7.3. Additional POST1 Postprocessing

The following additional POST1 postprocessing techniques are covered in this section:

7.3.1. Rotating Results to a Different Coordinate System

Results data, calculated during solution, consist of displacements (UX, UY, ROTX, etc.), gradients (TGX, TGY, etc.), stresses (SX, SY, SZ, etc.), strains (EPPLX, EPPLXY, etc.), etc. These data are stored in the database and on the results file in either the nodal coordinate system (for the primary, or nodal data) or the element coordinate system (for the derived, or element data). However, results data are generally rotated into the active results coordinate system (which is by default the global Cartesian system) for displays, listings, and element table data storage.

Using the RSYS command, you can change the active results coordinate system to global cylindrical (RSYS,1), global spherical (RSYS,2), any existing local coordinate system (RSYS,N, where N is the local coordinate system number), or the nodal and element coordinate systems used during solution (RSYS,SOLU). If you then list, display, or operate on the results data, they are rotated to this results coordinate system first. You may also set the results system back to global Cartesian (RSYS,0).

The default coordinate system for certain elements, notably shells, is not global Cartesian and is frequently not aligned at adjacent elements.

The use of RSYS,SOLU with these elements can make nodal averaging of component element results, such as SX, SY, SZ, SXY, SYZ, and SXZ, invalid and is not recommended.

Tthe following figure illustrates how displacements are reported for several different RSYS settings:

Figure 7.19:  Rotation of Results by RSYS

Rotation of Results by RSYS

The displacements are in terms of the nodal coordinate systems (which are always Cartesian systems), but issuing the RSYS command causes those nodal systems to be rotated into the specified system. For example, RSYS,1 causes the results to be rotated parallel to the global cylindrical system such that UX represents a radial displacement and UY represents a tangential displacement. (Similarly, AX and AY in a magnetic analysis and VX and VY in a fluid analysis are reported as radial and tangential values for RSYS,1.)


Caution:  Certain element results data are always output in the element coordinate system regardless of the active results coordinate system. These are miscellaneous result items that you would normally expect to be interpreted only in the element coordinate system. They include forces, moments, stresses, and strains for beam, pipe, and spar elements, and member forces and moments for some shell elements.


In most circumstances, such as when working with a single load case or during linear combinations of multiple load cases, rotating results data into the results coordinate system does not affect the final result values. However, most modal combination techniques (PSD, CQC, SRSS, etc.) are performed in the solution coordinate system and involve squaring operations. Since the squaring operation removes the sign associated with the data, some combined results may not appear as expected after being rotated into the results coordinate system. In these cases, RSYS,SOLU is on by default in order to keep the results data in the solution coordinate systems. No other coordinate system may be used.

As an example of when you would need to change the results coordinate system, consider the case of a cylindrical shell model, in which you may be interested in the tangential stress results. The SY stress contours before and after results coordinate system transformation are shown below for such a case.

PLNSOL,S,Y           ! Display a: SY is in global Cartesian system (default)
RSYS,1
PLNSOL,S,Y           ! Display b: SY is in global cylindrical system

See the RSYS and PLNSOL command descriptions for further information.

Figure 7.20:  SY in Global Cartesian and Cylindrical Systems

SY in Global Cartesian and Cylindrical Systems

Plot 1 (top) illustrates SY in global Cartesian system. Plot 2 (bottom) illustrates SY in global cylindrical system (note that nodes and elements are still in global Cartesian system).


In a large-deformation analysis--for example, if you have issued the NLGEOM,ON command and the element has large-deflection capability--the element coordinate system is first rotated by the amount of rigid body rotation of the element. Therefore, the component stresses and strains and other derived element data include the effect of the rigid body rotation. The coordinate system used to display these results is the specified results coordinate system rotated by the amount of rigid body rotation.

The exceptions to this are continuum elements such as PLANE182, PLANE183, SOLID185, SOLID186, SOLID187, SOLID272, SOLID273, and SOLID285. For these elements, the output of the element component results is by default in the initial global coordinate system, and all component result transformations to other coordinate systems will be relative to the initial global coordinate system.

The primary data (for example, displacements) in a large-deformation analysis do not include the rigid body rotation effect, because the nodal coordinate systems are not rotated by the amount of rigid body rotation.

