This webinar gives an overview of different Heat Transfer and Thermal-stress capabilities such as :
• Steady State and transient heat transfer
• Sequential and Fully Coupled Thermal Stress Analyses
• Contact in heat transfer problems.
The success of many structural designs requires a thorough understanding of both the thermal and mechanical response of the design. Temperature-dependent material properties, thermally-induced deformation, and temperature variations all may be important design considerations.
The webinar was run live three times for different regions around the globe. Please find below some of the Q and A from these sessions.
Q: Does Abaqus have a latent heat term/input or do you add it through a UMAT?
A: Yes, Abaqus does have a latent heat term and if you want to model complex phase change then you might have to use the UMAT. But for general cases you can use inbuilt latent heat option. Ref: Section 26.2.4 Latent heat of the Abaqus analysis users manual.
Q: Does Abaqus support Crank–Nicolson time integration?
A: The transient heat transfer analysis uses a modified Crank-Nicolson time integration.
Q: Do you have a way to define direction of gravity and then select one of the many empirical models of temperature-based convection models in order to apply convection coefficient automatically on the surfaces?
A: Not at the moment.
Q: Tech Question: How Abaqus will manage huge deformations on this case? Because some cases we could have huge elements deformations, na don that loosing element quality producing bad results
A: Whilst performing either sequential or fully coupled thermal stress analysis we need to make sure that the structural mesh is of sufficient refinement to be able to capture the thermal strain gradients. If using Explicit then we can make use of the ALE approach to ensure that element quality is maintained in large deformation problems. Ref: 12.2 ALE adaptive meshing of the Abaqus analysis users manual.
Q: In radiation analysis, does it take care of view factor in situations where surfaces exchage heat with each other through radiation? Or, do you have to turn it on explicitly during analysis?
A: In radiation analysis one of the inputs is the viewfactor. This needs to be specified before the analysis starts. However if you are using Cavity Radiation in Abaqus/Standard then the view factors are calculated automatically for you. Ref: Cavity radiation under Section 6.5.2 Uncoupled heat transfer analysis of the Abaqus analysis users manual. Ref: Section 2.11.5 View factor calculation of the Abaqus Theory Guide.
Q: In case of heat trasfer through contacts, could you make it dependent on pressure between the contacting surfaces?
A: Yes, this is possible. However this is valid only in the stress analysis side of the thermal stress problem (i.e. Fully coupled thermal stress) as contact pressure is valid only in a structural analysis and can change depending on how the surfaces move relative to each other. This can be a function of the clearance between the two surfaces, pressure and also mass flow rate.
Q: is there any restriction in abaqus w.r.t. radiation problem size ?
A: I am not aware of any restriction as such on the radiation problem size.
Q: How is the Gap Conduction depends on the distance between the surfaces... how do we estimate this parameter?
A: Gap conduction is dependent on the distance between the surfaces. A higher value of gap conduction indicates the presence of a liner between the surfaces with high conducting capacity hence more heat can flow between them. The value of the gap conductance depends on the materials of the underlying surfaces as well as the material of the liner between the surfaces.
Q: Any guidelines on how to select the DELTMX parameter?
A: There are no specific guidelines on selecting the DELTMX parameter. IF you run the analysis and you see that there are a lot of changes happening between successive increments and feel that you are not able to capture the physics in fine enough detail then you can force Abaqus to take increment such that the temperature changes at all nodes in the model is less that the DELTMX parameter. If in doubt then I would recommend you leave it as the default.
Q: What functions does Abaqus have to perform thermal cycling for thermal fatigue? Or will I need to create a step for each cycle?
A: Abaqus offers a low cycle fatigue analysis using the direct cyclic approach. Please refer to Section 6.2.7 Low-cycle fatigue analysis using the direct cyclic approach of the Abaqus Analysis Users Manual.
Q: Can you describe how the mapping happens in sequentially coupled analysis when the time increments and/or mesh don't match between the thermal and stress analysis?
A: Mesh don’t match: When you are mapping between different meshes then we have to set the option to be uncompatible while defining the mapping. When regions of elements in the heat transfer analysis are close or touching, the dissimilar mesh interpolation capability can result in an ambiguous temperature association. For example, consider a node in the current model that lies on or close to a boundary between two adjacent parts in the heat transfer model, and consider a case where temperatures in these parts are different. When interpolating, Abaqus will identify a corresponding parent element at the boundary for this node from the heat transfer analysis. This parent element identification is done using a tolerance-based search method. Hence, in this example the parent element might be found in either of the adjacent parts, resulting in an ambiguous temperature definition at the node. You can eliminate this ambiguity by specifying the source regions from which temperatures are to be interpolated. Ref: Section 34.2.1 Initial conditions in Abaqus/Standard and Abaqus/Explicit
Time increment: A transient heat transfer analysis that uses the Abaqus/Standard automatic time incrementation scheme will produce sets of temperature data points at times that do not necessarily correspond with the times generated by the automatic time incrementation scheme used by the subsequent structural analysis. Abaqus will interpolate linearly between the time points stored for the heat transfer analysis to obtain temperature values at the time points required by the structural analysis. Ensure that the heat transfer output contains sufficient data (that is, enough increments are stored) to make this interpolation meaningful.
