Encyclopaedia Index

## Space and Time Grids

### Spatial Grids

There are three kinds of spatial grids:

• Cartesian: the grid is composed of six-sided rectangular 'brick' elements. All the grid lines are straight. One plane of element faces is shown below. The 'region' , 'interval' and 'non-uniformity' features are present in all three grid kinds.

• Cylindrical-Polar: the grid is composed of six-sided annular 'brick' elements.
• The x-direction is always the angle, q, measured in radians.
• The y-direction is always the radius, r.
• The z-direction is always the axis.
• Body-Fitted (BFC): the grid is composed of topologically six-sided 'bricks' with arbitrarily-located corners. Their locations are measured in a Cartesian frame of reference.

### Switching Co-ordinate Systems

To switch between the co-ordinate systems, click on Menu / Geometry, then on Co-ordinate system. The Cartesian grid is the default.

IMAGE: Grid Mesh Settings Dialog

The change between Cartesian and Cylindrical-polar can be made in either direction.

Note that whilst it is (often) possible to convert existing cases to BFC, it is not possible to reverse the procedure.

Cartesian/Polar cases which cannot be converted are those which use geometries other than cuboids.

### Displaying the Grid

Turning the mesh toggle on the hand-set ON by clicking on the Grid mesh button causes the current grid to be displayed on the graphics image:

Image: GRID

The grid is displayed on a plane at the probe location. By default the plane is normal to the co-ordinate axis nearest the view direction. For example, if the view direction is along, or close to, +Z, the X-Y plane will be displayed. As the probe is moved or view directions are changed, the grid display will also change to follow.

To manually select the displayed plane, click the pull-down arrow next to the mesh toggle

and choose the required plane. This plane will now be displayed regardless how the view direction is changed, until another direction or 'Auto' is chosen. The position of the plane is still controlled by the probe location.

### The Default Grid - Auto Meshing

The grid-creation actions which the VR-Editor takes by default relate to the three aspects the Cartesian or polar grid, namely:
1. locating the boundaries of the regions;
2. determining the numbers of intervals in each region; and
3. choosing the type and numerical exponent of interval non-uniformity.

The orange lines shown in the above image are region boundaries. These are automatically created to match the edges of the object bounding boxes (see VR-Editor Object Dialogs - Object Size, Object Positioning), as a consequence of the default ticking of each of the x, y and z options in the 'object affects grid' menu shown below.

If the user removes the ticks, no region is created; nor, of course, are the intervals within them.

This is sometimes desirable; for the user may know that the objects in question, although truly present, can have negligible influence on phenomena of interest. If so, it is time-wasting to allow the grid to be refined around such objects. See Advice on Grid Settings below.

As objects are introduced, removed and re sized, the region lines will adapt to match the object layout.

The blue lines are 'ordinary' grid lines. By default, these are distributed by the auto-mesher according to the current set of rules. These are:

1. The maximum cell size is not allowed to exceed a set fraction (0.05 by default) of the domain size.
2. The ratios between the sizes of the first cell in the current region and the last cell in the previous region, and the last cell in the current region and the first cell in the next region, are not allowed to exceed a set limit (1.5 by default).
3. If the ratios are exceeded, the number of cells in that region is increased, and the spacing is set according to a geometrical or power-law progression using a set expansion ratio (geometrical 1.2 by default), until either the ratio criterion is satisfied at both ends of the region, or the cells at both ends are below a set minimum fraction (0.005 by default) of the domain size.

Note that if there are no region boundaries in a direction, the auto-meshing will usually assume that only one cell is required in that direction. This is appropriate for 2D cases in which all objects cover the whole domain in the third direction.

If there is an INLET, FAN, OUTLET or PLATE object on the edge of the domain, the auto-meshing will assume that grid is required in that direction, even if there is only one region.

Users should always inspect the grid visually to satisfy themselves that it is appropriate to their purposes. The default auto-mesh settings may sometimes be found to have created a rather coarse grid, suitable for first-exploration runs but not for realistic simulations. It is equally possible that they have created too fine a grid; or one that is fine in the wrong places. 'Object affects grid?' is too important a question for users to disregard.