7.3.2. Performing Arithmetic Operations Among Results Data

The earlier discussion of operations among path items was limited to items mapped on to a path. Using commands from the POST1 CALC module, you can perform operations among any results data in the database. The only requirement is that you must use the element table. The element table serves as a "worksheet" that allows arithmetic operations among its columns.

The procedure to do calculations among results data requires three simple steps:

  1. Issue the ETABLE command to bring one or more result items into the element table or "worksheet."

  2. Perform the desired arithmetic operations via commands from the CALC module (SADD, SMULT, SEXP, etc.).

  3. Review the outcome of the operations via PRETAB or PLETAB.

The ETABLE command moves specified results data for all selected elements into the element table. One value is stored per element. For example, if you select 10 elements and issue the command shown below, an average UX value is calculated for each element from the nodal displacements and stored in the element table under the "ABC" column.

ETABLE,ABC,U,X

The element table will be ten rows long (because only ten elements were selected). If you now want to double these displacements, the command (SMULT) to do so is:

SMULT,ABC2,ABC,,2

The element table now has a second column, labeled ABC2, containing twice the values in column ABC. To list the element table, simply choose PRETAB.

Example 7.13:  PRETAB Output
 PRINT ELEMENT TABLE ITEMS PER ELEMENT
***** POST1 ELEMENT TABLE LISTING *****                                      
 
   STAT    CURRENT     CURRENT 
   ELEM    ABC         ABC2    
      1   .21676      .43351    
     11   .27032      .54064    
     21   .23686      .47372    
     31   .47783      .95565    
     41   .36171      .72341    
     51   .36693      .73387    
     61   .13081      .26162    
     71   .50835      1.0167    
     81   .35024      .70049    
     91   .25630      .51260    
 MINIMUM VALUES
 ELEM        61          61
 VALUE    .13081      .26162    
 MAXIMUM VALUES
 ELEM        71          71
 VALUE    .50835      1.0167    

Another example of arithmetic operations is to calculate the total volume of selected elements. To do so, you might store all element volumes in the element table, select the desired elements, and sum them via the SSUM command:

ETABLE,VOLUME,VOLU           ! Store element volumes (VOLU) as VOLUME
ESEL,...                     ! Select desired elements
SSUM                         ! Calculate and print sum of VOLUME column

See the ETABLE, ESEL, and SSUM command descriptions for further information.

7.3.2.1. Hints and Recommendations

All operation commands (SADD, SMULT, SSUM, etc.) work only on the selected elements.

The program does not update element table entries automatically when a different set of results is read into the database. An element table output listing displays headers which indicate the status of each column relative to the current database. CURRENT indicates that the column data is from the current database, PREVIOUS indicates that it is from a previous database, and MIXED indicates that it results from an operation between previous and current data. (Once a column is labeled mixed, it will not change status unless you erase or redefine it with all elements selected.) The following commands cause column headers to change from CURRENT to PREVIOUS:

The ETABLE,REFL option, which refills (updates) the element table with values currently in the database, does not affect calculated items. In the above double-the-UX example, if you read in a different set of results and then issue ETABLE only the ABC column will be updated ("current" status). The ABC2 column remains as is (keeps its "previous" status).

The program does not update the element table automatically after a new SET command. You can use that behavior to good advantage, such as comparing element results between two or more load steps, or even between two or more analyses.

The following CALC module commands apply to calculations using the element table:

  • SABS -- Causes absolute values to be used in subsequent element table operations.

  • SADD -- Adds two specified columns in the element table.

  • SALLOW -- Defines allowable stresses for safety factor calculations.

  • SEXP -- Exponentiates and multiplies two columns in the element table.

  • SFACT -- Defines which safety factor calculations will be performed during subsequent display, select, or sort operations.

  • SFCALC -- Calculates safety factors (for ETABLE items).

  • SMAX -- Compares and stores the maximum of two columns.

  • SMIN -- Compares and stores the minimum of two columns.

  • SMULT -- Multiplies two specified columns in the element table.

  • SSUM -- Calculates and prints the sum of each element table column.

  • TALLOW -- Defines the temperature table for safety factor calculations.

  • VCROSS -- Calculates the cross product of two vectors stored in the element table.

  • VDOT -- Calculates the dot product of two vectors stored in the element table.

