Time Scale Control
The time scale (A time scale specifies divisions of time) used by the CFX-Solver can be controlled using one of three methods:
1- Auto Timescale (A default time scale specifies divisions of time pre-programmed into CFX).
2- Local Time Scale Factor (This is time scale specifies divisions of time for a location specfied by the user).
3- Physical Time Scale (A time scale specifies divisions of time for a specfic physical phenomena specfied by the user).
Understanding the three conditions is important in order to know their importance in which to b applied to your simulation. These settings can be applied from CFX-Pre by going to the Outline tree view and right-clicking Solver Control > Edit. Alternatively, you can use the CFX-Solver File Editor to achieve more control over the ANSYS CFX-Solver.
1- Auto Timescale (A default time scale specifies divisions of time pre-programmed into CFX).
2- Local Time Scale Factor (This is time scale specifies divisions of time for a location specfied by the user).
3- Physical Time Scale (A time scale specifies divisions of time for a specfic physical phenomena specfied by the user).
Understanding the three conditions is important in order to know their importance in which to b applied to your simulation. These settings can be applied from CFX-Pre by going to the Outline tree view and right-clicking Solver Control > Edit. Alternatively, you can use the CFX-Solver File Editor to achieve more control over the ANSYS CFX-Solver.
Auto Timescale
Auto Timescale is a fluid timescale control option that uses an internally calculated physical time scale based on the boundary conditions, flow conditions, physics, and domain geometry. The question to the researcher why would I care to what kind of time scale is used why?
Time scale is related to boundary conditions where for a simulation in a tube by knowing the length scale relating to tube diameter you can expect what kind of time scales.
Flow conditions relating to turbulence intesnity can also help in predicting the encountered time scales. You can either decrease your time scale or increase or use a moderate value one.
Next comes the question is what is the least time scale I can select and what is the maximum one I can select, well you can use the least time scale you can as long as the simulation wouldn't crash
Auto Timescale is the default timescale control setting. However, be aware that the Auto Timescale calculated by the solver is often conservative. This is usually robust, but faster convergence is often possible using a more aggressive setting. This can be done by:
1- Setting Length Scale Option to Aggressive.
2- Increasing the Time Scale Factor.
3- Changing to an appropriate Physical Time Scale.
It is also worth noting that, in some instances, the internal time scale calculation fails to find an appropriate velocity or length scale on which to base the time scale, this comes evident to the researcher after running simulations big deviations are visible between experimental and the numerical results.
For instance studying a buoyancy-driven flow problem (This phenomena is encountred in flames, Steam Boilers, atmospheric cases, ................ ) can be specified using a Sub-domain heat source (Heat source can be a flame for an example) in a cavity (Which represents the flame surface).
For the case of no velocity field difference or temperature difference being specified, a very large time scale (several orders of magnitude) can result. If this is the case, then you should try either:
1- Specifying a small fixed physical time scale and follow the general guidelines about increasing or decreasing time scale accordingly
2- Specifying an initial guess for velocity and/or temperature.
Time scale is related to boundary conditions where for a simulation in a tube by knowing the length scale relating to tube diameter you can expect what kind of time scales.
Flow conditions relating to turbulence intesnity can also help in predicting the encountered time scales. You can either decrease your time scale or increase or use a moderate value one.
Next comes the question is what is the least time scale I can select and what is the maximum one I can select, well you can use the least time scale you can as long as the simulation wouldn't crash
Auto Timescale is the default timescale control setting. However, be aware that the Auto Timescale calculated by the solver is often conservative. This is usually robust, but faster convergence is often possible using a more aggressive setting. This can be done by:
1- Setting Length Scale Option to Aggressive.
2- Increasing the Time Scale Factor.
3- Changing to an appropriate Physical Time Scale.
It is also worth noting that, in some instances, the internal time scale calculation fails to find an appropriate velocity or length scale on which to base the time scale, this comes evident to the researcher after running simulations big deviations are visible between experimental and the numerical results.
For instance studying a buoyancy-driven flow problem (This phenomena is encountred in flames, Steam Boilers, atmospheric cases, ................ ) can be specified using a Sub-domain heat source (Heat source can be a flame for an example) in a cavity (Which represents the flame surface).
