Thermal-mechanical coupling modeling and analysis method for refractory material masonry based on numerical simulation

Abstract

The invention discloses a thermal-mechanical coupling modeling and analysis method for a refractory material masonry based on numerical simulation. The invention aims to build a brick stack model by using refractory material masonry, simulate the actual heat shrinkage process of the brick stack, effectively obtain the stress concentration area of the brick stack in the shrinkage process, and avoid the problems of cracking and stack transfer caused by excessive stress concentration of the brick stack. According to the method, on the basis of finite element analysis software, a brick stack model and a lining plate model are arranged, a combination of the brick stack model and the lining plate model is assembled, it is guaranteed that the brick stack can freely contract after being heated, and the thermal analysis type of finite elements is sequential coupling. According to the method, the stress distribution of the brick stack in the shrinkage process caused by heating is obtained, the stress concentration area is marked as the easy-to-deform area, and brick stack deformation caused by overlarge thermal stress in the firing process is predicted. According to the method, the actual production process can be effectively guided, the stress is dispersed by optimizing the overlapping mode of the brick stack, and the problems of cracking and stack transfer caused by overlarge stress in the local area of the brick stack are avoided.

Description

Technical Field

[0001] The invention relates to the field of refractory brick production technology analysis, and in particular to a thermal-mechanical coupling modeling and analysis method for refractory material masonry based on numerical simulation. Background Art

[0002] Bauxite is a strategic resource in my country. In order to improve the comprehensive utilization rate of bauxite resources and enhance the quality stability of products, Chinese scholars have researched and developed a high-quality synthetic raw material with Chinese characteristics - bauxite-based homogeneous material. Using natural bauxite ore as raw material, alumina-based homogeneous synthetic refractory raw materials are prepared through processes such as ore dressing, homogenization, molding, and high-temperature calcination.

[0003] Before high-temperature calcination, the extruded bricks need to be stacked on the kiln car in a certain order. During high-temperature calcination, the aluminum oxide and silicon oxide in the bauxite will undergo a solid-phase reaction to form mullite, which is the main component of the bauxite-based mullite homogenous material. During the solid-phase synthesis process, the bricks soften at high temperatures on the one hand, and shrink in volume on the other hand, which causes the brick stack to collapse when passing through the high-temperature zone of the tunnel kiln. The collapsed bricks may fall into the connection between the kiln car and the tunnel kiln (curved seam), causing the kiln to get stuck. The occurrence of this phenomenon will not only reduce production efficiency, but also cause great economic losses.

[0004] Optimizing the stacking method of masonry is one way to improve the collapse of brick stacks. However, the optimization effect of the stacking scheme needs to be tested in the kiln. If the brick stack collapses during the test, it will also cause great losses. Summary of the invention

[0005] In order to overcome the deficiencies of the above-mentioned prior art, the present invention provides a thermal-mechanical coupling modeling and analysis method for refractory masonry based on numerical simulation, and uses finite element analysis software to simulate the stress distribution of brick stacks in high temperature zones to predict whether they will collapse in high temperature zones.

[0006] The technical solution adopted by the present invention is: a thermal-mechanical coupling modeling and analysis method of refractory masonry based on numerical simulation, comprising the following steps:

[0007] S1. Building a brick model: Building a brick model using 3D modeling software and importing the model into finite element analysis software;

[0008] S2. Assignment of material properties: Create a cross section of the brick model through the property module of the finite element analysis software, and assign the material properties of the brick model to the created cross section;

[0009] S3. Building a brick stack model: using the assembly module of the finite element analysis software to assemble the brick stack model, taking the brick model as the smallest unit, to build the brick stack model;

[0010] S4. Meshing of the brick stack model: Use the mesh module of the finite element analysis software to mesh the brick stack model and set the unit type to heat transfer;

[0011] S5. Setting of heat transfer analysis step for brick stack model: setting the analysis to “heat transfer” through the analysis step module of finite element software, and setting the “heat transfer” analysis step;

[0012] S6. Load setting for heat transfer of brick stack model: enable the load module of finite element analysis software to apply boundary conditions, and apply temperature to the heated surface of the brick stack model in the "heat transfer" analysis step as the boundary condition;

[0013] S7. Job settings for heat transfer of brick stack model: Create and submit a job in the job module. Set the multi-core processor to perform calculations in the parallel stage to simulate the heat transfer of the brick stack model, obtain the temperature field of the heat transfer of the brick stack model, record the incremental steps of the "heat transfer" analysis step, and save the odb file.

