Unable to converge on a solution

February 4, 2020 at 4:25 pm

fischr
Subscriber

Hello,

i want to import a temperature load to a static structural simulation in Workbench R19. But the solver engine is unable to converge on a solution. I used a command block to insert HSFLD242 Elements to model a fluid that is fully enclosed by solids.

The cavity is filled with HSFLD242 elements as you can see in the picture below:

does anyone have any idea why it is not converging? Do i need to define a thermal conductance for the material properties of my fluid ?
February 5, 2020 at 3:12 am

peteroznewman
Subscriber

There is useful information in the solve.out file in the solution folder. What is the error listed in that file? It looks like it nearly solved completely. Without seeing the information, it might help to have smaller elements.

February 5, 2020 at 10:59 am

fischr

Subscriber

Thanks for your reply. I tried a finer mesh, but it is still not converging and not even showing the heat convergence data.

The error messages are:

/COM,ANSYS RELEASE Release 19.0      BUILD 19.0      UP20171214       11:54:10

 *** WARNING ***                         CP =       1.391   TIME= 11:54:12
 Material property ALPX of material 1 is evaluated at a temperature of   
 0, which is below the supplied temperature range.  Temperature range    
 checking terminates.                                                    

 *** WARNING ***                         CP =       1.625   TIME= 11:54:12
 Element shape checking is currently inactive.  Issue SHPP,ON or         
 SHPP,WARN to reactivate, if desired.                                    

 *** WARNING ***                         CP =       5.391   TIME= 11:54:15
 Pivoting has been activated for the Distributed Sparse Matrix Solver .  
 The memory required may greatly exceed the predicted amount.  In that   
 event, use the DSPOPTION command to change the memory mode and/or       
 memory size used by the Distributed Sparse Matrix Solver.               

 *** WARNING ***                         CP =      16.516   TIME= 11:54:26
 There is not enough memory for the Distributed Sparse Matrix Solver to  
 proceed in the in-core memory mode.  The Distributed Sparse Matrix      
 Solver will now restart using the out-of-core memory mode.              

 *** WARNING ***                         CP =      16.797   TIME= 11:54:27
 The Distributed Sparse Matrix Solver is currently running in the        
 out-of-core memory mode.  This memory mode may provide significantly    
 worse performance compared to the in-core memory mode, depending on     
 the amount of available system memory and I/O speed.  Please monitor    
 the solver performance to ensure that the large amount of I/O to the    
 solver files does not create a bottleneck for performance.              

 *** WARNING ***                         CP =      16.797   TIME= 11:54:27
 Pivoting has been activated for the Distributed Sparse Matrix Solver .  
 The memory required may greatly exceed the predicted amount.  In that   
 event, use the DSPOPTION command to change the memory mode and/or       
 memory size used by the Distributed Sparse Matrix Solver.               

 *** ERROR ***                           CP =      36.172   TIME= 11:54:46
 There is not enough memory for the Distributed Sparse Matrix Solver to  
 proceed.  This is likely due to the use of pivoting while factoring     
 the matrix.  Please increase the virtual memory on your system and/or   
 increase the work space memory and rerun the solver.  Alternatively,    
 using the DSPOPTION command to switch to a different memory mode        
 and/or to specify additional memory for the solver may also help.  The  
 memory currently allocated for the Distributed Sparse Matrix Solver     
 solver = 134 MB.

February 5, 2020 at 11:08 am

fischr

Subscriber

with a course mesh i get these error messages:

/COM,ANSYS RELEASE Release 19.0      BUILD 19.0      UP20171214       12:03:18

 *** WARNING ***                         CP =       0.297   TIME= 12:03:19
 Material property ALPX of material 1 is evaluated at a temperature of   
 0, which is below the supplied temperature range.  Temperature range    
 checking terminates.                                                    

 *** WARNING ***                         CP =       0.359   TIME= 12:03:19
 Element shape checking is currently inactive.  Issue SHPP,ON or         
 SHPP,WARN to reactivate, if desired.                                    

 *** WARNING ***                         CP =       0.500   TIME= 12:03:19
 Pivoting has been activated for the Distributed Sparse Matrix Solver .  
 The memory required may greatly exceed the predicted amount.  In that   
 event, use the DSPOPTION command to change the memory mode and/or       
 memory size used by the Distributed Sparse Matrix Solver.               