For the case of no velocity field difference or temperature difference being specified, a very large time scale (several orders of magnitude) can result. If this is the case, then you should try either:
1- Specifying a small fixed physical time scale and follow the general guidelines about increasing or decreasing time scale accordingly
2- Specifying an initial guess for velocity and/or temperature.
Controlling the Time Scale for each Equation
CFX allows the researcher great flexibility in controlling the timescale used for each equation solved. You can specify a timescale on a global basis, a domain basis, a fluid basis, an equation-class basis, or an individual equation basis.
The researcher would ask the question why would I really need to understand the importance of the time scale for different equations, to answer such a question for a combustion chamber study the times scales for the momentum equations are bigger than the ones for the energy equation again why?
If you run a simulation without a heat release then you will see that the time scales to be studied are obvious and are related to some characteristic length scales such as inflow valve diameter, while when you have combined a case where heat release also occurs and this heat release is depending on different chemical reactions then it is necessary to refine the time scales more to monitor the different steps and that if there is a knocking effect occuring, if the time scale is too big the researcher would miss the knocking effect pressure fluctuations.
When setting timesteps like this, there will often be more than one timescale defined for any given equation. For example, you could define both a global timescale and a timescale for a single fluid in one domain.
The different ways in which a timescale can be set are outlined below in decreasing order of precedence below. For a given equation, the option with highest precedence will always be used:
1. For a specific equation, in a specific phase, in a specific domain. This comes of importance when you want to check that the chemical reaction time scales are the right ones to capture cetrain checmical reactions that only occur at ignition or flame out in a specfic region of the combustion chamber.
2. For a specific equation class, in a specific phase, in a specific domain.
3. For a specific equation class in a specific domain. Meaning the use of the same time scale for the three momentum equations that are used to calculate velocity components of the vector field.
4. For a specific equation class in all domains. As an example water occuring in three domains the first domain its in vapour form (very small concentrations) over the soil the second is after it condenses into droplets at the top soil layer then the last is where it drains to the resivouer.
5. For all equations, in a specific phase, in a specific domain. This is when the time scale is applied to all the solved equations momentum, mass and energy for a specfied domain and specified phase (gas,water,solid) found in the simulation.
6. For all equations in a specific domain.This is when the time scale is applied to all the solved equations momentum, mass and energy for a specfied domain found in the simulation.
7. For all equations globally. This is when the time scale is applied to all the solved equations momentum, mass and energy for all the domains found in the simulation.
8. For solid domains that use the Solid Timescale Factor option (when Solid Timescale Control is set to Auto Timescale).
An equation is a single-solved equation. This could be the momentum, continuity, or energy equation for a single fluid; the mass fraction equation for a single component; the volume fraction equation for a single fluid; one of the turbulence equations for a single fluid; or a single Additional Variable equation.
An equation class can include more than one equation. The equation classes are momentum, continuity, energy, rs (Reynolds stress), ke (turbulent kinetic energy), ed (turbulent eddy dissipation), tef (turbulent eddy frequency), meshdisp (mesh displacement), mf (mass fraction), vf (volume fraction) and av (Additional Variable).
The first eight of these will include more than one equation only in a multiphase and/or multi-domain simulation. The mf class will include as many equations as there are components, the vf class will include as many equations as there are fluids, and the av class will include as many equations as there are Additional Variables. The CFX-Pre user interface supports options 4, 7, and 8. To use other options, you must edit the CCL file.
The default approach for solid domains is thus the lowest priority option. If you wish to set a special timescale control for the energy equations in the fluid domain but not affect the solid domains, then you must use one of options 1, 2, or 3. If you use option 4 for the energy equation and also specify a Solid Timescale Factor, the Solid Timescale Factor will be ignored
The researcher would ask the question why would I really need to understand the importance of the time scale for different equations, to answer such a question for a combustion chamber study the times scales for the momentum equations are bigger than the ones for the energy equation again why?