[0014] S8. Import the thermal stress model of the brick stack model: copy the brick stack model in S3 and rename it;

[0015] S9. Establishment of lining model: Use 3D modeling software to establish the lining model, and import the lining model into finite element analysis software;

[0016] S10, assembling the brick stack model and the lining board model: using the assembly module of the finite element analysis software, assembling the lining board model below the brick stack model, placing the brick stack model on the lining board model, making the bottom surface of the brick stack model contact with the upper surface of the lining board model, and obtaining a combination of the brick stack model and the lining board model;

[0017] S11. Setting of analysis step for thermal stress of brick stack: Use the analysis step module of finite element analysis software to change the type of “heat transfer” in the “heat transfer” analysis step to “static, general” and set the “static, general” analysis step;

[0018] S12. Load setting of thermal stress of brick stack: Use the load module of finite element analysis software to create gravity load, boundary conditions and predefined fields of the combination of brick stack model and liner model;

[0019] S13. Contact setting between brick stack model and lining model: Use the interaction module of finite element analysis software to create contact action properties and edit the interaction;

[0020] S14, meshing the lining plate model, using a meshing module of a finite element analysis software to mesh the lining plate model;

[0021] S15. Mesh type setting for thermal stress of brick stack model: Use the mesh module of finite element analysis software to modify the module unit type and change "heat transfer" to "three-dimensional stress";

[0022] S16. Job setting of thermal stress of brick stack model: using the job module of finite element software to create and submit the job, and obtain the stress distribution of the brick stack model;

[0023] S17. The area with concentrated stress distribution found in S16 is the potential deformation area of ​​the brick stack model. The deformation behavior of bricks in the brick stack during high-temperature firing is predicted by the size of the stress distribution.

[0024] Furthermore, the 3D modeling software described in S1 and S9 is built-in 3D modeling software, Solidworks or Inventor.

[0025] Furthermore, the material properties described in S2 include density, Young's modulus, Poisson's ratio, specific heat capacity, thermal conductivity and thermal expansion coefficient of the brick model.

[0026] Where: density is 1.93e-9t / mm 3 , plasticity is 2MPa, Young's modulus is set to 10MPa, Poisson's ratio is 0.2, specific heat capacity is 1e8 J / k·℃, thermal conductivity is 20W / m·℃, thermal expansion coefficient varies with temperature, the expansion coefficient range is -0.00894 to -0.00485, and the expansion coefficient corresponds to a temperature of 1680℃ to 490℃.

[0027] Furthermore, the settings of the "heat transfer" analysis step in S5 include: time length, maximum temperature change value allowed per load step, maximum radiation change value allowed per load step, incremental step size, and the "heat transfer" analysis step field output request is set to the node temperature NT.

[0028] Among them: the time length is 4800, the maximum temperature change allowed per load step is 10, the maximum radiation change allowed per load step is 0.1, the initial increment step is 0.01, and the minimum is 1E-07.

[0029] Furthermore, the temperature applied to the heated surface of the brick stack model in the "heat transfer" analysis step in S6 is 1680°C.

[0030] Furthermore, the liner model type in S9 is discrete rigid, the shape in the basic features is shell, the type is plane, and the center of the plane is taken as the reference point of the rigid body plane.

[0031] Furthermore, the settings of the "static, general" analysis step in S11 include: time length, incremental step size; the "static, general" analysis step field output request is set to stress S, displacement U, strain E,

[0032] Among them, the time length is 1, the initial increment step is 0.01, and the minimum is 1E-07.

