General Mechanical

General Mechanical

Not Enough Memory Error?

    • Autonewbie


      I have a simple model with spring element between two solid parts and total 94K nodes. My workstation still has a lot of space... Why there is not enough memory?



      *** NOTE ***                            CP =     104.734   TIME= 200:53
       The initial memory allocation (-m) has been exceeded.                   
        Supplemental memory allocations are being used.                        

       *** ERROR ***                           CP =     104.938   TIME= 200:53
       There is not enough memory for the Distributed Sparse Matrix Solver to  
       proceed.  This error has occurred on the process with MPI Rank ID = 9   
       on machine .  Please increase the virtual   
       memory on your system and/or increase the work space memory and rerun   
       the solver.  The memory currently allocated by this process = 1024 MB.  
        The memory allocation attempted = 1248 MB.  The largest block of       
       memory allocated by this process that is available for the Distributed  
       Sparse Matrix Solver = 876 MB.                                          

       *** ERROR ***                           CP =     104.938   TIME= 200:53
       An error has occurred in the Distributed Sparse Matrix Solver while     
       attempting to allocate the memory required to process the matrix        
       structure.  Error code = -1001.  Please send the data leading to this   
       operation to your technical support provider, as this will allow        
       ANSYS, Inc to improve the program.                                      

       *** ERROR ***                           CP =     105.000   TIME= 200:53
       An unexpected error has occurred on MPI rank 0 in the MPI software used 
       by Distributed ANSYS.  Distributed ANSYS is unable to recover and will  
       terminate.  Please send the data leading to this operation to your      
       technical support provider, as this will allow ANSYS, Inc to improve    
       the program.       


    • Autonewbie


      Above is my workstation hdd space status

    • peteroznewman

      1. The memory referred to in the messages is RAM memory not storage, which you are showing in your image above.

      2. Did you make any entries or changes to the memory settings for the solution? Don't touch those. ANSYS manages them very well on its own. There are posts on this site from members who meddled with the settings, thinking they were helping ANSYS to manage the memory, but they didn't understand the meaning of the settings and all they did was cause the error!

      3. If you did not touch the memory settings, Restart your computer, open the model, Solve and see if the error repeats. Sometimes on a computer that has had many programs opening and closing and some programs still in memory, the memory gets chopped up into small pieces and no one piece is big enough to solve the ANSYS model. A Restart cleans that up.

      4. The Direct Solver needs more memory than the Iterative Solver. Try selecting the Iterative solver. Note that some models cannot be solved on the iterative solver due to the elements used in the model and can only run on the Direct solver.

      5. It's possible to have a model that is too large for the amount of available memory. In that case, you must reduce the node count or install more RAM.

      6. Does ANSYS successfully solve small models? It's possible the installation did not complete correctly.

    • Autonewbie

      Hi Peter,

      I restart the workstation (I did not change any memory setting) but it is issue with the warning below. However, I changed the model smaller with spring, it can run. But I have bigger model (3 - 4 times) for transient and random analyses also no problem except this time with spring. 


       *** WARNING ***                         CP =       8.641   TIME= 22:14:51

       Element shape checking is currently inactive.  Issue SHPP,ON or         

       SHPP,WARN to reactivate, if desired.                                    


       *** WARNING ***                         CP =      10.641   TIME= 22:14:51

       Material number 7 (used by element 287758) should normally have at      

       least one MP or one TB type command associated with it.  Output of      

       energy by material may not be available.                                


       *** WARNING ***                         CP =      18.344   TIME= 22:14:54

       Too many nodes 10720 are included in the force-distributed-surface      

       constraint identified by real constant set 5.  This may greatly affect  

       solver performance due to large wave fronts and memory consumption.     

       Also check results carefully and consider solving with a different      

       unit system.                                                            



    • Autonewbie

      Just an update here... after I re-run few times, it works but some findings:


      1.) Memory issue occurred when I changed to use deformable behavior for reference and mobile

      2.) Time to solve for deformable behavior is 1m40s but rigid behavior is 16s only

    • peteroznewman

      Make smaller faces on large solids to scope the spring reference and mobile ends to.

      Deformable results in a larger model than Rigid behavior on remote points used to scope spring ends to.

    • Autonewbie

      Do you mean cut a small face (as red circle) on the solid part? Thanks.


    • peteroznewman

      Yes. If you use SpaceClaim, that is as simple as opening a Sketch on that face and drawing a small rectangle. When you exit the sketch and return to 3D mode, the one face will become two faces. 

Viewing 7 reply threads
  • You must be logged in to reply to this topic.