Non-isothermal flow, thermal expansion and structural mechanics

Please login with a confirmed email address before reporting spam

Dear Comsol experts,

I have a project where I simulate the cooling of a polymer part in a steel mold that is cooled by water (injection molding). The mold is initially at the same temperature as the cooling fluid and the polymer part is well above that (about 200K).

I am interested in the dynamics of the cooling process as well as the occuring thermal stresses due to the temperature gradients within the mold and the polymer part. Furthermore, I like to check on the influence of thermal expansion on the flow of the cooling liquid (expansion or contraction of the flow channel due to expansion/contraction of the surrounding material) and the heat transfer of the polymer part (loss of wall contact due to shrinkage).

My question is wether or not I can couple these three physics and obviously in what way I can do it, if it is possible. If it is possible, maybe there is a tutorial that I didn't find yet. Up to now I only found tutorials for thermal stress and heat transfer and conjugate heat transfer, respectively.

Any help or recommendation on where to start is greatly appreciated.

Best regards, André

PS: Also I attached a 2D primitive sketch of the geometry with basic process parameters. The original 3D geometry is rather complex with small geometric features so I thought I start simple to familiarize myself with the necesseary model set up.



10 Replies Last Post 14 juni 2019 10:10 GMT−4

Please login with a confirmed email address before reporting spam

Posted: 2 weeks ago 31 maj 2019 17:41 GMT−4
Updated: 2 weeks ago 31 maj 2019 17:39 GMT−4

Yes, this can be done. I had a similar problem, and I also was quite surprised that an example problem of thermal expansion coupled with changes in heating/cooling flow geometry was not available (at least that I could find) in the application library. If you "turn on thermal expansion" in the structural mechanics, it will enable the "moving mesh" feature of COMSOL. The moving mesh then becomes the new boundary for the cooling flow. It is quite tricky and causes a considerable amount of nonlinear behaviour to the solution, but it does work. You can look at the FSI module which is similar, but instead of thermal expansion, it is using the movement of the structure by other means (not thermal expansion). The fluid flow, in my case, and I believe in yours as you describe it, is not sufficient to alter the structure, but the structure is altering the geometry of the fluid through thermal expansion, It is a very common problem, and needs to be included in the COMSOL application library.

-------------------
James D. Freels, Ph.D., P.E.
Yes, this can be done. I had a similar problem, and I also was quite surprised that an example problem of thermal expansion coupled with changes in heating/cooling flow geometry was not available (at least that I could find) in the application library. If you "turn on thermal expansion" in the structural mechanics, it will enable the "moving mesh" feature of COMSOL. The moving mesh then becomes the new boundary for the cooling flow. It is quite tricky and causes a considerable amount of nonlinear behaviour to the solution, but it does work. You can look at the FSI module which is similar, but instead of thermal expansion, it is using the movement of the structure by other means (not thermal expansion). The fluid flow, in my case, and I believe in yours as you describe it, is not sufficient to alter the structure, but the structure is altering the geometry of the fluid through thermal expansion, It is a very common problem, and needs to be included in the COMSOL application library.

Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 5 days ago 10 juni 2019 06:01 GMT−4
Updated: 5 days ago 10 juni 2019 06:01 GMT−4

Hi,

Changes in flow duct geometry due to thermal expansion is usually small, say an area change of 1% for a temperature difference of 200 K. The change in viscosity of the fluid will be much larger than that, and be the dominant effect in most cases. There could however be cases where large overall structural deformations caused by thermal expansion affect the geometry of a thin channel to significant degree.

Whether the deformation of the structure is caused by thermal or other effects is not important to the problem. When using FSI you select in which domains to use moving mesh, and all such domains have their shapes controlled by the structural deformations in the adjacent domains.

FSI, heat transfer, and thermal expansion should work seamlessly together. There are several possible entry points because of the multiphysics involved. In either case, you need to add some of the multiphysics couplings manually.