[0033] Furthermore, the gravity load, boundary conditions and predefined field of the combination of the brick stack model and the liner model in S12 are as follows: create a gravity load for the combination of the brick stack model and the liner model, disable the boundary conditions in S6, create a new boundary condition, apply the reference point of the regional liner model, the type is "displacement / rotation", select "U1, U2, U3, UR1, UR2, UR3", and their values ​​are all 0,

[0034] A predefined field is created for the "Static, General" analysis step. The predefined field is a temperature field with a type of "temperature" and a value in degrees Celsius. The temperature field acts on a combination of the brick stack model and the lining model. The distribution is "from the result or output database file". The file name is the odb text saved in S7. The start analysis step, start increment, and end analysis step are all 1, and the end increment is the number of incremental steps recorded in S7.

[0035] Furthermore, the creation of contact action attributes and editing of interactions in S13 specifically include the following steps:

[0036] S131. Create contact action properties, select the friction formula "penalty" for tangential behavior, the friction coefficient is 0.5, the normal behavior, the pressure interference is hard contact, and separation after contact is not allowed;

[0037] S132. Edit the interaction and create an interaction for the "Static, General" analysis step. The type is surface-to-surface contact, where the master surface is the upper surface of the liner model and the slave surface is the bottom surface of the brick stack model.

[0038] Beneficial effects of the present invention:

[0039] The present invention is based on finite element analysis software, by setting a brick stack model and a lining model, and assembling a combination of the brick stack model and the lining model, to ensure that the brick stack can shrink freely when heated, and the finite element thermal analysis type is sequential coupling. The present invention obtains the stress distribution of the brick stack during the shrinkage process caused by heat, and marks the stress concentration area as an easy-to-deform area, so as to predict the deformation of the brick stack caused by excessive thermal stress during the firing process. The present invention can effectively guide the actual production process, and by optimizing the overlapping method of the brick stack, the stress is dispersed to avoid the cracking and stacking problems caused by excessive stress in the local area of ​​the brick stack. BRIEF DESCRIPTION OF THE DRAWINGS

[0040] Figure 1 The temperature field cloud diagram of the brick stack during the firing process in the embodiment of the present invention;

[0041] Figure 2 This is a cloud diagram of the Z-axis stress field during the firing process of the brick stack in an embodiment of the present invention;

[0042] Figure 3 It is a Y-axis stress field cloud diagram during the brick stack firing process in an embodiment of the present invention. DETAILED DESCRIPTION

[0043] In order to more clearly understand the technical solution of the present invention, the present invention is further described below in conjunction with the accompanying drawings;

[0044] like Figure 1-Figure 3 As shown, the thermal-mechanical coupling modeling and analysis method of refractory masonry based on numerical simulation includes the following steps:

[0045] S1. Establishment of brick model: Use 3D modeling software to establish brick model, and import the model into finite element analysis software. The 3D modeling software is built-in 3D modeling software, Solidworks or Inventor. When using it, choose the appropriate 3D modeling software according to the proficiency of the operator.

[0046] S2. Assignment of material properties: Create a cross section of the brick through the property module of the finite element analysis software, and assign the material properties of the brick to the created cross section.

[0047] Specifically, in this embodiment, the material properties include the density, Young's modulus, Poisson's ratio, specific heat capacity, thermal conductivity and thermal expansion coefficient of the brick model.

[0048] Where: density is 1.93e-9t / mm 3 , plasticity is 2MPa, Young's modulus is set to 10MPa, Poisson's ratio is 0.2, specific heat capacity is 1e8 J / k·℃, thermal conductivity is 20W / m·℃, thermal expansion coefficient varies with temperature, and the expansion coefficient ranges from -0.00894 to -0.00485. Due to the characteristics of refractory materials, its expansion coefficient is negative, and the expansion coefficient corresponds to a temperature of 1680℃ to 490℃.

[0049] S3. Establishment of brick stack model: Use the assembly module of finite element analysis software to assemble the brick stack model, and use the brick model as the smallest unit to build the brick stack model.

[0050] S4. Meshing of the brick stack model: Use the mesh module of the finite element analysis software to mesh the brick stack model and set the unit type to heat transfer.