In most cases auto-set grids will require adjustment, either by changing the auto-grid rules or by manual adjustment before the final runs are made.

### Modifying the Grid

Clicking on the mesh with the left mouse button whilst the grid mesh display is on will show the Grid Mesh Settings Dialog. The selected regions will be highlighted in blue, as shown below. The cursor was in the top-right corner of the mesh when the left mouse-button was clicked.

Image: GRID Mesh SETTINGS - Auto

Entering a different region number in the 'Modify region' input box will cause that region to be highlighted instead.

By default, the auto-meshing feature is turned on, as shown in the image above.

The grayed-out values cannot be changed from this dialog unless the auto-mesh is turned off for any direction, as shown here:

Image: GRID Mesh SETTINGS - Manual

Settings on this dialog which are common to auto-mesh on or off are:

• Co-ordinate system: Toggles between Cartesian, cylindrical-polar and Body-Fitted (BFC).
• Time dependence: Toggles between Steady and Transient
• Inner radius (only for cylindrical-polar): Sets the inner radius for a cylindrical-polar grid.
• Time step settings (only for transient): Displays a dialog for managing the time-step distribution.
• Partial solids treatment: This activates the special treatment of partially-blocked cells, PARSOL.
• Partial solids treatment settings: This displays a dialog from which the minimum and maximum fluid volume fractions for PARSOL can be set. Any cell in which the fluid volume fraction is below the minimum value is considered fully-blocked, and any cell in which it is above the maximum is considered full-open. The default values are 0.001 and 0.999. Resetting these to, say, 0.01 and 0.99 can eliminate very small fluid cut-cells, which can lead to unrealistic pressures.
• Domain size: Sets the total extent of the domain in the X, Y and Z directions. In cylindrical-polar co-ordinates, the X size is set in radians.
• Tolerance: Sets the tolerance in each direction (in the same units as the domain dimension, usually meters) used for matching the grid to objects.

Changing the Auto-mesh Rules

When the auto-grid setting is ON or AUTO, the grid in that direction is generated based on certain rules. These are:

1. The maximum cell size is not allowed to exceed a set fraction of the domain size.
2. The ratios between the sizes of the first cell in the current region and the last cell in the previous region, and the last cell in the current region and the first cell in the next region, are not allowed to exceed a set limit.
3. If the ratios are exceeded, the number of cells in that region is increased, and the spacing is set according to a geometrical or power-law progression using a set expansion ratio, until either the ratio criterion is satisfied at both ends of the region, or the cells at both ends are below a set minimum fraction of the domain size.

When the grid is automatically generated, the normal grid settings in that direction are inactive. To modify one of the regions, the automatic grid must be turned off.

To change the auto-mesh settings for any direction, click 'Edit all regions in' on the Grid Mesh Settings dialog for the direction in question. The following dialog will appear:

Image: X Direction Auto-mesh Settings

The grayed-out values cannot be changed manually unless the auto-meshing is turned off. They reflect the settings generated by the current auto-mesh control parameters.

The 'Reg'(ion) button causes the selected region to be highlighted in in blue in the graphics display. You may have to drag the dialogs to the side to get a clear view of the mesh display.

The following settings influence the auto-meshing:

• Auto grid settings: ON / OFF Toggles the auto-meshing on and off for this direction. The default is on.
• Set defaults: Resets all values to their defaults. These are:

Version 2017 V2 onwards:

Min cell factor 0.01
Max cell factor 1.0
Max size ratio 1.5
Expansion power 1.1
Expansion form Geometric Progression
Boundaries Auto

Earlier Versions

Min cell factor 0.005
Max cell factor 0.05
Max size ratio 1.5
Expansion power 1.2
Expansion form Geometric Progression
Boundaries Off (On for Flair)
• Min cell factor: This sets the smallest cell size allowed as a fraction of the domain size in that direction. The default is 1.0%.
• % Domain: toggles the minimum cell size between a % of the domain size and an absolute size.
• Boundary - Low: When set to OFF, the grid in the first region expands backwards from the end of the first region towards the domain boundary. This would be appropriate if the domain boundary were, say, a fixed-pressure zone, or a symmetry plane where nothing much happens.

