17.6.2. Format and Details of the Solver Settings File

Format of Solver Settings File

The following table shows the format and details of each of the fields.

KeysValues
solution-type"combustion"
combustion_simulation_type"full_eng_full_cycle"
rpm1800
crank_angle_step_size0.25
crank_radius0.045
piston_pin_offset0
piston_stroke_cutoff0.013
connecting_rod_length0.144
min_valve_lift0.0002
auto_activate_deactivate #t
symmetry_engine#t
ice_mesh_topologyice_mesh_topology#t
symm_normal(0 1 0)
point_on_symmetry(0 0.0002)
hybrid/layering"h"
conf/nonconfn
withbowl#f
piston_type3
no_of_valves2
cylinder_axis(0 0 1)
cylinder_axis_origin(0 -0 0.011)
cylinder_radius0.042
 
start_crank_angle0
insert_angle47
delete_angle313
reference_mesh_size0.000930
setup_valve_list((1 "invalve1" "invalve1" 323 563 0.015 (0 -0.24 0.97) (-0.02 -0.15 0.009) (smoothing #t) (end-valve-open-smoothing 384.4 ) (begin-valve-close-smoothing 528.7))

(2 "exvalve1" "exvalve1" 160 402 0.014 (-0 0.327 0.94) (-0.02 0.0197 0.0088) (smoothing #t) (end-valve-open-smoothing 185.3) (begin-valve-close-smoothing 365.4)) )


Note:  

  • The order of the keys is not important in the file.

  • All the units are in SI.


Details of Fields

solution-type

is the type of simulation you have chosen. Here it is set to "combustion”.

combustion_simulation_type

is the sub type of combustion simulation you have chosen. Here it is set to "full_engine_full_cycle”.

rpm

is the engine speed, which will be used along with crank angle step size to calculate the time step size.

crank_angle_step_size

will be used to calculate the time step. 0.25 is a good default value.

∆t=θ/6N(RPM)

crank_radius

is the crank radius in meter when the piston is at the Bottom Dead Center (BDC) position.

piston_pin_offset

is piston offset value in meter.

piston_stroke_cutoff

is the distance till which the layering part of the mesh will move as a rigid body. After this it will stop moving, but the piston head will continue to move until it reaches BDC. Thus the layering process will begin from the cutoff distance. This is required to create a large enough space in the upper part of the cylinder, that is meshed with tetrahedra. It ensures that the valves can fully move in that zone and the smoothing and remeshing process can happen. This value along with the value of min_valve_lift are used to control the actual values of the valve lift and piston stroke, such that:

νlift = max (vclift, vminlift)

ps = min (pcs, pmins)

connecting_rod_length

is the length of the connecting rod in meters.

min_valve_lift

takes the floating numerical value of the minimum valve lift in meters. Fluent assumes that once you have set up the mesh topology, the mesh topology is unchanged throughout the entire simulation. Therefore, Fluent does not allow you to completely close the valves such that the cells between the valve and the valve seat degenerate (become flat cells) when these surfaces come in contact. (Removing these flat cells would require the creation of new boundary face zones). To prevent this collapse, you need to define a minimum valve lift and Fluent will automatically stop the motion of the valve when the valve lift is smaller than the minimum valve lift value.

auto_activate_deactivate

is set to Boolean #t or #f. This will be used to deactivate some of the fluid zones which are not part of the simulation.

symmetry_engine

will take the value #t or #f, depending on whether the engine has symmetry defined or not.

ice_mesh_topology

will take the value #t if the mesh topology is the default ICE topology.

symm_normal

takes the format of (x y z). If symmetry is defined, you have to provide the normal at the given point.

point_on_symmetry

takes the format of (x y z). If symmetry is defined, you have to provide a point on the symmetry.

hybrid/layering

takes the input "h" or "l" with quotes. If you are opting for a hybrid mesh i.e. layering in the valve region and combination of re-meshing and layering in the cylinder and dome region, you need to set it as "h". If you are opting for a layered mesh in the valve, dome, and the cylinder region, then you need to set it as "l".

conf/nonconf

takes the input "n" or “c” (with quotes) depending on whether the mesh has non conformal interfaces ("n") or conformal ("c" ) interfaces.

withbowl

takes the Boolean value #t or #f, and will be used to define proper interfaces.

piston_type

will be used in the case of a hybrid approach. It takes input 1 or 3. 1 is for straight valve, or canted valve engine with chamber decomposition. 3 is used for straight or canted valve engines, without chamber decomposition. In the case of layered approach this value will not be used.

no_of_valves

is the number of valves in the setup valve list.

cylinder_axis

takes the input in the form of (x y z). It is the axis of the cylinder.

cylinder_axis_origin

takes the input in the form of (x y z). It signifies the point of origin of the cylinder axis.

cylinder_radius

is the radius of the cylinder in meters.

Values of cylinder axis, origin, and radius are used to define the rigid body motion for the piston and also for remeshing of the dynamic cylinder zone.

start_crank_angle

is the angle at which decomposition takes place. It is set to 0 by default.

insert_angle

is used to insert an interior zone in case of canted or straight valve engines without chamber decomposition. This is in the case where there is no initial layering zone.

delete_angle

is used to delete the interior zone inserted by the insert_angle.

reference_mesh_size

is a reference value. Some global and local mesh setting values are dependent on this term. This term is used to set layering height for vlayer, ch-lower, and ch-valve bodies.

  • For vlayer layer height is equal to (0.4 X reference_mesh_size).

  • For ch-lower and ch-valve layer height is equal to (0.8 X reference_mesh_size).

setup_valve_list

contains all the information related to valve in the format shown.

((Valve-Index “Valve-Name” “Valve-Profile-Name” Valve-Open-Angle Valve-Close-Angle (valve Axis vector) (Valve origin coordinates) Variable-urf? Variable-timestep? (smoothing #t) (end-valve-open-smoothing 384.4) (begin-valve-close-smoothing 528.7))(Valve-Index ……..))

If the field Variable-urf? is #t Fluent automatically increases and decreases the URF (under relaxation factors) values of the flow.

Similarly if Variable-timestep is #t Fluent will modify the time step during valve openings.

If smoothing is set to #t, solver will only do smoothing while valve is opening, till reaching the crank angle end-valve-open-smoothing. (Here for the invalve you have set it to 384.4). Also solver will stop layering and start smoothing while closing the valve at begin-valve-close-smoothing. (In this example it for the invalve it is set at 528.7 degrees).


Release 18.2 - © ANSYS, Inc. All rights reserved.