Maybe the most natural starting point is to start by adding Fluid-Structure Interaction. Then continue by adding the Heat Transfer in Solids and Heat Transfer in Fluids physics interfaces to the appropriate domain. Finally, the multiphysics couplings Nonisothermal Flow, Thermal Expansion, and Temperature Coupling must then added manually to the model.

There are many possible combinations of bidirectional and unidirectional couplings in a problem like this. This will strongly affect the optimal solver strategy.

@Jim - I do not understand what you refer to with the statement "If you "turn on thermal expansion" in the structural mechanics, it will enable the "moving mesh" feature".

Regards,
Henrik

Hi, Changes in flow duct geometry due to thermal expansion is usually small, say an area change of 1% for a temperature difference of 200 K. The change in viscosity of the fluid will be much larger than that, and be the dominant effect in most cases. There could however be cases where large overall structural deformations caused by thermal expansion affect the geometry of a thin channel to significant degree. Whether the deformation of the structure is caused by thermal or other effects is not important to the problem. When using FSI you select in which domains to use moving mesh, and all such domains have their shapes controlled by the structural deformations in the adjacent domains. FSI, heat transfer, and thermal expansion should work seamlessly together. There are several possible entry points because of the multiphysics involved. In either case, you need to add some of the multiphysics couplings manually. Maybe the most natural starting point is to start by adding **Fluid-Structure Interaction**. Then continue by adding the **Heat Transfer in Solids** and **Heat Transfer in Fluids** physics interfaces to the appropriate domain. Finally, the multiphysics couplings **Nonisothermal Flow**, **Thermal Expansion**, and **Temperature Coupling** must then added manually to the model. There are many possible combinations of bidirectional and unidirectional couplings in a problem like this. This will strongly affect the optimal solver strategy. @Jim - I do not understand what you refer to with the statement "If you "turn on thermal expansion" in the structural mechanics, it will enable the "moving mesh" feature". Regards, Henrik

Please login with a confirmed email address before reporting spam

Posted: 5 days ago 11 juni 2019 03:40 GMT−4

Dear Jim and Henrik,

thanks first for your insightful replies and an apology for my late reply. I got sick and just returned to work today.

I will try your to implement your suggestions as soon as there is time and let you know wether or not they worked.

Also I thought that this sort of problem is quite common, so maybe Comsol can add an example to the model library.

Thanks again and best regards, André

Dear Jim and Henrik, thanks first for your insightful replies and an apology for my late reply. I got sick and just returned to work today. I will try your to implement your suggestions as soon as there is time and let you know wether or not they worked. Also I thought that this sort of problem is quite common, so maybe Comsol can add an example to the model library. Thanks again and best regards, André

Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 4 days ago 11 juni 2019 10:58 GMT−4

Hi Andre,

Providing an example of coupled FSI-Thermal analysis is a good idea. We will create a simplistic such example and upload it to the Application Gallery within a few days.

Stay tuned. We will post a message in this thread when it is available.

By the way, there are other complications in your model too: The possible loss of wall contact between the plastic and the mold. As long as the plastic can be modeled using Solid Mechanics, this is feasible (it is 'just' a contact problem), but if the plastic is initially a fluid which through a phase change is converted into a solid, then the problem is much more difficult.

Regards,
Henrik

Hi Andre, Providing an example of coupled FSI-Thermal analysis is a good idea. We will create a simplistic such example and upload it to the Application Gallery within a few days. Stay tuned. We will post a message in this thread when it is available. By the way, there are other complications in your model too: The possible loss of wall contact between the plastic and the mold. As long as the plastic can be modeled using Solid Mechanics, this is feasible (it is 'just' a contact problem), but if the plastic is initially a fluid which through a phase change is converted into a solid, then the problem is much more difficult. Regards, Henrik

Please login with a confirmed email address before reporting spam

Posted: 4 days ago 12 juni 2019 05:20 GMT−4
Updated: 4 days ago 12 juni 2019 05:22 GMT−4

Dear Henrik,

first of all I tried to implement your and Jims suggestions. However, I ran into some problems regarding the contact between the mold and the plastic part.