If you run a simulation without a heat release then you will see that the time scales to be studied are obvious and are related to some characteristic length scales such as inflow valve diameter, while when you have combined a case where heat release also occurs and this heat release is depending on different chemical reactions then it is necessary to refine the time scales more to monitor the different steps and that if there is a knocking effect occuring, if the time scale is too big the researcher would miss the knocking effect pressure fluctuations.
When setting timesteps like this, there will often be more than one timescale defined for any given equation. For example, you could define both a global timescale and a timescale for a single fluid in one domain.
The different ways in which a timescale can be set are outlined below in decreasing order of precedence below. For a given equation, the option with highest precedence will always be used:
1. For a specific equation, in a specific phase, in a specific domain. This comes of importance when you want to check that the chemical reaction time scales are the right ones to capture cetrain checmical reactions that only occur at ignition or flame out in a specfic region of the combustion chamber.
2. For a specific equation class, in a specific phase, in a specific domain.
3. For a specific equation class in a specific domain. Meaning the use of the same time scale for the three momentum equations that are used to calculate velocity components of the vector field.
4. For a specific equation class in all domains. As an example water occuring in three domains the first domain its in vapour form (very small concentrations) over the soil the second is after it condenses into droplets at the top soil layer then the last is where it drains to the resivouer.
5. For all equations, in a specific phase, in a specific domain. This is when the time scale is applied to all the solved equations momentum, mass and energy for a specfied domain and specified phase (gas,water,solid) found in the simulation.
6. For all equations in a specific domain.This is when the time scale is applied to all the solved equations momentum, mass and energy for a specfied domain found in the simulation.
7. For all equations globally. This is when the time scale is applied to all the solved equations momentum, mass and energy for all the domains found in the simulation.
8. For solid domains that use the Solid Timescale Factor option (when Solid Timescale Control is set to Auto Timescale).
An equation is a single-solved equation. This could be the momentum, continuity, or energy equation for a single fluid; the mass fraction equation for a single component; the volume fraction equation for a single fluid; one of the turbulence equations for a single fluid; or a single Additional Variable equation.
An equation class can include more than one equation. The equation classes are momentum, continuity, energy, rs (Reynolds stress), ke (turbulent kinetic energy), ed (turbulent eddy dissipation), tef (turbulent eddy frequency), meshdisp (mesh displacement), mf (mass fraction), vf (volume fraction) and av (Additional Variable).
The first eight of these will include more than one equation only in a multiphase and/or multi-domain simulation. The mf class will include as many equations as there are components, the vf class will include as many equations as there are fluids, and the av class will include as many equations as there are Additional Variables. The CFX-Pre user interface supports options 4, 7, and 8. To use other options, you must edit the CCL file.
The default approach for solid domains is thus the lowest priority option. If you wish to set a special timescale control for the energy equations in the fluid domain but not affect the solid domains, then you must use one of options 1, 2, or 3. If you use option 4 for the energy equation and also specify a Solid Timescale Factor, the Solid Timescale Factor will be ignored
Controlling the Time Scale with the CFX-Solver File Editor
Advanced control over the auto time stepping algorithm is available using CCL directly or using the CFX-Solver File Editor. The following additional parameters are available:
a-Timescale Update Frequency: Controls the frequency with which a new timescale is updated (default is every 5 iterations)
b-Number of Timescale Updates: Controls the number of times that a new timescale is calculated (unbounded by default)
c-Timescale Ramping Factor: If the Number of Timescale Updates has been passed, and the Maximum Timescale is larger than the internally-calculated timescale, the solver increases the timescale every iteration by a factor of the Timescale Ramping Factor until the Maximum Timescale is reached. The default is 1.2.
a-Timescale Update Frequency: Controls the frequency with which a new timescale is updated (default is every 5 iterations)
b-Number of Timescale Updates: Controls the number of times that a new timescale is calculated (unbounded by default)
c-Timescale Ramping Factor: If the Number of Timescale Updates has been passed, and the Maximum Timescale is larger than the internally-calculated timescale, the solver increases the timescale every iteration by a factor of the Timescale Ramping Factor until the Maximum Timescale is reached. The default is 1.2.
Unless otherwise noted, all content on this site is @Copyright by Ahmed Al Makky 2012-2014- http://cfd2012.com