[0051] S5. Heat transfer analysis step setting for brick stack model: Set the analysis step module of finite element software to "heat transfer" and set the "heat transfer" analysis step.

[0052] Specifically, in this embodiment, the settings of the "heat transfer" analysis step include: time length, maximum temperature change value allowed per load step, maximum radiation change value allowed per load step, and incremental step size. The "heat transfer" analysis step field output request is set to the node temperature NT, where: the time length is 4800, the maximum temperature change value allowed per load step is 10, the maximum radiation change value allowed per load step is 0.1, the initial incremental step is 0.01, and the minimum is 1E-07.

[0053] S6. Load setting for heat transfer of brick stack: Use the load module of finite element analysis software to apply boundary conditions, and apply temperature to the heated surface of the brick stack model in the "heat transfer" analysis step as the boundary condition.

[0054] Specifically, in this embodiment, the temperature applied to the heated surface of the brick stack model in the "heat transfer" analysis step is 1680°C.

[0055] S7. Job settings for heat transfer of brick stack model: Create and submit the job in the job module. Set the multi-core processor to perform calculations in the parallel stage to simulate the heat transfer of the brick stack model and obtain the temperature field of the heat transfer of the brick stack model. Record the incremental steps of the "heat transfer" analysis step and save the odb file.

[0056] S1-S7 calculates the heating of the brick stack model, the temperature transfer from the outside to the inside, and the overall heat transfer to obtain a temperature gradient.

[0057] S8. Import of thermal stress model of brick stack model: Copy the brick stack model in S3 and rename it.

[0058] S9. Establishment of lining model: Use 3D modeling software to establish lining model, and import the lining model into finite element analysis software. The 3D modeling software is built-in 3D modeling software, Solidworks or Inventor. When using it, choose the appropriate 3D modeling software according to the proficiency of the operator.

[0059] Specifically, in this embodiment, the liner model type is discrete rigidity, the shape in the basic feature is shell, the type is plane, and the center of the plane is taken as the reference point of the rigid body plane.

[0060] The lining model is set to be unaffected by thermal shrinkage. In this simulation, it is a non-deformable component. Under the action of temperature and gravity, each layer of the brick stack model shrinks. In the finite element calculation, the brick stack model needs to be fixed on a plane to reflect the effect of gravity on the brick stack model. Therefore, a lining model is set.

[0061] S10, assembling the brick stack model and the lining model: using the assembly module of the finite element analysis software, assembling the lining model under the brick stack model, placing the brick stack model on the lining model, making the bottom surface of the brick stack model contact with the upper surface of the lining model, and obtaining a combination of the brick stack model and the lining model.

[0062] If the bottom surface of the brick stack is selected for fixing, the brick stack will be affected by heat shrinkage, making the bottom brick stack unable to shrink freely, and thus generating a huge tensile stress, making the simulation calculation results inconsistent with reality. Therefore, a lining plate is added to the bottom of the brick stack, and the lining plate is fixed by using boundary conditions to apply gravity load. At the same time, it is ensured that the bottom layer of the brick stack can shrink freely under the influence of the temperature field.

[0063] S11. Analysis step setting of thermal stress of brick stack: Use the analysis step module of finite element analysis software to change the type of "heat transfer" in the "heat transfer" analysis step to "static, general" and set the "static, general" analysis step.

[0064] Specifically, in this embodiment, the settings of the "static, general" analysis step include: time length, incremental step size; the "static, general" analysis step field output request is set to stress S, displacement U, strain E, where the time length is 1, the initial incremental step is 0.01, and the minimum is 1E-07.

[0065] S12. Load setting for thermal stress of brick stack: Use the load module of the finite element analysis software to create the gravity load, boundary conditions and predefined fields of the combination of the brick stack model and the liner model.

[0066] Specifically, in this embodiment, the gravity load, boundary conditions and predefined fields of the combination of the brick stack model and the liner model are as follows: create a gravity load for the brick stack, disable the boundary conditions in S6, create a new boundary condition, apply the area to the reference point of the combination of the brick stack model and the liner model, set the type to "displacement / rotation", select "U1, U2, U3, UR1, UR2, UR3", and set their values ​​to 0.