Secondly, thanks for your efforts in providing an example and your additional information.

Regarding your comment: The plastic initially is a fluid. However, since the plastic is solid close to the wall due to the low temperature of the mold and since the properties do not vary to much between solid and liquid state, I assumed the entire plastic part to be solid as a starting point.

As you pointed out, I do have a contact problem. This means, that I need to form the geometry in assembly mode. (This is what I understand from the manual.) By choosing assembly mode, Comsol automatically creates contact pairs, which also include those for the contact between the fluid domain and the solid mold. In this configuration neither FSI nor FSI (Pair) multiphysics will recognize the respective boundaries as valid and indicate that the boundary condition is not applicable.

Furthermore, I included gravity as a body force. Otherwise due to contact loss there wouldn't be any heat transfer. However, the plastic part moves right through the mold when I try it. I guess there is something wrong with my contact boundary condition. For implementation of the contact boundary condition I followed a video presentation (indentation test, halfsphere steel and rubber) from the Comsol website.

And finally, actually there is no heat transfer between the plastic part and the mold. I added a pair thermal contact node to the ht-interface and also added the temperature coupling and thermal expansion to the Multiphysics-Node. However, there is absolutely no change in temperature. Du I need to imlement the boundary condition differently?

Thanks again for your support and advice. I greatly appreciate it.

Best regards, André

PS: I guess I'll just wait for the example. This should clarify at least some of my questions.

Dear Henrik, first of all I tried to implement your and Jims suggestions. However, I ran into some problems regarding the contact between the mold and the plastic part. Secondly, thanks for your efforts in providing an example and your additional information. Regarding your comment: The plastic initially is a fluid. However, since the plastic is solid close to the wall due to the low temperature of the mold and since the properties do not vary to much between solid and liquid state, I assumed the entire plastic part to be solid as a starting point. As you pointed out, I do have a contact problem. This means, that I need to form the geometry in assembly mode. (This is what I understand from the manual.) By choosing assembly mode, Comsol automatically creates contact pairs, which also include those for the contact between the fluid domain and the solid mold. In this configuration neither FSI nor FSI (Pair) multiphysics will recognize the respective boundaries as valid and indicate that the boundary condition is not applicable. Furthermore, I included gravity as a body force. Otherwise due to contact loss there wouldn't be any heat transfer. However, the plastic part moves right through the mold when I try it. I guess there is something wrong with my contact boundary condition. For implementation of the contact boundary condition I followed a video presentation (indentation test, halfsphere steel and rubber) from the Comsol website. And finally, actually there is no heat transfer between the plastic part and the mold. I added a pair thermal contact node to the ht-interface and also added the temperature coupling and thermal expansion to the Multiphysics-Node. However, there is absolutely no change in temperature. Du I need to imlement the boundary condition differently? Thanks again for your support and advice. I greatly appreciate it. Best regards, André PS: I guess I'll just wait for the example. This should clarify at least some of my questions.

Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 3 days ago 12 juni 2019 10:30 GMT−4
Updated: 3 days ago 12 juni 2019 10:30 GMT−4

Hi André,

A conceptual example is now available in https://www.comsol.com/model/bimetallic-strip-in-flow-74251 . This will however not help you with the more advanced questions.

If you are new to contact analysis, I think you should start by reading the Contact Modeling section in the Structural Mechanics User's Guide. There you can find hints about, for example, how to get convergence in the initial state.

Note that it is not formally necessary to use assembly mode for contact analysis. The only important thing is that the the contacting boundaries are not 'glued' by Form Union. Along another track: When you use assembly mode, you can prepare your model by doing explicit Union operations, so that there is a 'slit' only where you want it.

Why FSI (Pair) does not recognize the boundaries, I cannot guess. It is the correct approach if you are in assembly mode.

Pair Thermal Contact relies on the Contact feature in Solid Mechanics. As long as the latter identifies contact, then there should be a heat flux between the parts.