Q: Does Abq/Std have the ALE capability?
A: Yes, it does. Ref: Section 12.2.1 ALE adaptive meshing: overview of the Abaqus Analysis Manuals.
Q: Can you provide a resource that describes various thermal cycling/fatigue analysis methods?
Article ID : QA00000008275
Abstract : Abaqus Technology Brief: Low-cycle Thermal Fatigue of a Surface-mount Electronics Assembly
Link : Article Id : https://kb.dsxclient.3ds.com/mashup-ui/page/document?q=docid:QA00000008275
Family Id: https://kb.dsxclient.3ds.com/mashup-ui/page/index?q=famid:QA00000008275
Q: Must Abaqus explicit be used for thermal cycling analysis? If so, and since XFEM can't be used in explicit, what methods for crack growth can be used in thermal fatigue
A: Not required. The low cycle fatigue option is available in Abaqus/Standard.
Q: Slide pg 31 & 44, how do you create graphs like that?
A: These can be created by using XY plots. You can operate and extract results from Field output variables and then customize these plots. Please refer to Section 47 X–Y plotting of the Abaqus CAE Users manual.
Q: are there example models of gap radiation?
A: There are some benchmark models available which can be used to understand gap radiation. Ref: Benchmark number 1.6.3 Coupled temperature-displacement analysis: one-dimensional gap conductance and radiation of the Abaqus Benchmarks Guide.
Q: what effect does different mesh densities make using GAP Conduction. what effect does different surface sizes make to the conduction in reality the mating surfaces are usually slightly different areas
A: We will have to run some test models to understand this behavior in detail.
Q: for one piece (no contact with others)that we can use sequentially coupled thermal stress analysis, if we use fully analyse, can we have the same results? (know that for example sequentially use C3D8T but fully use C3D8)
A:Yes, the results should be same. If the stress field does not affect the temperature field then the results should be very similar to doing a sequentially coupled analysis. However depending on the problem size this might be more expensive in terms of time required to solve the problem.
Q: Where can we find the four constant values used in the gap radiation calculation?
A: the value of the Stefan Boltzmann constant should be freely available in literature. The emissivity’s depend on the material and again should be available in literature. The View Factor can be calculated using a formula. Ref: Section 2.11.5 View factor calculation of the Abaqus Theory Guide.
Q: wasn't clear where the heat transfer coefficient could be defined
A: HTC can be defined at the nodal level or on the surface as well.
Q: Can we fully couple thermal analysis with viscoelastic materials
A: In Abaqus/Standard a fully coupled temperature-displacement analysis can be used to analyze static creep and swelling problems, which generally occur over fairly long time periods (“Rate-dependent plasticity: creep and swelling,” Section 23.2.4); viscoelastic materials (“Time domain viscoelasticity,” Section 22.7.1); or viscoplastic materials (“Rate-dependent yield,” Section 23.2.3).
Q: Is the 'film coefficient' the same as 'heat transfer coefficient'?
A: Yes.
Q: can you define a time-varying thermal gradient in shell elements directly for the structural analysis?
A: Yes, This can be done. The time variation can be done by an Amplitude curve.
Q: Is the gap the actual gap in distance?
A: Yes, This is the normal distance between the two surfaces.
Q: do you know when the 16Gb limit will be lifted on the data file within pre, this limit on size exists when running pre and reading input loading data. This limits the size of the thermal model.
A: We are aware of this limit and whilst HQ are working on this, there might not be significant improvements due to the limitation in the architecture. I think as a WA you can run multiple restarts. Though not an elegant solution this is what we have at the moment.
Q: How to map variable heat fulx and nodal temperature from CFD(as initial BC's) run into my Abaqus Heat transfer run in ABAQUS CAE?
A: Nodal temperature if you have them in ASCII format you can read them in via the pre-defined field option. Heat flux can be mapped as a mapped field. Ref: Section 58.7 Creating mapped fields from the Abaqus CAE Users Manual.
All answers are pretty short and to the point. If more details are required you can contact your local support offices. All the references to the manual are based on the Abaqus 6.14 User manuals. Please find below a link to the replay of the eSeminar.