 *** WARNING ***                         CP =       0.984   TIME= 12:03:19
 Material property KXX of material 1 of element 172 is evaluated at a    
 temperature of 546.910916, which is above the supplied temperature      
 range.  Temperature range checking terminates.                          

 *** WARNING ***                         CP =       2.266   TIME= 12:03:20
 Pivoting has been activated for the Distributed Sparse Matrix Solver .  
 The memory required may greatly exceed the predicted amount.  In that   
 event, use the DSPOPTION command to change the memory mode and/or       
 memory size used by the Distributed Sparse Matrix Solver.               

 *** WARNING ***                         CP =       3.797   TIME= 12:03:22
 Pivoting has been activated for the Distributed Sparse Matrix Solver .  
 The memory required may greatly exceed the predicted amount.  In that   
 event, use the DSPOPTION command to change the memory mode and/or       
 memory size used by the Distributed Sparse Matrix Solver.               

 *** WARNING ***                         CP =       5.266   TIME= 12:03:23
 Pivoting has been activated for the Distributed Sparse Matrix Solver .  
 The memory required may greatly exceed the predicted amount.  In that   
 event, use the DSPOPTION command to change the memory mode and/or       
 memory size used by the Distributed Sparse Matrix Solver.               

 *** WARNING ***                         CP =      11.250   TIME= 12:030
 Solution not converged at time 0.1 (load step 1 substep 1).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      17.609   TIME= 12:036
 Solution not converged at time 0.2 (load step 1 substep 2).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      23.797   TIME= 12:03:43
 Solution not converged at time 0.3 (load step 1 substep 3).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      30.141   TIME= 12:03:49
 Solution not converged at time 0.4 (load step 1 substep 4).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      36.250   TIME= 12:03:56
 Solution not converged at time 0.5 (load step 1 substep 5).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      42.516   TIME= 12:04:02
 Solution not converged at time 0.6 (load step 1 substep 6).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      48.547   TIME= 12:04:08
 Solution not converged at time 0.7 (load step 1 substep 7).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      54.844   TIME= 12:04:15
 Solution not converged at time 0.8 (load step 1 substep .             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      61.031   TIME= 12:04:21
 Solution not converged at time 0.9 (load step 1 substep 9).             
  Run continued at user request.                                         

 *** WARNING ***                         CP =      67.109   TIME= 12:04:28
 Solution not converged at time 1 (load step 1 substep 10).              
  Run continued at user request.

Without using HSFLD242 elements the solution is converging.

February 5, 2020 at 11:14 am

fischr

Subscriber

and if i set solver pivot checking on programm controlled i get these error messages:

/COM,ANSYS RELEASE Release 19.0      BUILD 19.0      UP20171214       12:09:40

 *** WARNING ***                         CP =       0.297   TIME= 12:09:41
 Material property ALPX of material 1 is evaluated at a temperature of   
 0, which is below the supplied temperature range.  Temperature range    
 checking terminates.                                                    

 *** WARNING ***                         CP =       0.359   TIME= 12:09:41
 Element shape checking is currently inactive.  Issue SHPP,ON or         
 SHPP,WARN to reactivate, if desired.                                    

 *** WARNING ***                         CP =       0.516   TIME= 12:09:41
 Pivoting has been activated for the Distributed Sparse Matrix Solver .  
 The memory required may greatly exceed the predicted amount.  In that   
 event, use the DSPOPTION command to change the memory mode and/or       
 memory size used by the Distributed Sparse Matrix Solver.               

 *** ERROR ***                           CP =       0.969   TIME= 12:09:41
 There are 543 small equation solver pivot terms (e.g., at the UY degree 
 of freedom of node 494).  Please check for an insufficiently            
 constrained model.

February 5, 2020 at 11:45 am

fischr
Subscriber

This is node 494:
February 6, 2020 at 1:49 pm

peteroznewman
Subscriber

I read the ANSYS help on the assumptions and restrictions on the HSFLD242 element and find that the fluid volume must have a uniform temperature without any gradients. That doesn't seem to be consistent with a Transient Thermal model where temperature gradients are present.

