6.1.1. Basic Settings

In the Basic Settings tab you have the following settings:

Solution Type

shows the Solution Type you have selected in the Properties view of the ICE cell. You cannot make any changes here.

Initialize Flow

is set to Yes by default. This will initialize the flow. To check the initialization settings see the Solution Initialization task page in ANSYS Fluent.

Set Default Models

is set to Yes by default. For cold flow simulation some models of ANSYS Fluent have been chosen as default for better results. These are the Energy model, and the Standard k-epsilon model from the list of Viscous models with Standard Wall Functions. You can check them at the Models task page of ANSYS Fluent.

Auto Save Type

is set to Crank Angle by default. This means that the intermediate case and data files will be saved at the entered frequency crank angles. You can also select Time from the drop-down menu if you want to save the case and data files at a specific frequency of time steps.

Auto Save Frequency

shows the number of crank angle or time steps, after which the case and data file will be saved in ANSYS Fluent. This will depend upon your selection of Auto Save Type. Here the default value is 30.

Engine Speed(rpm)

It is set to a default value of 1800. The engine speed is used along with the crank angle step size to calculate the time step size. You can enter the speed of your engine here. You can enable the check box next to it to parameterize it.

Number of CA to run

is set to 720 by default. This corresponds to a full cycle. You can enter the number of crank angles you want to run the simulation

Read Profile File

allows you to read multiple profile files. Clicking on Read Profile File opens Browse profile file dialog box. In the browsing window three types of file extensions will be supported .prof (profile file), .ttab (transient table), and .csv. All Files option is also present if you have a file extension which does not match with either of the given extensions. In this case the file type will be automatically identified, and an error will be thrown if the format is not supported.

If you select a .csv file and click Open, then a Read CSV File dialog box opens.

  • You need to enter a name for Profile Name. This name will appear in the drop-down list of Profiles in the Profile Editor dialog box.

  • If you retain the default setting of Yes for Read CSV Titles then the quantity or variable names will be as per the names in the CSV file.

  • If you choose No for Read CSV Titles then you have to specify the No. of Columns of the CSV file you want to read. For each column you have to select a different variable name from the drop-down list. In this case the titles of the CSV columns will not be read. Your selections for the columns will be the titles.


    Important:  

    • All the columns in CSV should have same number of values. Variable number of values and interpolation is not supported in the current version.

    • Ensure that there are no empty spaces in the titles.


    The format of the standard profile file is

     ((profile-name transient n periodic?)
     (field_name-1 a1 a2 a3 .... an)
     (field_name-2 b1 b2 b3 .... bn)
     .
     .
     .
     .
     (field_name-r r1 r2 r3 .... rn)) 
    

    The profile name as well as the field names have to be shorter than 64 characters. One of the field_name should be used for the time field, and the time field section must be in ascending order. n is the number of entries per field. The periodic? entry indicates whether or not the profile is time-periodic. Set it to 1 for a time-periodic profile, or 0 if the profile is not time-periodic.

    An example is shown below:

    ((sampleprofile transient 8 0 0)
    (angle
    4.400000e+02 4.412000e+02
    4.644900e+02 4.656900e+02
    6.400000e+02
    6.412000e+02 6.480800e+02 6.492800e+02)
    (mass-flow
    0.000000e+00 2.450040e-03 2.450040e-03 0.000000e+00 0.000000e+00
    2.475870e-03 2.475870e-03 0.000000e+00)
    (velocity
    0.000000e+00 1.941520e+02 1.941520e+02 0.000000e+00 0.000000e+00
    1.922430e+02 1.922430e+02 0.000000e+00)
    )

    Important:  All quantities, including coordinate values, must be specified in SI units because ANSYS Fluent does not perform unit conversion when reading profile files. Also, profile names must have all lowercase letters (for example, name). Uppercase letters in profile names are not acceptable.


The format of the transient table file is

 profile-name n_field n_data periodic?
 field-name-1 field-name-2 field-name-3 .... field-name-n_field 
 v-1-1  v-2-1... ... ... ... v-n_field-1 
 v-1-2  v-2-2... ... ... ... v-n_field-2
 .
 .
 .
 .
 .
 v-1-n_data v-2-n_data ... ... ... ... v-n_field-n_data 

The first field name (for example field-name-1) should be used for the time field, and the time field section, which represents the flow time, must be in ascending order. The periodic? entry indicates whether or not the profile is time-periodic. Set it to 1 for a time-periodic profile, or 0 if the profile is not time-periodic.

An example is shown below:

sampletprofile 3 8 0
angle        mass-flow    velocity
440          0.0          0.0
441.2        0.00245004   194.152
464.49       0.00245004   194.152
465.69       0.0          0.0
640          0.0          0.0
641.2        0.00247587   192.243
648.08       0.00247587   192.243
649.28       0.0           0.0

This file defines the same transient profile as the standard profile example above.


Important:  All quantities, including coordinate values, must be specified in SI units because ANSYS Fluent does not perform unit conversion when reading profile files. Also, profile names must have all lowercase letters (for example, name). Uppercase letters in profile names are not acceptable. When choosing the field names, spaces or parentheses should not be included.


After reading the files the profiles will be available in the boundary condition drop-down lists.

Profile Editor

allows you to view the plot of the profiles.

  • Select a profile from the drop-down list of Profiles. The TIMESTEP profile is added to the list by default.

  • When a particular profile is selected all corresponding variables will be displayed in the X Axis and Y Axis drop-down lists.

  • Select the variable for X Axis and Y Axis and click Plot. The plot will be displayed in the area of Profile Chart.

  • You can select the type of chart to be displayed from the Chart Style drop-down list. Options of Spline, Step and Line are provided.

  • You can also read a profile by clicking on Read File.

  • The read profile which is presently selected can be deleted from the list by clicking on Remove Profile.

  • You can make changes to the values in the profile table displayed. Click Plot to view the Profile Chart with the changed values. You can save the profile with the edited values by clicking on Save.

  • To manipulate the chart view:

    Table 6.1:  Chart Manipulation

     Operation
    Rotate Middle Mouse Zoom
    Shift + Middle MouseZoom
    Ctrl + Middle MousePan
    Drag Right MouseBox Zoom
    F keyFit to Window


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