7.3.3. Creating and Combining Load Cases

In a typical postprocessing session, you read one set of data (load step 1 data, for instance) into the database and process it. Each time you store a new set of data, POST1 clears the results portion of the database and then brings in the new results data. If you want to perform operations between two entire sets of results data (such as comparing and storing the maximum of two sets), you need to create load cases.

A load case is a set of results data that has been assigned an arbitrary reference number. For instance, you can define the set of results at load step 2, substep 5 as load case number 1, the set of results at time = 9.32 as load case number 2, and so on. You can define up to 99 load cases, but you can store only one load case in the database at a time.


Note:  You can define a load case at any arbitrary time by via the SET command (to specify the time argument) and then via LCWRITE to create that load case file. The values will be a linear interpolation of the results already available before and after your specified time.


A load case combination is an operation between load cases, typically between the load case currently in the database and a load case on a separate results file (or on the load case file, explained later). The outcome of the operation overwrites the results portion of the database, which permits you to display and list the load case combination.

A typical load case combination involves the following steps:

  1. Define load cases via the LCDEF command.

  2. Read one of the load cases into the database via the LCASE command.

  3. Perform the desired operation via the LCOPER command.

As an example, suppose the results file contains results for several load steps, and you want to compare load steps 5 and 7 and store the maximum in memory. The commands to do this would look like this:

LCDEF,1,5               ! Load case 1 points to load step 5 
LCDEF,2,7               ! Load case 2 points to load step 7
LCASE,1                 ! Reads load case 1 into memory
LCOPER,MAX,2            ! Compares database with load case 2 and stores the
                        !  maximum in memory 

The database now contains the maximum of the two load cases, and you can perform any desired postprocessing function.


Note:  Load case operations (LCOPER) are performed only on the raw solution results in the solution coordinate system.


The solution results are:

  • Element component stresses, strains, and nodal forces in the element coordinate systems

  • Nodal degree-of-freedom values, applied forces, and reaction forces in the nodal coordinate systems

To have a load case operation act on the principal/equivalent stresses instead of the component stresses, issue the SUMTYPE,PRIN command.

It is important that you know how load case operations are performed. Many load case operations, such as mode combinations, involve squaring, which renders the solution results unsuitable for transformation to the results coordinate system, typically the Global Cartesian, and unsuitable for performing nodal or element averages. A typical postprocessing function such as printing or displaying average nodal stresses (PRNSOL, PLNSOL), for example, involves both a coordinate system transformation to the results coordinate system and a nodal average. Furthermore, unless SUMTYPE,PRIN has been requested, principal/equivalent stresses are not meaningful when computed from squared component values.

To view correct mid-surface results for shells (SHELL,MID), use KEYOPT (8) = 2 (for SHELL181, SHELL208, SHELL209, SHELL281, or ELBOW290). These KEYOPT settings write the mid-surface results directly to the results file, and allow the mid-surface results to be directly operated on during squaring operations, instead of averaging the squared TOP and BOTTOM results.

You should therefore use only untransformed (RSYS,SOLU), unaveraged (PRESOL, PLESOL) results whenever you perform a squaring operation, such as in a spectrum (SPRS,PSD) analysis.

Issue the FORCE command prior to any load case operations to insure that the forces are correctly summed before the operation. Note that once a force type has been combined, the other components are no longer available and will be zero.

7.3.3.1. Saving a Combined Load Case

By default, the results of a load case combination are stored in memory, overwriting the results portion of the database. To save these results (for later review or for subsequent combinations with other load cases), use one of the following methods:

  • Write the data to a load case file.

  • Append the data to the results file.

Issue the LCWRITE command to write the load case currently in memory to a load case file. The file is named Jobname.Lnn, where nn is the load case number you assign. Using nn in subsequent load case combinations will refer to the load case stored on the load case file.