Try to use a CPT217 element which is capable of modeling coupled physics phenomena such as structural-pore-fluid-diffusion-thermal analysis and structural implicit gradient regularization using a nonlocal field. The element has a quadratic displacement, and linear pore-pressure and temperature behavior. With KEYOPT(11)=1, you specify you want a Structural-Thermal coupled field analysis.

Because it is a coupled-field analysis, you provide both thermal BCs and structural BCs and issue an ANTYPE,SOIL command and use the spares direct solver.
February 6, 2020 at 2:23 pm

fischr
Subscriber

Okay thank you for your answer! I will try using CPT217 Elements for the Fluid. I suppose I have to model the body of the fluid and mesh the fluidbody with CPT217? Then I have to model the contact between solid and fluid as well, is that right?
February 6, 2020 at 4:26 pm

peteroznewman
Subscriber

If I had used DesignModeler or SpaceClaim to prepare this geometry, I would have used Shared Topology so that nodes on the spherical surface were shared by the fluid elements on one body and the solid elements on the other body. In that case, I don't need any contact.
February 6, 2020 at 4:49 pm

fischr
Subscriber

Could you please explain how to implement CPT217 elements in ansys workbench?

I inserted a command snippet under the individual part (fluid) in Geometry tree:

ET,matid, CPT217
keyopt,matid,11,1

But this did not change the element type from SOLID187 to CPT217
February 6, 2020 at 6:46 pm

peteroznewman
Subscriber

Check the Solution Output to verify that SOLID187 elements were used in the mesh. Perhaps the mesh used linear elements? You can set the mesh to use quadratic elements.

February 7, 2020 at 2:02 pm

fischr

Subscriber

i set the mesh to use quadratic elements and it is meshing with SOLID87. With the command snippet i get the error message:

 *** ERROR ***                           CP =       0.328   TIME=

14:596
 An element referred to as 271 is a "null" or undefined element.

February 11, 2020 at 4:49 pm

fischr

Subscriber

it is still not working.

i used shared topology

inserted a command snippet under the body of the fluid with:

```
et,2,217

keyopt,2,11,1

keyopt,2,12,1
```

set the solver type to: direct

made a command snippet in solu:

```
antype,soil
```

used Full-Newton-Raphson-method, because i had error message:

The THOPT,QUASI option is valid only for the TEMP degree of freedom

it is still not finishing the solution :

in the error file i have only warning:

/COM,ANSYS RELEASE Release 19.0      BUILD 19.0      UP20171214       170:18

 *** WARNING ***                         CP =       0.297   TIME= 170:19
 Material property ALPX of material 2 is evaluated at a temperature of   
 0, which is below the supplied temperature range.  Temperature range    
 checking terminates.                                                    

 *** WARNING ***                         CP =       0.328   TIME= 170:19
 Element shape checking is currently inactive.  Issue SHPP,ON or         
 SHPP,WARN to reactivate, if desired.                                    

 *** WARNING ***                         CP =       0.953   TIME= 170:19
 Material property EX of material 2 of element 812 is evaluated at a     
 temperature of 473.991869, which is above the supplied temperature      
 range.  Temperature range checking terminates.                          

 *** WARNING ***                         CP =       1.109   TIME= 170:19
 A reference fluid flow value times the tolerance is used by the         
 Newton-Raphson method for checking convergence.  The calculated         
 reference FL FLOW CONVERGENCE VALUE= 0 is less than a threshold.  This  
 threshold defaults to 1.0e-6 or is specified as MINREF on the CNVTOL    
 command.  Check results carefully.

any suggestions on what to do?

February 11, 2020 at 10:37 pm

peteroznewman
Subscriber

You are getting 200 converged increments. Why do you say it is not working?

What do the results look like during these converged increments?

You are only showing warnings, not errors.