Regards,
Henrik

Hi André, A conceptual example is now available in . This will however not help you with the more advanced questions. If you are new to contact analysis, I think you should start by reading the *Contact Modeling* section in the *Structural Mechanics User's Guide*. There you can find hints about, for example, how to get convergence in the initial state. Note that it is not formally necessary to use assembly mode for contact analysis. The only important thing is that the the contacting boundaries are not 'glued' by **Form Union**. Along another track: When you use assembly mode, you can prepare your model by doing explicit **Union** operations, so that there is a 'slit' only where you want it. Why FSI (Pair) does not recognize the boundaries, I cannot guess. It is the correct approach if you are in assembly mode. **Pair Thermal Contact** relies on the **Contact** feature in Solid Mechanics. As long as the latter identifies contact, then there should be a heat flux between the parts. Regards, Henrik

Please login with a confirmed email address before reporting spam

Posted: 2 days ago 13 juni 2019 08:16 GMT−4
Updated: 2 days ago 13 juni 2019 08:41 GMT−4

Dear Henrik,

thank you for providing this example. It clarified some concepts.

I guess I will still use the assembly mode, since the plastic part has initially contact with the mold and will susbseuqently shrink due to cooling.

Regarding the FSI (Pair) issue: I resolved the problem. It was a stupid mistake on my part. I just highlighted the wrong Contact Pairs in the selection section.

However, if I may, I have another problem that I cannot get rid off. I think it is some error on my side. To provide resonable initial conditions for the fluid flow (pressure, velocity field), I added an additional stationary study step with an auxialliary sweep with respect to the inlet velocity that just solves for the flow problem. However, the problem does not converge to a reasonable solution. For some reason it always converges to a flow field that is 1 to 3 orders of magnitude above the average inlet velocity, which obviously cannot be true. I already checked my inlet (average inlet velocity between .001 and .1 m/s) and outlet condition (5 bar). The flow channel wall has a no-slip condition. If you have an idea on what I could possibly do wrong or any advice what to check, once again I'd greatly appreciate it.

Best regards, André.

Dear Henrik, thank you for providing this example. It clarified some concepts. I guess I will still use the assembly mode, since the plastic part has initially contact with the mold and will susbseuqently shrink due to cooling. Regarding the FSI (Pair) issue: I resolved the problem. It was a stupid mistake on my part. I just highlighted the wrong Contact Pairs in the selection section. However, if I may, I have another problem that I cannot get rid off. I think it is some error on my side. To provide resonable initial conditions for the fluid flow (pressure, velocity field), I added an additional stationary study step with an auxialliary sweep with respect to the inlet velocity that just solves for the flow problem. However, the problem does not converge to a reasonable solution. For some reason it always converges to a flow field that is 1 to 3 orders of magnitude above the average inlet velocity, which obviously cannot be true. I already checked my inlet (average inlet velocity between .001 and .1 m/s) and outlet condition (5 bar). The flow channel wall has a no-slip condition. If you have an idea on what I could possibly do wrong or any advice what to check, once again I'd greatly appreciate it. Best regards, André.

Please login with a confirmed email address before reporting spam

Posted: 2 days ago 13 juni 2019 08:45 GMT−4
Updated: 2 days ago 13 juni 2019 09:11 GMT−4

Dear Henrik, dear fellow COMSOLers,

I just found the solution myself. I had to deactivate the respective physics in the model (Modify model configuration in study step) instead of just 'unticking' the physics in the study step setup. I guess the latter deactivates the physics on a different level.

However, now when moving to the unsteady study step I get an error, that the wall velocity in the fluid domain is undefined for one of the fsi boundaries. I thought this is taken care of by the fsi multiphysics coupling,isn't it? I couldn't find anything in the manual (CFD or Solid Mechanics). Any hints on what to do?

The solver error message is as follows:

Failed to find consistent initial values. Velocity u_fluid, Pressure p Singular matrix.

