[Stuntmanbob]

Hi,
I know, there are a lot of postings to the "Stopped in routine MEMERR"-error, but non of them i found really fits my problem.

A short description of my simulation:
I have a cascade of 13 airfoils of a turbomachinery stage, where the blade in the middle is in motion. So i built a mesh, transformed it, so i got 13 channels that are glued together an startet a steady solution (without the blade in the middle moving) for initial values. After that i used the steady solution as initial values to the transient simulation (now with a moving Blade).

The steady simulation works fine, but the transient doesn't want to start.
On of the most appearing failures is the MEMERR-Error:



Details of error:-
----------------
Error detected by routine MAKDIR
CDRNAM = CAL_MESHDISP_BCS
CRESLT = OLD

Current Directory : /FLOW/SOLUTION/TSTEP1/CLOOP0/ZN1/BELG6/BVX

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine MEMERR
............


That's all the information i get from the Solver.

To "my" computer:
High performance super computer for scientific research! With up to 200CPUs an 200Gbyte Ram, so i dont think the size of the Memory is the problem.
Tested the simultation with Ansys CFX 15 and CFX 16, but there is no difference, the failure ist the same.

Thanks in advance,
Stuntmanbob

[ghorrocks]

Are you using mesh motion to model a rotating machine? That is a mistake. Use a rotating frame of reference instead.

[Stuntmanbob]

Hi,
Thank you for the fast reply :-)
The cascade doesn't rotate. I am using mesh motion for the moving blade, option: 'specified displacement', Displacement X Component = dx, Displacement Y Component = dy, Displacement Z Component = dz.... With dx, dy and dz defined in the Expressions.

I've done a lot of similar simulations, where the expressions and the displacements are always the same. But it is difficult to get the mesh motion with an highly enough vibration magnitude AND a mesh of good quality at the same time. So i startet the meshing with a wall cell size of 1exp(-5) and coarsen it a few times to get a motion with a magnitude that's really affected the pressure course in time.

So i always build new meshs with coursen wall cell size (it's really simpel in autogrid). The geometry is always the same, the mesh different. Now the wall cell size is 1exp(-2), but the rest of the quality of mesh (expansion factor, minimum/maximum angle and also the number of grid points) ist much better then in the previous meshs. I know this wall cell size isn't really good, but that's not the point in my simulation (a high vibration magnitude is more important).

I've also tried to delete the mesh of a former simulation and replace it with the new, with no positive effect, the failure is always the same.


Thanks in advance,
Stuntmanbob

[Thomas MADELEINE]

just to be sure I have understood every thing correctly.

You model 13 blades of one stage.
The blade in the middle is fluttering.
your simulation stop before first timestep.

so usually when I do some moving mesh simulation I take care of two things:
- what is my maximal displacement per timestep I have ? How big is it compare to my cell dimension ?

- to be sure the solver is doing the good displacement I want, I deactivate the fluid equations (in expert parameter) and only solve the mesh displacement during a run.
If it works properly then, I run a complete simulation with fluid equation and initialization.

[Stuntmanbob]

Hi,
Oh, i'm sorry. My former information weren't correct. The simulation stop while the first timestep . But also before solving the wall scale....


Maybe more information will help:

......
CFD Solver started: Tue May 19 16:58:37 2015


+--------------------------------------------------------------------+
| Convergence History |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| Writing transient file 0.trn |
| Name : Transient Results 1 |
| Type : Boundary Only |
| Option : Time Interval |
+--------------------------------------------------------------------+


================================================== ====================
| Timestepping Information |
----------------------------------------------------------------------
| Timestep | Courant Number | Acoustic Courant Number |
+----------------+-------------------------+-------------------------+
| | RMS MAX | RMS MAX |
+----------------+-------------------------+-------------------------+
| 1.9723E-03 | 726.38 999.99 | 999.99 999.99 |
----------------------------------------------------------------------

================================================== ====================
TIME STEP = 1 SIMULATION TIME = 1.9723E-03 CPU SECONDS = 2.145E+02
----------------------------------------------------------------------
| SOLVING : Mesh Displacement |
----------------------------------------------------------------------
| Equation | Rate | RMS Res | Max Res | Linear Solution |
+----------------------+------+---------+---------+------------------+

Details of error:-
----------------
Error detected by routine MAKDIR
CDRNAM = CAL_MESHDISP_BCS
CRESLT = OLD

Current Directory : /FLOW/SOLUTION/TSTEP1/CLOOP0/ZN1/BELG6/BVX

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine MEMERR |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 2. No results file |
| has been created. |
+--------------------------------------------------------------------+
..........



And yes, you're right.
The full stage has 30 blades.

Can you please tell me what parameter exactly i need to deactivate? This will bevery helpful and save me a lot of time :-)

Thanks,
Stuntmanbob

[Thomas MADELEINE]

I can't remember the exact name but right click on solver -> add expert parameter -> go to the last tab -> activate the parameter and set it to false
I remember the name was pretty obvious (something like solve fluid maybe)

[Opaque]

Please post the expression used for the motion of the blade.

It seems there is some kind of error in the expressions when CALculating the MESH DISPlacement Boundary ConditionS

[Stuntmanbob]

Hi,
Don't know if i can post the expressions, need to ask my tutor first (who is unfortunately on vacation).
But usually i edit the expressions with copy and paste (there are maybe 30 partially complicated expressions, through transformation of coordinates).
I don't think there will be an error, due to the fact of copy and paste. There are also no error-warnings in cfx-pre.
But i will check the on the morrow and post again.

Thanks,
StuntmanBob

[misagh]

Originally Posted by Stuntmanbob

Hi,
I know, there are a lot of postings to the "Stopped in routine MEMERR"-error, but non of them i found really fits my problem.

A short description of my simulation:
I have a cascade of 13 airfoils of a turbomachinery stage, where the blade in the middle is in motion. So i built a mesh, transformed it, so i got 13 channels that are glued together an startet a steady solution (without the blade in the middle moving) for initial values. After that i used the steady solution as initial values to the transient simulation (now with a moving Blade).

The steady simulation works fine, but the transient doesn't want to start.
On of the most appearing failures is the MEMERR-Error:



Details of error:-
----------------
Error detected by routine MAKDIR
CDRNAM = CAL_MESHDISP_BCS
CRESLT = OLD

Current Directory : /FLOW/SOLUTION/TSTEP1/CLOOP0/ZN1/BELG6/BVX

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine MEMERR
............


That's all the information i get from the Solver.

To "my" computer:
High performance super computer for scientific research! With up to 200CPUs an 200Gbyte Ram, so i dont think the size of the Memory is the problem.
Tested the simultation with Ansys CFX 15 and CFX 16, but there is no difference, the failure ist the same.

Thanks in advance,
Stuntmanbob

I found that error when I set a transient Outlet BC. You aren't allowed to
set a transient outlet BC with "pressure averaging: radial equilibrium".
Hope you get an idea.

[Stuntmanbob]

Hello misagh,
thanks for your advice :-)

I solved the problem a few month ago. The problem was in the mesh deformation Setting. After i changed the "Mesh Deformation relative to" from "Initial Mesh" to "previous mesh" the simultation works fine.

Greetings,
Stuntmanbob