February 12, 2020 at 11:11 am

fischr

Subscriber

i can't plot any results, i have a read lightning bolt symbol :

this are the last steps from the solver output:

     FORCE CONVERGENCE VALUE  =  0.2116E-05  CRITERION=  0.5312E-04
     FL

FLOW CONVERGENCE VALUE=   0.000      CRITERION=  0.5312E-08
     HT FLOW

CONVERGENCE VALUE=  0.5705E-11  CRITERION=  0.1000E-05
     DISP CONVERGENCE

VALUE   =  0.6118E-09  CRITERION=  0.2784E-05 <<< CONVERGED
   

EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.2388E-05
    

FORCE CONVERGENCE VALUE  =  0.1900E-11  CRITERION=  0.1062E-03 <<<

CONVERGED
     FL FLOW CONVERGENCE VALUE=  0.4197E-24  CRITERION=  0.5312E-08

<<< CONVERGED
     HT FLOW CONVERGENCE VALUE=  0.7400E-13 

CRITERION=  0.1000E-05 <<< CONVERGED
    >>> SOLUTION

CONVERGED AFTER EQUILIBRIUM ITERATION   1
 *** LOAD STEP     1   SUBSTEP  

193  COMPLETED.    CUM ITER =    195
 *** TIME =  0.970000         TIME INC

=  0.500000E-02
 *** RESPONSE EIGENVALUE =  6.590       OSCILLATION LIMIT =

0.3295E-01
 *** RESPONSE FREQ = 0.3964E+05   PERIOD=  0.2522E-04  PTS/CYC =

0.50E-02
 *** AUTO STEP TIME:  NEXT TIME INC = 0.50000E-02 

UNCHANGED

     FORCE CONVERGENCE VALUE  =  0.2105E-05  CRITERION= 

0.5312E-04
     FL FLOW CONVERGENCE VALUE=   0.000      CRITERION= 

0.5312E-08
     HT FLOW CONVERGENCE VALUE=  0.5705E-11  CRITERION= 

0.1000E-05
     DISP CONVERGENCE VALUE   =  0.5800E-09  CRITERION= 

0.2784E-05 <<< CONVERGED
    EQUIL ITER   1 COMPLETED.  NEW TRIANG

MATRIX.  MAX DOF INC=  0.2375E-05
     FORCE CONVERGENCE VALUE  = 

0.1842E-11  CRITERION=  0.1062E-03 <<< CONVERGED
     FL FLOW

CONVERGENCE VALUE=  0.4489E-24  CRITERION=  0.5312E-08 <<<

CONVERGED
     HT FLOW CONVERGENCE VALUE=  0.7400E-13  CRITERION=  0.1000E-05

<<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM

ITERATION   1
 *** LOAD STEP     1   SUBSTEP   194  COMPLETED.    CUM ITER

=    196
 *** TIME =  0.975000         TIME INC =  0.500000E-02
 ***

RESPONSE EIGENVALUE =  6.590       OSCILLATION LIMIT = 0.3295E-01
 ***

RESPONSE FREQ = 0.3963E+05   PERIOD=  0.2524E-04  PTS/CYC = 0.50E-02
 ***

AUTO STEP TIME:  NEXT TIME INC = 0.50000E-02  UNCHANGED

     FORCE

CONVERGENCE VALUE  =  0.2095E-05  CRITERION=  0.5312E-04
     FL FLOW

CONVERGENCE VALUE=   0.000      CRITERION=  0.5312E-08
     HT FLOW

CONVERGENCE VALUE=  0.5705E-11  CRITERION=  0.1000E-05
     DISP CONVERGENCE

VALUE   =  0.6052E-09  CRITERION=  0.2784E-05 <<< CONVERGED
   

EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.2362E-05
    

FORCE CONVERGENCE VALUE  =  0.1878E-11  CRITERION=  0.1062E-03 <<<

CONVERGED
     FL FLOW CONVERGENCE VALUE=  0.4287E-24  CRITERION=  0.5312E-08

<<< CONVERGED
     HT FLOW CONVERGENCE VALUE=  0.7400E-13 

CRITERION=  0.1000E-05 <<< CONVERGED
    >>> SOLUTION

CONVERGED AFTER EQUILIBRIUM ITERATION   1
 *** LOAD STEP     1   SUBSTEP  

195  COMPLETED.    CUM ITER =    197
 *** TIME =  0.980000         TIME INC

=  0.500000E-02
 *** RESPONSE EIGENVALUE =  6.590       OSCILLATION LIMIT =

0.3295E-01
 *** RESPONSE FREQ = 0.3961E+05   PERIOD=  0.2525E-04  PTS/CYC =

0.50E-02