When set to ON, the grid in the first region expands symmetrically from the domain boundary and the first region boundary. This would be appropriate if the domain boundary were a plate or inlet, where changes in flow are expected.

When set to AUTO, the grid expands symmetrically if a PLATE, INLET, FAN, OUTLET or WIND_PROFILE object is detected at the start of the domain. If a WIND object is detected, the grid will expand symmetrically from the ground and side boundaries.

• Boundary - High: When set to OFF, the grid in the last region expands forwards from the start of the last region towards the domain boundary. This would be appropriate if the domain boundary were, say, a fixed-pressure zone, or a symmetry plane where nothing much happens.

When set to ON, the grid in the last region expands symmetrically from the domain boundary and the start of the last region. This would be appropriate if the domain boundary were a plate or inlet, where changes in flow are expected.

When set to AUTO, the grid expands symmetrically if a PLATE, INLET, FAN, OUTLET or WIND_PROFILE object is detected at the end of the domain. If a WIND object is detected, the grid will expand symmetrically from the ground and side boundaries.

• Show mesh quality parameters: This displays a dialog similar to the one shown below:

which shows parameters indicating the 'quality' of the mesh:
Minimum cell-size ratio.
Maximum cell-size ratio.

These are the ratios between the size of the first cell in a region and the last cell in the previous region, and the last cell in a region and the first cell in the next region. They should both be within the set limits.

Minimum region-boundary cell-size
Maximum region-boundary cell-size

These are the smallest and largest cells at either end of a region. They should both be larger than the set minimum value, unless the region itself is smaller than the limit.

• Advanced Settings: Displays a dialog on which further, less commonly needed, mesh-control values can be set.

• Init cell fraction: This sets the initial cell size as a fraction of the domain size in that direction. The default is 100.0%, which means the mesh starts with one cell per region, and is then refined until the conditions are met.
• % Domain: By default, the minimum and initial cell factors are set as fractions of the domain size. This makes it easier to handle any domain size. When clicked, the setting changes to 'Size'. The minimum and initial cell sizes are now set as physical sizes in metres.
• Max size ratio: When the ratio of the size of the first cell in the current region to the last cell in the previous region, or the last cell in the current region to the first cell in the next region, is greater than this (1.5 by default), the number of cells in the current region will be increased until either:
• the ratios at both ends are satisfied; or
• the cells at both ends are smaller than the minimum fraction of the domain size.

As well as progressively increasing the number of cells in this region, the cells are distributed using a geometric or power-law expansion. To keep the cell distribution with the region uniform the expansion power should be set to 1.0.

The grid is expanded using a symmetrical expansion, except in the first and last regions, where there is choice of symmetrical expansion or expansion from the internal region boundary to the domain edge.

• Expansion Power: This sets the expansion power used to adjust the grid with a region so as to satisfy the cell-size ratios at the region ends. The default value is 1.2.

A power of 1 will keep the grid in the region uniform, but may use a lot of cells. Powers > 1 will reduce the number of cells, but will introduce non-uniformity.

• Form: The grid can expand using a geometrical progression, or a power-law expansion. The default geometrical progression gives a faster change in grid-size for the same power, thus keeping the number of cells down.
• Reset defaults: This sets all the auto-mesh parameters to their default values, as described above.

Clicking on the mesh with the right mouse button whilst the grid mesh display is on will show the interactive Auto Meshing Dialog.

Moving the slider to the left will reduce the minimum cell fraction or size and hence increase the number of cells in the selected direction. Moving it to the right will increase the minimum cell seize and hence reduce the number of cells. Alternatively, an exact value for the minimum size can be entered into the data input box, and the number of cells will be updated. The box showing the number of cells is display-only. It is not possible to directly enter a specific number of cells.