Example 7.14:  Use of the LCWRITE Command
LCDEF,1,5               ! Load case 1 points to load step 5 
LCDEF,2,7               ! Load case 2 points to load step 7
LCDEF,3,10              ! Load case 3 points to load step 10
LCASE,1                 ! Reads load case 1 into memory
LCOPER,MAX,2            ! Stores max. of database and load case 2 in memory 
LCWRITE,12              ! Writes current load case to Jobname.L12
LCASE,3                 ! Reads load case 3 into memory
LCOPER,ADD,12           ! Adds database to load case on Jobname.L12
LCDEF,STAT              ! Results in the following output:

Example 7.15:  Output from LCDEF,STAT
 LOAD CASE=  1  SELECT= 1  ABS KEY= 0  FACTOR=  1.0000    
  LOAD STEP=     5  SUBSTEP=     2  CUM. ITER.=     4  TIME/FREQ=  .25000    
  FILE=beam.rst                                          
   Simply supported beam                                                  
                                                                          
 LOAD CASE=  2  SELECT= 1  ABS KEY= 0  FACTOR=  1.0000    
  LOAD STEP=     7  SUBSTEP=     3  CUM. ITER.=    10  TIME/FREQ=  .75000    
  FILE=beam.rst                                          
   Simply supported beam                                                  
                                                                          
 LOAD CASE=  3  SELECT= 1  ABS KEY= 0  FACTOR=  1.0000    
  LOAD STEP=     10  SUBSTEP=    2  CUM. ITER.=    12  TIME/FREQ=  1.0000    
  FILE=beam.rst                                          
   Simply supported beam                                                  
                                                                          
 LOAD CASE= 12  SELECT= 1  ABS KEY= 0  FACTOR=  1.0000    
  LOAD STEP=     0  SUBSTEP=     0  CUM. ITER.=     0  TIME/FREQ=  .00000E+00
  FILE=beam.l12                                          
   Simply supported beam                                                  
                                                                          

The RAPPND command appends the load case currently in memory to the results file. The data are stored on the results file just like any other results data set except that:

  • You (not the program) assign the load step and substep numbers used to identify the data.

  • Only summable and constant data are available by default; non-summable data are not written to the results file unless requested (LCSUM command).

Example 7.16:  Use of the RAPPND Command
/POST1       !  Following a 2 load step analysis
SET,1              !  Store load step 1
LCDEF,1,2          !  Identify load step 2 as load case 1
LCOPER,ADD,1       !  Add load case 1 to database (ls 1 + ls 2)
RAPPND,3,3         !  Append the combined results to the results file
!  as ls 3, time = 3
SET,LIST           !  Observe addition of new load step to results file

You can issue the RAPPND command to combine results from two results files (created with the same database.) Use the POST1 FILE command to toggle between the two results files to alternately store results from one and append to the other.

7.3.3.1.1. Hints and Recommendations

You can define a load case by setting a pointer to a load case via the LCFILE command. Later, you can issue the LCASE or LCOPER commands to read data from the file into memory.

You can erase any load case by issuing LCDEF,LCNO,ERASE, where LCNO is the load case number. To erase all load cases, issue LCDEF,ERASE. These options not only delete all load case pointers, but also delete the appropriate load case files (those with the default file name extensions).

To zero the results portion of the database, issue a LCOPER,ZERO command.

The LCABS and LCFACT commands enable you to specify absolute values and scale factors for specific load cases. The program uses these specifications when you issue either LCASE or LCOPER. The program applies scale factors after it calculates absolute values.

Results data read into the database from the results file (via SET or LCASE commands) will include boundary condition information (constraints and force loads). However, load cases read in from a load case file will not. Therefore, if boundary conditions appear on graphics displays after you issue an LCASE command, they are from a previously processed load case. The LCASE command does not reset the boundary condition information in memory.

After a load case combination is performed for structural line elements, the principal stress data are not automatically updated in the database. Issue LCOPER,LPRIN to recalculate line element principal stresses based on the current component stress values.

You can select a subset of load cases via the LCSEL command. After a subset is selected, you can use the label ALL in place of a load case number on load case operations.

Element nodal forces are operated on before summing at the node.

7.3.3.2. Combining Load Cases in Harmonic Element Models

For models with harmonic elements (axisymmetric elements with nonaxisymmetric loads), the loads are frequently applied in a series of load steps based on a Fourier decomposition (See the Element Reference). To get usable results, combine the results of each load step in POST1. You can do so via load case combinations, by saving and summing all results data at a given circumferential angle.