[0067] A predefined field is created for the "Static, General" analysis step. The predefined field is a temperature field with a type of "temperature" and a value in degrees Celsius. The temperature field acts on a combination of the brick stack model and the lining model. The distribution is "from the result or output database file". The file name is the odb text saved in S7. The start analysis step, start increment, and end analysis step are all 1, and the end increment is the number of incremental steps recorded in S7.

[0068] S13. Contact setting between the bottom surface of the brick stack and the lining: Use the interaction module of the finite element analysis software to create contact properties and edit the interaction.

[0069] Specifically, in this embodiment, creating contact action attributes and editing interactions specifically include the following steps:

[0070] S131. Create contact action properties, select the friction formula "penalty" for tangential behavior, the friction coefficient is 0.5, the normal behavior, the pressure interference is hard contact, and separation after contact is not allowed;

[0071] S132, edit the interaction, create an interaction for the "Static, General" analysis step, the type is surface-to-surface contact, where the master surface is the lining and the slave surface is the bottom surface of the brick stack.

[0072] Bricks and lining plates are two different materials. In finite element calculations, two materials with different properties need to establish contact, that is, interaction, to ensure that the two parts are a whole, and then proceed to the next step of meshing and stress calculation. In the model, the contact parts of the two parts are the bottom surface of the brick stack model and the upper surface of the lining plate model. Therefore, the contact property is defined as "surface-to-surface contact".

[0073] S14. Meshing of the lining model: Use the mesh module of the finite element analysis software to mesh the lining model.

[0074] S15. Mesh type setting for thermal stress of brick stack model: Use the mesh module of finite element analysis software to modify the module unit type and change "heat transfer" to "three-dimensional stress".

[0075] S16. Job setting for thermal stress of brick stack: Use the job module of the finite element software to create and submit the job to obtain the stress distribution of the brick stack model.

[0076] S17. The area with high numerical stress distribution found in S16 is the potential deformation area of ​​the brick stack model. The deformation behavior of bricks in the brick stack during high-temperature firing is predicted by the size of the stress distribution.

[0077] The above description is only a preferred embodiment of the present invention, so all equivalent changes or modifications made according to the structure, characteristics and principles described in the scope of the patent application of the present invention are included in the scope of the patent application of the present invention.

Claims

1. A thermal-mechanical coupling modeling and analysis method for refractory masonry based on numerical simulation, characterized in that: The following steps are involved: S1. Building a brick model: Building a brick model using 3D modeling software and importing the model into finite element analysis software; S2. Assignment of material properties: Create a cross section of the brick model through the property module of the finite element analysis software, and assign the material properties of the brick to the created cross section; S3. Building a brick stack model: using the assembly module of the finite element analysis software to assemble the model, taking the brick model as the smallest unit, to build a brick stack model; S4. Meshing of the brick stack model: Use the mesh module of the finite element analysis software to mesh the brick stack model and set the unit type to heat transfer; S5. Setting of heat transfer analysis step for brick stack model: Set the analysis step module of finite element software to "heat transfer" and set the "heat transfer" analysis step; S6. Load setting for heat transfer of brick stack model: Use the load module of finite element analysis software to apply boundary conditions, and apply temperature to the heated surface of the brick stack model in the "heat transfer" analysis step as the boundary condition; S7. Job settings for heat transfer of brick stack model: Create and submit a job in the job module. Set the multi-core processor to perform calculations in the parallel stage. Perform heat transfer simulation of the brick stack model to obtain the temperature field of heat transfer of the brick stack model. Record the incremental steps of the "heat transfer" analysis step and save the odb file. S8. Import the thermal stress model of the brick stack model: copy the brick stack model in S3 and rename it; S9. Establishment of lining model: Use 3D modeling software to establish the lining model, and import the lining model into finite element analysis software. S10, assembling the lining model: using the assembly module of the finite element analysis software, assembling the lining model below the brick stack model, placing the brick stack model on the lining model, making the bottom surface of the brick stack model contact with the upper surface of the lining model, and obtaining a combination of the brick stack model and the lining model; S11. Analysis step setting of thermal stress of brick stack model: Use the analysis step module of finite element analysis software to change the type "heat transfer" in the "heat transfer" analysis step to "static, general" and set the "static, general" analysis step; S12. Load setting of thermal stress of brick stack model: Use the load module of finite element analysis software to create gravity load, boundary conditions and predefined fields of the combination of brick stack model and liner model; S13. Contact setting between brick stack model and lining model: Use the interaction module of finite element analysis software to create contact action properties and edit the interaction; S14, meshing the lining plate model, using a meshing module of a finite element analysis software to mesh the lining plate model; S15. Mesh type setting for thermal stress of brick stack model: Use the mesh module of finite element analysis software to modify the module unit type and change "heat transfer" to "three-dimensional stress"; S16. Job setting of thermal stress of brick stack model: using the job module of finite element software to create and submit the job, and obtain the stress distribution of the brick stack model; S17. The area with concentrated stress distribution found in S16 is the potential deformation area of ​​the brick stack model. The deformation behavior of bricks in the brick stack during high-temperature firing is predicted by the size of the stress distribution.

2. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The 3D modeling software described in S1 and S9 is built-in 3D modeling software, Solidworks or Inventor.

3. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The material properties described in S2 include the density, Young's modulus, Poisson's ratio, specific heat capacity, thermal conductivity and thermal expansion coefficient of the brick model. Where: density is 1.93e-9t / mm 3 , plasticity is 2MPa, Young's modulus is set to 10MPa, Poisson's ratio is 0.2, specific heat capacity is 1e8 J / k·℃, thermal conductivity is 20W / m·℃, thermal expansion coefficient varies with temperature, the expansion coefficient range is -0.00894 to -0.00485, and the expansion coefficient corresponds to a temperature of 1680℃ to 490℃.

4. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The settings of the "heat transfer" analysis step described in S5 include: time length, maximum temperature change value allowed per load step, maximum radiation change value allowed per load step, incremental step size, and the "heat transfer" analysis step field output request is set to the node temperature NT. Among them: the time length is 4800, the maximum temperature change allowed per load step is 10, the maximum radiation change allowed per load step is 0.1, the initial increment step is 0.01, and the minimum is 1E-07.

5. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The temperature applied to the heated surface of the brick stack model in the "Heat Transfer" analysis step described in S6 is 1680°C.

6. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The liner model type described in S9 is discrete rigidity, the shape in the basic features is shell, the type is plane, and the center of the plane is taken as the reference point of the rigid body plane.

7. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The settings for the "Static, General" analysis step described in S11 include: time length, incremental step size; the "Static, General" analysis step field output request is set to stress S, displacement U, strain E, Among them, the time length is 1, the initial increment step is 0.01, and the minimum is 1E-07.

8. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The specific method of the gravity load, boundary conditions and predefined field of the combination of the brick stack model and the lining model in S12 is as follows: create a gravity load for the combination of the brick stack model and the lining model, disable the boundary conditions in S6, create a new boundary condition, apply the area to the reference point of the lining model, set the type to "displacement / rotation", select "U1, U2, U3, UR1, UR2, UR3", and all of their values ​​are 0, Create a predefined field for the "Static, General" analysis step. The predefined field is a temperature field with a type of "Temperature" and a value in degrees Celsius. The temperature field acts on the brick stack model and is distributed as "From result or output database file". The file name is the odb file saved in S7. The start analysis step, start increment, and end analysis step are all 1, and the end increment is the number of incremental steps recorded in S7.

9. The method for thermal-mechanical coupling modeling and analysis of refractory masonry based on numerical simulation according to claim 1, characterized in that: The creation of contact action properties and editing of interactions described in S13 specifically include the following steps: S131. Create contact action properties, select the friction formula "penalty" for tangential behavior, the friction coefficient is 0.5, the normal behavior, the pressure interference is hard contact, and separation after contact is not allowed; S132. Edit the interaction and create an interaction for the "Static, General" analysis step. The type is surface-to-surface contact, where the master surface is the upper surface of the liner model and the slave surface is the bottom surface of the brick stack model.

Images