 *** AUTO STEP TIME:  NEXT TIME INC = 0.50000E-02 

UNCHANGED

     FORCE CONVERGENCE VALUE  =  0.2085E-05  CRITERION= 

0.5312E-04
     FL FLOW CONVERGENCE VALUE=   0.000      CRITERION= 

0.5312E-08
     HT FLOW CONVERGENCE VALUE=  0.5705E-11  CRITERION= 

0.1000E-05
     DISP CONVERGENCE VALUE   =  0.5737E-09  CRITERION= 

0.2784E-05 <<< CONVERGED
    EQUIL ITER   1 COMPLETED.  NEW TRIANG

MATRIX.  MAX DOF INC=  0.2349E-05
     FORCE CONVERGENCE VALUE  = 

0.1918E-11  CRITERION=  0.1062E-03 <<< CONVERGED
     FL FLOW

CONVERGENCE VALUE=  0.4431E-24  CRITERION=  0.5312E-08 <<<

CONVERGED
     HT FLOW CONVERGENCE VALUE=  0.7400E-13  CRITERION=  0.1000E-05

<<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM

ITERATION   1
 *** LOAD STEP     1   SUBSTEP   196  COMPLETED.    CUM ITER

=    198
 *** TIME =  0.985000         TIME INC =  0.500000E-02
 ***

RESPONSE EIGENVALUE =  6.590       OSCILLATION LIMIT = 0.3295E-01
 ***

RESPONSE FREQ = 0.3959E+05   PERIOD=  0.2526E-04  PTS/CYC = 0.51E-02
 ***

AUTO STEP TIME:  NEXT TIME INC = 0.50000E-02  UNCHANGED

     FORCE

CONVERGENCE VALUE  =  0.2075E-05  CRITERION=  0.5312E-04
     FL FLOW

CONVERGENCE VALUE=   0.000      CRITERION=  0.5312E-08
     HT FLOW

CONVERGENCE VALUE=  0.5705E-11  CRITERION=  0.1000E-05
     DISP CONVERGENCE

VALUE   =  0.5984E-09  CRITERION=  0.2784E-05 <<< CONVERGED
   

EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.2336E-05
    

FORCE CONVERGENCE VALUE  =  0.1928E-11  CRITERION=  0.1062E-03 <<<

CONVERGED
     FL FLOW CONVERGENCE VALUE=  0.4688E-24  CRITERION=  0.5312E-08

<<< CONVERGED
     HT FLOW CONVERGENCE VALUE=  0.7400E-13 

CRITERION=  0.1000E-05 <<< CONVERGED
    >>> SOLUTION

CONVERGED AFTER EQUILIBRIUM ITERATION   1
 *** LOAD STEP     1   SUBSTEP  

197  COMPLETED.    CUM ITER =    199
 *** TIME =  0.990000         TIME INC

=  0.500000E-02
 *** RESPONSE EIGENVALUE =  6.590       OSCILLATION LIMIT =

0.3295E-01
 *** RESPONSE FREQ = 0.3957E+05   PERIOD=  0.2527E-04  PTS/CYC =

0.51E-02
 *** AUTO STEP TIME:  NEXT TIME INC = 0.50000E-02 

UNCHANGED

     FORCE CONVERGENCE VALUE  =  0.2065E-05  CRITERION= 

0.5312E-04
     FL FLOW CONVERGENCE VALUE=   0.000      CRITERION= 

0.5312E-08
     HT FLOW CONVERGENCE VALUE=  0.5705E-11  CRITERION= 

0.1000E-05
     DISP CONVERGENCE VALUE   =  0.5676E-09  CRITERION= 

0.2784E-05 <<< CONVERGED
    EQUIL ITER   1 COMPLETED.  NEW TRIANG

MATRIX.  MAX DOF INC=  0.2323E-05
     FORCE CONVERGENCE VALUE  = 

0.1916E-11  CRITERION=  0.1062E-03 <<< CONVERGED
     FL FLOW

CONVERGENCE VALUE=  0.5016E-24  CRITERION=  0.5312E-08 <<<

CONVERGED
     HT FLOW CONVERGENCE VALUE=  0.7400E-13  CRITERION=  0.1000E-05

<<< CONVERGED
    >>> SOLUTION CONVERGED AFTER EQUILIBRIUM

ITERATION   1
 *** LOAD STEP     1   SUBSTEP   198  COMPLETED.    CUM ITER

=    200
 *** TIME =  0.995000         TIME INC =  0.500000E-02
 ***

RESPONSE EIGENVALUE =  6.590       OSCILLATION LIMIT = 0.3295E-01
 ***

RESPONSE FREQ = 0.3955E+05   PERIOD=  0.2529E-04  PTS/CYC = 0.51E-02
 ***

AUTO STEP TIME:  NEXT TIME INC = 0.50000E-02  UNCHANGED

