube with "Heat source on each body".

Other BCs are:

-inlet, specifying velocity and temperature;

-outlet, specifying only static pressure.

Marc_21384

Alberto Sardi said:

Hi Marc,

on the Wall ribbon I chose in "Thermal" section the type "None" and for "Wall Velocity" I chose the type "Match Mesh Velocity".

 

Wall BC was assigned to inner surfaces of the tube and for the outer surfaces of the cube.

A "Heat Source" was assigned to the cube with "Heat source on each body".

Other BCs are:

-inlet, specifying velocity and temperature;

-outlet, specifying only static pressure.

Hi Alberto,

Can you share the inp file? If I understood correctly, something like this you are modelling: 

Where you have adiabatic walls, but there's a heat source inside the fluid, right?

Kind regards,

Marc

acupro

Alberto Sardi said:

Hi acupro,

attached you find the file log. 

Thermal boundary conditions are:

1-"Heat source" on the cube, and I assinged it like a "Heat source on each body";

2-"Inlet" has both velocity (0.26 m/s) and temperature (0°C).

 

On the boundaries of tube and cube I put only "Wall", selecting corrisponding surfaces and for the "Wall velocity" i chose the type "Match Mesh Velocity" and for "Thermal" I chose the type "None".

Some things I see from the Log file:

acuPrep:          Minimum coordinates = -7.5000e-03 -7.5000e-03 -1.0000e-02
acuPrep:          Maximum coordinates =  7.5000e-03  7.5000e-03  1.0000e-02
acuPrep:                   Dimensions =  1.5000e-02  1.5000e-02  2.0000e-02
acuPrep:                  Total nodes =       8156
acuPrep:               Total elements =      36722

Are the model dimensions correct?  This is very small, assuming distances are in meters.  Also there's not much mesh - only 8000 nodes.  Have you used boundary layer meshing from the walls - to capture the flow/thermal profiles near the walls?  I notice the flow is 'converging' very well - but thermal is not.  This is also likely due to the lack of mesh - very difficult to resolve what's actually happening with not much mesh.  If there is a blockage in the flow - it's also quite likely to be transient, with vortex shedding, etc - and more mesh will capture that, too.

I suggest you look at refining the mesh.

That being said - there's also this in the Log file - at the end:

acuTrans:  Variable                         Min           Max           Ave
acuTrans: x_coordinates                  -7.500000e-03  7.500000e-03  3.365293e-06
acuTrans: y_coordinates                  -7.500000e-03  7.500000e-03  2.683025e-05
acuTrans: z_coordinates                  -1.000000e-02  1.000000e-02  7.357848e-06
acuTrans: x_velocity                     -2.107209e-01  1.988981e-01 -1.244213e-04
acuTrans: y_velocity                     -1.865665e-01  1.938669e-01 -1.222682e-04
acuTrans: z_velocity                     -5.085958e-01  5.026934e-02 -9.856034e-02
acuTrans: pressure                       -1.528366e-01  4.104723e-01  4.896650e-02
acuTrans: temperature                     2.681050e+02  1.125299e+11  2.787033e+09

Temperature is going very high.  Again - could be problem setup or lack of mesh.  Could you attach your SimLab database?  Or at least the input file?

Alberto Sardi

acupro_21778 said:

Some things I see from the Log file:

acuPrep:          Minimum coordinates = -7.5000e-03 -7.5000e-03 -1.0000e-02
acuPrep:          Maximum coordinates =  7.5000e-03  7.5000e-03  1.0000e-02
acuPrep:                   Dimensions =  1.5000e-02  1.5000e-02  2.0000e-02
acuPrep:                  Total nodes =       8156
acuPrep:               Total elements =      36722

Are the model dimensions correct?  This is very small, assuming distances are in meters.  Also there's not much mesh - only 8000 nodes.  Have you used boundary layer meshing from the walls - to capture the flow/thermal profiles near the walls?  I notice the flow is 'converging' very well - but thermal is not.  This is also likely due to the lack of mesh - very difficult to resolve what's actually happening with not much mesh.  If there is a blockage in the flow - it's also quite likely to be transient, with vortex shedding, etc - and more mesh will capture that, too.

I suggest you look at refining the mesh.

That being said - there's also this in the Log file - at the end:

acuTrans:  Variable                         Min           Max           Ave
acuTrans: x_coordinates                  -7.500000e-03  7.500000e-03  3.365293e-06
acuTrans: y_coordinates                  -7.500000e-03  7.500000e-03  2.683025e-05
acuTrans: z_coordinates                  -1.000000e-02  1.000000e-02  7.357848e-06
acuTrans: x_velocity                     -2.107209e-01  1.988981e-01 -1.244213e-04
acuTrans: y_velocity                     -1.865665e-01  1.938669e-01 -1.222682e-04
acuTrans: z_velocity                     -5.085958e-01  5.026934e-02 -9.856034e-02
acuTrans: pressure                       -1.528366e-01  4.104723e-01  4.896650e-02
acuTrans: temperature                     2.681050e+02  1.125299e+11  2.787033e+09

Temperature is going very high.  Again - could be problem setup or lack of mesh.  Could you attach your SimLab database?  Or at least the input file?

Hi acupro,

attached you find the SimLab file.

I solved the Thermal Flow problem introducing Interface Surface between air and the other solid parts.

Does it make sense?

Alberto Sardi

Marc_21384 said:

Hi Alberto,

Can you share the inp file? If I understood correctly, something like this you are modelling: 

Where you have adiabatic walls, but there's a heat source inside the fluid, right?

Kind regards,

Marc

Hi Marc,

attached you find the SimLab file.

Yes, this is the problem, adding on the outer surface also the insulating.

I solved the thermal flow introducing Interface Surface between air and the other solid parts.

Does it make sense?

Marc_21384

Alberto Sardi said:

Hi Marc,

attached you find the SimLab file.

Yes, this is the problem, adding on the outer surface also the insulating.

I solved the thermal flow introducing Interface Surface between air and the other solid parts.

Does it make sense?

Hi Alberto,

Yes, that makes sense. My recommendation would be, you're already using parasolid (CAD). You can use the boolean tool to combine them all, just make sure you have "Create connected bodies" option enabled. Then you can do your surface mesh, select the mesh created and do right click -> unmerge, this will give you back your original assembly. Now you can continue with the rest without using Interface Surface.

The boolean tool will make sure you have shared faces/mesh between your bodies, which is the best way to work with. Hopefully this helps out.

Have a great week,

Marc

Alberto Sardi

Marc_21384 said:

Hi Alberto,

Yes, that makes sense. My recommendation would be, you're already using parasolid (CAD). You can use the boolean tool to combine them all, just make sure you have "Create connected bodies" option enabled. Then you can do your surface mesh, select the mesh created and do right click -> unmerge, this will give you back your original assembly. Now you can continue with the rest without using Interface Surface.

The boolean tool will make sure you have shared faces/mesh between your bodies, which is the best way to work with. Hopefully this helps out.

Have a great week,

Marc

Thank you so much Marc, you have been so helpful.

Have a great week you too,

kind regards,

Alberto