Manually Changing the Grid by Region

When the auto-meshing for a direction is turned off, the number of cells in any region, and the distribution within any region, can be set by clicking on the region to be modified. The initial region settings will be those created by the auto-mesher. Clicking on X region 3 and Y region 1 of the example shown previously, for example, brings up the dialog box shown below:

Image: GRID Mesh SETTINGS - manual

• Number of cells: Sets the total number of cells in the X, Y and Z directions. If all regions are 'Set', this value cannot be changed directly as there are no 'Free' regions to accommodate the change.
• Tolerance: Sets the tolerance used for this direction. Object edges closer together than this will not generate separate regions.
• Number of regions: This displays the current number of regions in each direction. This can only be changed by modifying objects or modifying the tolerance.
• Modify region: This is the number of the region selected for modification. In the diagram above, an X-Y plane is displayed, and the cursor was clicked into the third region in X, and the first region in Y. To modify a different region, enter its number here directly and click 'Apply', or click OK, then click on the new region.
• Size: This displays the size (in meters or radians) of the region selected for modification. The size of a region can only be changed by modifying objects or modifying the tolerance.
• Distribution: This toggles between Power law and Geometrical progression. It controls how the cells within the region are spaced.
• Cell Power: This toggles between Free and Set. Free means that the number of cells can be automatically adjusted as the total number of cells is changed, so as to keep the grid as uniform as possible. Set means that the number of cells in this region, and their distribution, have been set by the user and cannot be automatically changed.
• Cells in region: This initially displays the number of cells allocated to this region by the automatic meshing algorithm. The number of cells in this region can be changed by typing in a different value. Cells will be taken from, or distributed amongst other 'Free' regions to keep the total number constant.
• Power/ratio: This sets the expansion power, or geometric expansion common ratio. The default setting of 1.0 gives a uniform grid. Positive values mean that the expansion goes from the start of the region towards the end, negative values mean the expansion starts at the end and goes to the beginning.
• Symmetric: This toggles between No and Yes. If Yes, the expansion specified by Distribution and Power/ratio is applied symmetrically from each end of the region.
• Edit all regions: This displays a dialog which shows all the region settings in a particular direction and allows them to be changed. This is the easiest way to change the settings for several regions.

The diagram below shows a simple three-part grid. Region 1 has 10 cells with a power of -1.5. Region 2 has 10 cells with a symmetric power of 1.5, and region 3 has 10 cells with a power of +1.5.

Image: DIAGRAM 1

The next diagram shows the same grid, but with geometrical expansions in all three regions:

Image: DIAGRAM 2

The two most important pieces of advice to the user who has allowed the grid to be created by the automesher are:

1. Look at the grid which has been created; and
2. Consider critically whether the automesher has placed the finer-grid regions in places which are of most importance to the user.
The answer to the last question will most often be negative; for how can the satellite know what it has not been told?

An example is shown by the following picture which shows the automeshed grid for the simulation of what happens when a car catches fire in a car park. The car, one might suppose, is of greatest interest, and so should have the finest grid. However automesher has paid attention to the numerous small ventilation apertures in the car-park wall; and, precisely because of their smallness, has created a grid which fits them.

Having recognised that automeshing has created a grid which, because it is very fine, will require large computer times but ignores his needs, what should the user do? The answer depends upon his expertise level.

Many would do best to seek from CHAM, or from their in-house experts, a Q1 file which corresponds better to reality and to their desires. Do-it-yourselfers however, who wish be their own in-house experts, should proceed as follows:

1. Clarify precisely what is the purpose of the simulation.
2. Use their general knowledge of physics (or that of their advisers) to determine what geometrical aspects of the scenario are most likely to influence the simulation outcomes which bear on that purpose.
3. Judiciously switch off the 'Object affects grid' attributes of selected objects to prevent the creation of regions where they are not needed.
4. Judiciously add NULL objects to create extra regions where they appear to be needed but have not been created by any current object.
5. Judiciously simplify the problem by, for example, replacing many small inlets with an single larger equivalent.