Example 7.17:  Combining Load Cases in a Harmonic Element Model
/POST1                 
SET,1,1,,,,90          ! Read load step 1 with circumferential
                       !  angle of 90°
LCWRITE,1              ! Write load case 1 to load case file
SET,2,1,,,,90          ! Read load case 2, with circumferential
                       !  angle of 90°
LCOPER,ADD,1           ! Use load case operations to add results 
                       !  from first load case to second 
ESEL,S,ELEM,,1         ! Select element number 1
NSLE,S                 ! Select all nodes on that element
PRNSOL,S               ! Calculate and list component stresses
PRNSOL,S,PRIN          ! Calculate and list principal
                       !  stresses S1, S2, S3; stress intensity
                       !  SINT; and equivalent stress SEQV
FINISH

See the SET, LCWRITE, LCOPER, ESEL, NSLE, and PRNSOL command descriptions for further information.

7.3.3.3. Summable, Non-Summable, and Constant Data

By default, when you perform load case combinations in POST1, the program combines only data that are valid for linear superposition, such as displacements and component stresses. Other data, such as plastic strains and element volumes, are not combined, because it is not appropriate or meaningful to combine such data. To determine which data should be combined and which should not, result items are grouped into summable, non-summable, and constant data. This grouping applies to the following POST1 database operations:

  • Load case combinations (LCOPER).

  • Reading in a load case with active scale factors (LCFACT or LCASE).

  • Reading in results data and modifying them via the FACT or ANGLE field on the SET command.

Summable data are those that can participate in the database operations. All primary data (DOF solutions) are considered summable. Among the derived data, component stresses, elastic strains, thermal gradients and fluxes, magnetic flux density, etc. are considered summable (see Table 7.2: Examples of Summable POST1 Results). (For an inclusive list of summable data, see the description of the ETABLE command in the Command Reference.)

Sometimes, combining summable data may result in meaningless results. For example, adding nodal temperatures from two load cases of a linear, pure-conduction analysis gives meaningful results, but if convection is involved, the addition of temperatures is not meaningful. Exercise your engineering judgement when reviewing combined load cases.

Non-summable data are those that are not valid for linear superposition, such as nonlinear data (plastic strains, hydrostatic pressures), thermal strains, magnetic forces, Joule heat, etc. (See Table 7.3: Examples of Non-Summable POST1 Results.) These data are simply set to zero when the programs performs a database operation. You can combine non-summable data (LCSUM,ALL) before issuing LCOPER commands, but take care to interpret the values appropriately.

Constant data are those that cannot be meaningfully combined, such as element volumes and element centroidal coordinates (see Table 7.4: Examples of Constant POST1 Results). These data are held constant (unchanged) when the program performs a database operation.

Table 7.2:  Examples of Summable POST1 Results

"Vector" Data
ItemComponentItemComponentItemComponent
UX, Y, Z ROTX, Y, ZVX, Y, Z
AX, Y, Z SX, Y, Z, XY, YZ, XZEPELX, Y, Z, XY, YZ, XZ
TGX, Y, Z TFX, Y, ZPGX, Y, Z
EFX, Y, Z DX, Y, ZHX, Y, Z
BX, Y, Z FX, Y, ZMX, Y, Z
VFX, Y, Z CSGX, Y, ZJSX, Y, Z
CGX,Y,ZDFX,Y,ZEPDIX, Y, Z, XY, YZ, XZ
LS(ALL) LEPEL(ALL)SMISC(ALL)

"Scalar" Data
TEMPMACHSTRMNDENNVISPTOT
TBOTHEATFLOWAMPSFLUXECON
TE2PRESVOLTMAGPCOE 
TTOTHFLUHFLMTCONEVIS 

Table 7.3:  Examples of Non-Summable POST1 Results

"Vector" Data
ItemComponentItemComponentItemComponent
EPPLX, Y, Z, XY, YZ, XZEPTHX, Y, Z, XY, YZ, XZNLSEPL, SRAT, HPRES, EPEQ, PSV, PLWK
FMAGX, Y, Z BFETEMPLEPTH(ALL)
LEPPL(ALL) LEPCR(ALL)NLIN(ALL)
LBFE(ALL) NMISC(ALL)  

"Scalar" Data
EPSWSENEKENEJHEAT

Table 7.4:  Examples of Constant POST1 Results

"Vector" Data
ItemComponent
CENTX, Y, Z

"Scalar" Data
VOLU 

7.3.4. Mapping Results onto a Different Mesh or to a Cut Boundary

Just as the PDEF command maps results onto an arbitrary path in the model, POST1 also has the ability to map results on to an entirely new mesh or to a portion of a new mesh. This functionality is mainly used in submodeling, where you initially analyze a coarse mesh, build a finely meshed submodel of a region of interest, and map results data from the coarse model to the fine submodel.