There are 636 void equations (empty rows in matrix) for the variable comp1.fsip1.vWallx. at coordinates: (-0.85,-0.4), (-0.8375,-0.4), (-0.825,-0.4), (-0.8125,-0.4), (-0.8,-0.4), ... There are 636 void equations (empty rows in matrix) for the variable comp1.fsip1.vWally. at coordinates: (-0.85,-0.4), (-0.8375,-0.4), (-0.825,-0.4), (-0.8125,-0.4), (-0.8,-0.4), ... There are 636 void equations (empty rows in matrix) for the variable comp1.fsip1.vWallz. at coordinates: (-0.85,-0.4), (-0.8375,-0.4), (-0.825,-0.4), (-0.8125,-0.4), (-0.8,-0.4), ... and similarly for the degrees of freedom (empty columns in matrix). Last time step is not converged.

I checked via mesh statistics, the contact pairs for the fsi of the wall velocities have exactly 636 elements hence 636 equations. Something seems wrong with my setup.

Any advice is again greatly appreciated.

Best regards, André

PS: I attached the model file. It is set up in Comsol MP 5.4 Update 4.

Dear Henrik, dear fellow COMSOLers, I just found the solution myself. I had to deactivate the respective physics in the model (Modify model configuration in study step) instead of just 'unticking' the physics in the study step setup. I guess the latter deactivates the physics on a different level. However, now when moving to the unsteady study step I get an error, that the wall velocity in the fluid domain is undefined for one of the fsi boundaries. I thought this is taken care of by the fsi multiphysics coupling,isn't it? I couldn't find anything in the manual (CFD or Solid Mechanics). Any hints on what to do? The solver error message is as follows: Failed to find consistent initial values. Velocity u_fluid, Pressure p Singular matrix. There are 636 void equations (empty rows in matrix) for the variable comp1.fsip1.vWallx. at coordinates: (-0.85,-0.4), (-0.8375,-0.4), (-0.825,-0.4), (-0.8125,-0.4), (-0.8,-0.4), ... There are 636 void equations (empty rows in matrix) for the variable comp1.fsip1.vWally. at coordinates: (-0.85,-0.4), (-0.8375,-0.4), (-0.825,-0.4), (-0.8125,-0.4), (-0.8,-0.4), ... There are 636 void equations (empty rows in matrix) for the variable comp1.fsip1.vWallz. at coordinates: (-0.85,-0.4), (-0.8375,-0.4), (-0.825,-0.4), (-0.8125,-0.4), (-0.8,-0.4), ... and similarly for the degrees of freedom (empty columns in matrix). Last time step is not converged. I checked via mesh statistics, the contact pairs for the fsi of the wall velocities have exactly 636 elements hence 636 equations. Something seems wrong with my setup. Any advice is again greatly appreciated. Best regards, André PS: I attached the model file. It is set up in Comsol MP 5.4 Update 4.


Henrik Sönnerlind COMSOL Employee

Please login with a confirmed email address before reporting spam

Posted: 1 day ago 14 juni 2019 09:40 GMT−4
Updated: 1 day ago 14 juni 2019 09:40 GMT−4

This is an error which could happen if you are using Contact Pair and not Identity Pair on the solid-fluid boundary pairs.

Regards, Henrik

This is an error which could happen if you are using Contact Pair and not Identity Pair on the solid-fluid boundary pairs. Regards, Henrik

Please login with a confirmed email address before reporting spam

Posted: 1 day ago 14 juni 2019 10:10 GMT−4

Dear Henrik,

actually I figured that out myself just today. The contact pairs were generated with form assembly.

Anyways, thanks a lot again for all your great advice.

Best regards, André.

Dear Henrik, actually I figured that out myself just today. The contact pairs were generated with form assembly. Anyways, thanks a lot again for all your great advice. Best regards, André.

Reply

Please read the discussion forum rules before posting.

Please log in to post a reply.

Note that while COMSOL employees may participate in the discussion forum, COMSOL® software users who are on-subscription should submit their questions via the Support Center for a more comprehensive response from the Technical Support team.