The actions will now be discussed in more detail.

Distinct purposes might be:

1. To simulate the car-burning process, i.e. to calculate its rate of progress, taking account of the rate of mass transfer of oxygen to its fuel-bearing parts.etc.
2. Having instead specified the rate of burning to establish whether the rate of air and smoke extraction through ventilation apertures is sufficient to draw away all that is produced, or alternatively will allow smoke to accumulate if the garage space or perhaps even to spread, and cause further conflagrations, elsewhere.
3. To establish how low should be the external pressure applied to the ventilation apertures so as to ensure that all the smoke produced will be extracted.

Whichever is the purpose, the grid which automesher created is totally unsuitable.

• For (a) the finest-grid region should be concentrated around the car.
• For (b) a much coarser grid, spread uniformly through the garage space would have sufficed.
• For (c) a fine grid concentrated around and within just one of the ventilation devices would be needed, its detailed internal geometry being taken into account.

Let us suppose that inquiry shows that whoever commissioned the simulation had purpose (b) in mind, and that the scenario specification consisted of:

• the amount of smoke generated by the burning car as a function of time; and
• the rate of extraction of air through each ventilation aperture in cubic meters per second.

If that is the case, it must be admitted that a CFD simulation is not truly needed at all; for a back-of-envelope sum will indicate the ratio of the rates of smoke production and extraction.

However, if CFD is to be used, a 20-by-20-by-20 grid will suffice to demonstrate that the back-of-envelope sum was not far wrong.

How would the extractor devices be represented in such a model? Fixed-mass-flux patches at the walls would be quite good enough.

### Body-Fitted Co-ordinates

All BFC library cases, and all user-generated BFC cases can be loaded into PHOENICS-VR.

The possible methods of grid generation are:

• The BFC Menu in the VR-Editor.

### Displaying the Grid

Turning the mesh toggle on the hand-set ON by clicking on the Grid mesh button causes the current grid to be displayed on the graphics image:

Image: BFC Grid

The grid is displayed on a plane at the probe location. The plane is normal to the co-ordinate axis nearest the view direction. For example, if the view direction is along, or close to, +Z, the X-Y plane will be displayed. As the probe is moved or view directions are changed, the grid display will also change to follow.

In a multi-block grid, the grid will be displayed in the block containing the probe.

#### Moving the Probe

In BFC, the probe can only be moved from cell-centre to cell-centre. The probe location is always in IX, IY, IZ.

In a multi-block case, these are shown in 'big' grid co-ordinates, not in local block co-ordinates. Any cell can be moved to directly by typing the cell IX,IY,IZ values into the hand-set.

Note the colouring of the block containing the probe:

• The blue axis is the I axis
• The green axis is the J axis
• The yellow axis is the K axis

In a complex multi-block case, this will help in identifying which way to move the probe.

To move the probe from one block to the next, move up to a linked face, and then step through it by continuing to move in that direction.

The axis colouring will jump to the next block. If the Move probe button is kept pressed, and the IJK orientation of the next block is different, the probe may take off in an unexpected direction - it may even jump back to the previous block if the axes are reversed!

### Modifying the Grid

#### Creating a Grid with the PHOENICS Grid Generator

To enter the Grid Generator, turn the grid display ON by clicking on the Grid mesh button. Click on the grid anywhere in the domain. The BFC Menu will appear.

The main functions on the BFC Menu are:

• Dimension - set the total number of cells in each direction.
• Points - Create new points, move or delete existing points.
• Lines - Create new lines, modify or delete existing lines. Lines can be:
• Straight lines joining two points
• Arcs passing through three points
• Spline curves passing through a number of points
• Surfaces - Create surface grids on four-sided frames
• Volumes - Create volume grids by:
• Extruding a surface
• Rotating a surface
• Interpolating between two surfaces
• Filling in a block defined by six surfaces
• Delete All - delete all gridding elements
• Display - Control the grid display

For those users not familiar with the BFC grid generator, several tutorials are available, reached from POLIS / Learn / BFC tutorials. There is also a lecture, reached from POLIS / Learn /Lectures describing... / Body-fitted co-ordinates; introduction describing the fundamentals of BFC Grid generation.