The CBDOF command maps degree-of-freedom results from the coarse model to the cut boundaries of the submodel. BFINT maps body force loads (mainly temperatures for a structural analysis) from the coarse model to the submodel. Both commands require a file of nodes to which results are to be mapped, and both commands write a file of appropriate load commands.

For more information, see Submodeling in the Mechanical APDL Advanced Analysis Guide.

7.3.5. Creating or Modifying Results Data in the Database

You can postprocess without also generating a results file. Create a database containing nodes, elements, and property data, and then put your own results into the database via the following commands:

DESOL -- Defines or modifies solution results at a node of an element.
DETAB -- Modifies element table results in the database.
DNSOL -- Defines or modifies solution results at a node.

After the data are defined, you can use almost any postprocessing function: graphics displays, tabular listings, path operations, etc.

Issuing the DNSOL command requires that you have placed the data type (stress/strain) in the element nodal records. To get around this requirement, use the DESOL command to add a "dummy" element stress/strain record.

The program performs all load case combinations in the solution coordinate system, and the data resulting from load case combinations are stored in the solution coordinate system. The resultant data are then transformed to the active results coordinate system when listed or displayed; therefore, unless RSYS,SOLU is set (no transformation of results data), you may see some unexpected results such as negative values after a square operation or negative values even when you request absolute values.

This feature is intended for reading in data from your own, special-purpose program. By writing output data from that program in the form of the above commands, you can read them into POST1 and process them the same way you would Mechanical APDL results. If you have a Mechanical APDL results file, it is not affected by these commands.

7.3.6. Splitting Large Results Files

If you have a results file that is too large for you to postprocess on your local machine (such as from running a large model on a server or cluster), you can split the results file into smaller files based on subsets of the model. You can then process these smaller files on your local machine. For example, if your large model is an assembly, you can create individual results files for each part.

You can also use this capability to create a subset of results for efficient postprocessing. For example, you could take the results file from a large model that had all results written, and create a smaller results file containing only stresses on the exterior surface. This smaller file would load and plot quickly, while not losing any of the detailed data written to the full results file.

When you use this feature, the subset geometry is also written to the results file so that you do not need the database file (no SET command required). However, do not resume any database when postprocessing one of these results files, and your original results file must have the geometry written to it (that is, do not issue /CONFIG,NORSTGM,1).

To use the results file splitting feature, issue the RSPLIT command. You can use results file splitting with INRES to limit the amount of data written to the results files.

Example 7.18:  Splitting Large Results Files
/POST1
FILE,jobname,rst            ! Import *.rst file
ESEL,all
INRES,nsol,strs             ! Write out only nodal solution and stresses
RSPLIT,ext,esel,myexterior  ! Write the results for the exterior of the whole model to a file 
                            ! named myexterior.rst
FINISH
/EXIT
...
/POST1
FILE,myexterior
PLNS,s,eqv                   ! Postprocess the myexterior.rst file as usual
PLNS,u,sum
FINISH

7.3.7. Magnetics Command Macros

The following magnetic command macros are also available for calculating and plotting results from a magnetic analysis:

  • CURR2D -- Calculates current flow in a 2-D conductor.

  • EMAGERR -- Calculates the relative error in an electrostatic or electromagnetic field analysis.

  • EMF -- Calculates the electromotive force (emf) or voltage drop along a predefined path.

  • EMFT -- Summarizes electromagnetic forces and torques on a selected set of nodes.

  • FLUXV -- Calculates the flux passing through a closed contour.

  • MAGSOLV -- Specifies magnetic solution options and initiates the solution for a static analysis.

  • MMF -- Calculates magnetomotive force along a path.

  • PERBC2D -- Generates periodic constraints for 2-D planar analysis.

  • PLF2D -- Generates a contour line plot of equipotentials.

  • PMGTRAN -- Summarizes electromagnetic results from a transient analysis.

  • POWERH -- Calculates the RMS power loss in a conducting body.