     FORCE

CONVERGENCE VALUE  =  0.2054E-05  CRITERION=  0.5312E-04
     FL FLOW

CONVERGENCE VALUE=   0.000      CRITERION=  0.5312E-08
     HT FLOW

CONVERGENCE VALUE=  0.5705E-11  CRITERION=  0.1000E-05
     DISP CONVERGENCE

VALUE   =  0.5913E-09  CRITERION=  0.2784E-05 <<< CONVERGED
   

EQUIL ITER   1 COMPLETED.  NEW TRIANG MATRIX.  MAX DOF INC= -0.2310E-05
    

FORCE CONVERGENCE VALUE  =  0.1778E-11  CRITERION=  0.1062E-03 <<<

CONVERGED
     FL FLOW CONVERGENCE VALUE=  0.4592E-24  CRITERION=  0.5312E-08

<<< CONVERGED
     HT FLOW CONVERGENCE VALUE=  0.7400E-13 

CRITERION=  0.1000E-05 <<< CONVERGED
    >>> SOLUTION

CONVERGED AFTER EQUILIBRIUM ITERATION   1
 *** LOAD STEP     1   SUBSTEP  

199  COMPLETED.    CUM ITER =    201
 *** TIME =   1.00000         TIME INC

=  0.500000E-02
 *** RESPONSE EIGENVALUE =  6.590       OSCILLATION LIMIT =

0.3295E-01
 *** RESPONSE FREQ = 0.3953E+05   PERIOD=  0.2530E-04  PTS/CYC =

0.51E-02

also my global min of temperature is really low -2922°C , i set the ambient temperature to 200°C. i will try using a finer mesh.

February 12, 2020 at 4:36 pm

peteroznewman
Subscriber

Delete the two result plots and insert a new Temperature result, then Evaluate All Results. Even though it is a red lightening bolt, there are still 200 converged substeps. In the tabular data, you can pick any one of those 200 rows and Retrieve Results. Now the display is showing a converged result. What does that look like?
February 12, 2020 at 4:43 pm

fischr
Subscriber

and how can i describe the elasticity of my fluid in the material data? Is there a special setting for fluids? The elasticity of a fluid is described by the bulk modulus, but if i set the shear modulus to 0, my young modulus will also be 0 . Then it shows me a question mark in the definition of isotropic elasticity and i cannot perform a structural analysis.
February 12, 2020 at 6:59 pm

peteroznewman
Subscriber

This is what I used for Water some time ago...
February 13, 2020 at 2:02 pm

fischr
Subscriber

if i delete the result plots and insert a new temperature result, it is still not showing any tabular data. Under messages i get the error:

An error occurred when the post processor attempted to load a specific result. Please review all messages.

Current result file may not contain requested result data . Please clear the solution and solve again.

under solution information there is also no data to display for the temperature change.
February 13, 2020 at 3:24 pm

peteroznewman
Subscriber

You might have to open the model in Mechanical APDL to look at the results from a SOIL analysis type, I don't know. You might want to open a new Discussion to ask the specific question about obtaining results from a SOIL analysis. Someone else will have to answer that question.

You can try to open Mechanical APDL and open the results file in that application. I don't use that application so I can't help you with that either. I recommend performing a simple model in APDL that solves without error to get used to the user interface before you attempt to look at this SOIL model.