The images above show the geometry created by the BFC tutorials.

#### Importing a Grid Created by an External Grid Generator

Whichever external grid generator is used, the outcome will be a skeleton Q1, and at least one grid file. If the case is a multi-block case, there will be one grid file for each block.

The skeleton Q1 file will contain a READCO command to read the grid file(s), and instructions for linking the blocks.

An example skeleton file for a single-block grid stored in the grid file grid1 must contain at the very least:

```TALK=T; RUN(1,1)
BFC=T
STOP```

It may also contain (M)PATCH statements locating boundary conditions, and also COVAL commands setting inlet values.

In GeoGrid (Note: this software is no longer available, but the images are shown for illustrative purposes) the name of the Q1 will be project.Q1, where project is the name of the GeoGrid project.

To import this into PHOENICS-VR, click on File - Open existing case from the top bar of the main VR-Editor/Viewer graphics window. Double-click on project.Q1 to open it in PHOENICS-VR.

The first image shows a very simple 3-block example in GeoGrid.

One inlet (purple, on the left) and one outlet (blue, on the right) have been designated.

The second image shows the same case imported into PHOENICS-VR.

Note: The grid files must be in the current working directory, OR the READCO(filename+) command must be modified to include the path to where they are.

If a grid generator other than GeoGrid is used, please ensure that the skeleton Q1 is copied to the working directory as case.Q1, together with all the necessary grid files. Use File - Open existing case to open case.Q1.

#### Creating a Grid with PIL

If the user is familiar with the PIL GSET suite of commands, the Q1 can be edited to create the grid in any convenient way. PHOENICS-VR will recognise and retain all GSET commands.

It does not recognise the older SETPT, DOMAIN, SETLIN or MAGIC commands. If the grid is built with these, or some of these commands are used to smooth parts of the grid, use the DUMPC(name) command to write out a grid file, and supply PHOENICS-VR with a  Q1 that just contains:

```TALK=T;RUN(1,1)
BFC=T
STOP```

The final result should be a file called case.Q1, which either contains the required GSET commands, or a READCO to read an existing grid file (or files).

#### Modifying the Grid for an Existing Case

Often, once a case has been set up and run, it becomes obvious that the original grid is inadequate. It may be generally too coarse, or grid may be concentrated in the wrong places.

If the grid was generated in the PHOENICS Grid Generator, this can be used to modify the grid as required. On exit from the Grid Generator, most of the objects will have to be re-located and re-sized , as they will still be in their original IJK positions.

If the grid was generated externally, in many cases this can be avoided. Re-enter the grid generator, say GeoGrid, and modify the grid as required. Save the PHOENICS output file with a different name to that used for the original grid.

In VR-Editor, click on Main Menu - Geometry - Read new geometry from file. This will bring up a file browsing window, which will allow the selection of the new Q1 written by the grid generator. The new grid will be read in, and boundary condition locations will be remapped to the new grid when Open is clicked. Note that only boundary conditions common to both grids will be remapped.

### Time Grids

To simulate transient behaviour, time is discretised in a similar way to the space dimensions. The Earth solver produces a solution for each step in time before advancing to the next step. An extra term is automatically added to the equations solved, which expresses the influence of the previous time-step.

The default equation formulation is implicit, so there are no extra stability criteria to satisfy when setting the size of the time-steps. If the steps are too large, the details of the transient behaviour will not be picked up.

In Transient mode, objects representing sources will have additional dialogs allowing start and end times to be set.

#### Switching Between Steady and Transient

To switch from Steady to Transient, click on the Steady button on the   Grid Mesh Settings dialog,

or in BFC,

on the BFC menu dialog. A new button labeled Time Steps will appear.