  • RACE -- Defines a "racetrack" current source.

  • SENERGY -- Determines the stored magnetic energy or co-energy.

For more information, see Electric and Magnetic Macros in the Mechanical APDL Low-Frequency Electromagnetic Analysis Guide.

7.3.8. Comparing Nodal Solutions From Two Models or From One Model and Experimental Data (RSTMAC)

In a typical design procedure, you may want to make small changes to your model and compare the solutions you obtain from the new model to solutions from the original model. You may also want to compare numerical solutions with experimental ones.

The RSTMAC command compares the nodal solutions from two results files (.rst or .rstp) or from one results file and one Universal Format file (.unv). The details about the Universal Format file supported records can be found in Universal Format File Records.

Only structural degrees of freedom are considered, and nodal solutions (real or complex) from any analysis type are supported. The procedure is based on the Modal Assurance Criterion (MAC) calculations (see POST1 - Modal Assurance Criterion (MAC) for more details).

Because the two files may correspond to different models and/or meshes, the first step consists of either of the following actions:

If you want to compare the nodal solutions of cyclic symmetric sectors (CYCLIC), model 1 and model 2 must have the same number of sectors and the solutions must correspond to the same harmonic index. If the MSUP option is not activated (CYCOPT,MSUP,NO) only the mapping and interpolation method (TolerN = -1) is available. Because the nodes of the basic sector and the nodes of the duplicate sector are coincident, the node mapping is done separately for each sector.

The next steps consist of:

All three of these steps are detailed below using two models of a simply supported beam. Model 1, tsolid, is a solid element mesh. Model 2, tbeam, is a beam element mesh.

All of the first ten eigensolutions are compared, and a full printout is requested (KeyPrint=2 on the RSTMAC command).

7.3.8.1. Matching the Nodes

The input is:

rstmac, tsolid,1,all, tbeam,1,all,,,, 2		

The output is:

   ******************** MATCHED NODES ********************
      Node in             Node in             Distance
      tsolid.rst          tbeam.rst           
         33                   1              0.0000E+00
        521                   2              0.0000E+00
        526                   4              0.0000E+00
        531                   6              0.2220E-15
        536                   8              0.4441E-15
        541                  10              0.8882E-15
        546                  12              0.1776E-14
        551                  14              0.2665E-14
        556                  16              0.3553E-14
       5000                  50              0.0000E+00

If there is no pair of nodes within the tolerance specified (TolerN and/or TolerR), the node matching is failing and the MAC calculations will not be performed.

The tolerance (TolerN > 0) is an absolute distance between nodes. Any pair of nodes with a distance smaller than the tolerance is considered matched. The tolerance value specified must be smaller than the element size to obtain relevant matched pairs. The default tolerance value is 0.01.

You can also use the relative tolerance (TolerR with TolerN = -2) for matching the nodes. It is a fraction of the minimum element dimension. The default relative tolerance value is 0.5 (50%).

The tolerance value specified must be smaller than the element size. The default value is 0.01.

Only the matched nodes will contribute to the MAC calculations.

If you want to match a set of selected nodes only, you may do one of the following:

  • Write only the solutions at the desired nodes on the results file via the OUTRES command (at the solver level).

  • Specify a component name (Cname) on the RSTMAC command. This component must be based on the desired nodes.

7.3.8.2. Mapping the Nodes

First, the database corresponding to tsolid must be resumed.

When comparing the nodal solutions of cyclic symmetric structures, the database must be saved AFTER the solution is finished. The same applies when comparing solutions obtained with the linear perturbation procedures, because the node coordinates are updated with the base analysis displacements during the solution.

The input is:

rstmac, tsolid,1,all, tbeam,1,all, -1,,, 2

The output is:

 ******************** MAPPED NODES ********************
              Node in             Element in
              tbeam.rst           tsolid.rst          
                  1                    1
                  2                   40
                  3                    3
                  4                    5
                  5                    8
                  6                   10
                  7                   13
                  8                   15
                  9                   18
                 10                   20
                 11                   23
                 12                   25
                 13                   28
                 14                   30
                 15                   33
                 16                   35
                 17                   38

Only the mapped nodes will contribute to the MAC calculations.

Nodes that are coincident may lead to erroneous interpolation. For example, this can occur in the case of spring/mass systems attached to solid elements.