The Steady button will now be labeled Transient. To switch back to Steady, click on Transient.

#### Setting the Time-Step Distribution

Clicking on the Time Steps button displays the Time Step Settings dialog.

IMAGE: Time Step Settings dialog

Time can be divided into regions by the Split Regions button. Within each time region, the number of time steps can be set, together with a geometrical or power-law size distribution.

#### Saving Intermediate Results

To save intermediate results for plotting in the VR-Viewer or any other post-processor, click on 'Main menu', 'Output', 'Field dumping'. The following dialog will appear:

IMAGE: Transient Field dumping dialog

Set the step frequency for dumping. If dumping is not to start at step 1, or finish before the and last time step, the 'Limits' dialog allows the first and last steps to be set. Set a start letter for the intermediate output files. A start letter of A, and a dump frequency of 1 will result in files called A1, A2, A3 etc being dumped at the end of each time step.

The letter Q should not be used, as the file dumped on step 1 will overwrite the Q1 input file!

The size of the intermediate files can be reduced by choosing not to dump each variable to the file. Changing the Y to an N in the OUTPUT 3 DUMP line will prevent that variable from being written to the intermediate file. If the property-marked variable, PRPS, is so excluded, Viewer will not be able to determine which cells are blocked. Depending on which variables are excluded, it may not be possible to restart the calculation from the intermediate files. All variables are written to the final solution files (PHIDA or PHI and PBCL.DAT) regardless of the dump settings.

If the case is 2D in X and Y, the start letter can be left blank. In this case, a special output file called PARADA or PARPHI is written, in which the results of each time step are saved as a Z plane. In the viewer, sweeping through Z in effect sweeps through time.

To print flow fields to the RESULT file every time step, go to 'Main menu', 'Output', 'Field printout', and set NTPRIN to 1. Note that NTPRIN may be displayed on the next page of the menu. Click 'Page down' to display settings on the next page.

Note that the intermediate output files are optionally saved by 'File', 'Save as a Case', and restored by 'File', 'Open existing case'. The output files can be big and numerous, so it may be better to either ZIP them up, or copy them to a CD for safe-keeping.

The intermediate files can be selected for plotting in the Viewer by choosing 'Use intermediate step files - Yes' on the 'File names' dialog displayed when the Viewer starts.

#### Restarting Transient Cases

There are two main possibilities:

1. Restarting to continue with more time steps
2. Restart from some intermediate point and re-calculate some steps.

To restart and continue the run, bring up the Time step setting dialog. In the 'Time at end of last step' box, enter the new extended end time of the run. Leave 'Time at start of step 1' at zero. In the 'Last step number' box, enter the new total number of steps. In the 'First step number' box, enter the previous last step+1. A dialog will appear asking if a restart is to be activated. Click 'Yes'. The restart will be activated, and the names of the restart files will be deduced from the start letter chosen for saving the intermediate fields.

Please check that the names are correct. To force a restart from the final solution files which are guaranteed to contain all the solved and stored variables, set the 'Solution file' to phida (or phi) and the 'Cut-cell file' to pbcl.dat.

For example, the original run did 100 steps from time 0.0s to 10.0s ( thus giving time steps of 0.1s each). It is now desired to do the next 10.0s with the same time step size. Set 'Time at end of last step' to 20.0, 'Last step number' to 200, and 'First step number' to 101. To activate the restart, click on 'Yes' when asked about activating the restart.

To restart from an intermediate step, say step 50, just set 'First step number' to 51. A dialog will appear asking if a restart is to be activated. Click 'Yes'. The restart will be activated, and the names of the restart files will be deduced from the start letter chosen for saving the intermediate fields.

IMAGE: Time Step Settings dialog for restart

The names of the restart files are also displayed on (and can be set from) the 'Main Menu', 'Initialisation' panel. An active restart is shown by all the initial values (FIINIT) being shown as READFI.