If nodes and/or elements are selected (NSEL and/or ESEL, respectively), the results of the mapping and/or the interpolation show differences. To perform the MAC calculation on a part of the model, you can use the ESEL command. For a cyclic analysis where the MSUP option is not activated (CYCOPT,MSUP,NO), select the elements of both the base sector and the duplicate sector. For a cyclic analysis where the MSUP option is activated (CYCOPT,MSUP,YES) select the elements of the base sector only. All selected element nodes must also be selected (NSLE).

Issue the OUTRES command only when generating the second results file (File2). If the OUTRES command is issued to reduce the solution data written to the first results file (File1), the interpolation may be incorrect. (The problem can occur when an element does not have all of its nodes in the results file, for example.) This option is not supported when comparing cyclic symmetric structure results.

7.3.8.3. Evaluate MAC Between Solutions at Matched/Mapped Nodes

The MAC output for interpolated solutions (mapped nodes) is:

   ****** Modal Assurance Criterion (MAC) VALUES ******
                    Solutions are real
    Rows:     10 substeps in load step  1 interpolated from file tsolid.rst
    Columns:  10 substeps in load step  1 from file tbeam.rst

           1       2       3       4       5       6       7       8       9      10
    1   1.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000
    2   0.000   1.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000
    3   0.000   0.000   1.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000
    4   0.000   0.000   0.000   1.000   0.000   0.000   0.000   0.000   0.000   0.000
    5   0.000   0.000   0.000   0.000   1.000   0.000   0.000   0.000   0.000   0.000
    6   0.000   0.000   0.000   0.000   0.000   1.000   0.000   0.000   0.000   0.000
    7   0.000   0.000   0.000   0.000   0.000   0.000   1.000   0.000   0.000   0.000
    8   0.000   0.000   0.000   0.000   0.000   0.000   0.000   1.000   0.000   0.000
    9   0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000   1.000   0.000
   10   0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000   0.000   1.000

The modal assurance criterion values can be retrieved as parameters (*GET with Entity = RSTMAC).

The modes obtained after a modal analysis of a cyclic symmetric structure are repeated when the harmonic index is not equal to zero and not equal to the number of sectors divided by 2 (for an even number of sectors). In this case, the MAC values table is merged to allow the solutions matching. This merging consists of summing and averaging the MAC values of the repeated frequencies.

7.3.8.4. Match the Solutions

The Matched Solutions output for interpolated solutions (mapped nodes) is as follows:

   ********************************** MATCHED SOLUTIONS **********************************
    Substep in         Substep in           MAC value       Frequency          Frequency
      tsolid.rst          tbeam.rst                       difference (Hz)       error (%)
    (interpolated)
          1                   1               1.000          0.10E-01            0.2
          2                   2               1.000         -0.47E-02            0.1
          3                   3               1.000          0.26E-01            0.2
          4                   4               1.000          0.27E-01            0.1
          5                   5               1.000          0.40E-01            0.1
          6                   6               1.000          0.13E+00            0.2
          7                   7               1.000          0.11E+00            0.2
          8                   8               1.000          0.82E-01            0.1
          9                   9               1.000         -0.12E+00            0.1
         10                  10               1.000         -0.96E+00            0.6

If no pair of solutions has a MAC value greater than the minimum acceptable value specified (MacLim on the RSTMAC command), the matching of the solutions is failing. The default limit is set to 0.9.

7.3.8.5. Universal Format File Records

The Universal Format file records supported are the following.

  • Dataset Number 15 or 2411: Nodes

  • Dataset Number 55: Data at Nodes

    • Record 6

      • Field 1: Model Type = 1 (Structural)

      • Field 2: Analysis Type = 3 (Complex eigenvalue first order)

      • Field3: Data Characteristic = 2 (3 DOF) or 3 (6 DOF)

      • Field4: Specific Data Type = 8 (Displacement) or 12 (Acceleration)

      • Field5: Data Type = 2 (Real) or 5 (Complex)

    The modal assurance criterion is a normalized quantity. Multiplying one solution vector by a constant does not modify the end result. As a consequence, because the modal acceleration is equal to the modal displacement multiplied by the frequency squared, a modal displacement result on the results file can be compared to a modal acceleration vector on the .UNV file.


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