Please help me out: linear solver Overflow
Hello everyone,
I tried to simulate a baffled mixing tank in which dense solidliquid system are mixed. When I set up the domains and boundary and initial conditions, I got fatal error saying that Fatal overflow in linear solver. I assigned the top of the tank as freeslip wall and no OUTLET and INLET conditions at all in the model. Anyone can help me out? Do I need to assign a Openning boundary condition at a small area of the top of the tank? And is it possible to simulate a domain without any INLET and OUTLET boundary conditions? I will really appreciate your help. Sincerely, Jeniffer 
Re: Please help me out: linear solver Overflow
Hi Jennifer, It is possible, but the solver does prefere if an opening is prescribed somewhere in the model. We were looking at a falling column of water into a sealed tank. We did manage to get the model to run, but once we had defined a small opening, the solution was more stable. Bob

Re: Please help me out: linear solver Overflow
Hi Jeniffer,
It is possible to simulate your tank without openings, however the solver must have the pressure level defined somewhere in the computational domain. In the absense of a pressure boundary condition, the solver will default to setting the pressure level at the first control volume to be equal to your domain reference pressure. Since your initial guess should include a hydrostatic pressure distribution, your initial pressure field may not agree with the location of this pressure. You have 2 options. You could open your def file in post and find the location of node 1, then define your initial guess with this in mind. Or you could add a small opening to your tank, probably at the top, and define your initial guess relative to the pressure level at that opening. Personally, I would go with the latter. Best regards, Robin 
Re: Please help me out: linear solver Overflow
Hi, Bob and Robin,
Thank you very much for your response. I will try to add a small opening at the top of the tank. Best regards, Jeniffer 
Re: Please help me out: linear solver Overflow
Robin, how do yuo use post to identify node numbers and locations ? When we defined our reference pressure we used some fortran (supplied by CFX) to extract the nearest node (number) from a defined monitor point. It was a little bit of a pain as you had to run for one timestep, extract the node number then restart with the expert parameter to define the reference pressure location. I understand the requriment for defining this location has been passed onto the developers. Bob

Re: Please help me out: linear solver Overflow
Hi Bob,
The Point object in CFXPost has an option to create a point at a given node number. Robin 
Re: Please help me out: linear solver Overflow
Robin, is it possible to reverse the process and define a point then using a function extract the node number ? Bob

Re: Please help me out: linear solver Overflow
Hi, Robin and Bob,
I tried an openning on the top of the surface then assigned a static pressure for the Openning BC. I am running EurlerEurler solidliquid simulation in rotationay and stationary domains (steadystate). After 200 time steps, the RSM residuals for continuous liquid and dispersed solid are of 10^(3) magnitude, while the imbalance of PVol for both domains remains +100% and 98% respectively. My question is why imbalance for solidphase and liquid phase in both domains are close to (+/)100% after 200 time steps. Are the RSMs for PVol, SolidMass and LiquidMass calculated in such a way that the total imbalance in the whole domain (Rotationary plus Statiionary domain) is counted? Thank you very much! Jeniffer 
Re: Please help me out: linear solver Overflow
Not as far as I know. But may I ask why you would need to do this?
Robin 
Re: Please help me out: linear solver Overflow
Robin, If we wanted to define a reference pressure for a free surface (sloshing) problem we would want to define it in the air region of the model. If I could define a point which I know before hand is in the air then extract the node number, it would save me time and hassle. At the moment I use a fortran routine to extract the node number from a monitor point which I create. I then feed this back into the simulation for the reference pressure location. Its not a major hassle unless I do mesh sensativity tests and mess up my node numeber. Bob

Re: Please help me out: linear solver Overflow
Hi Bob,
Apparently you can get the nearest node number. If you right click on the point object in post and select "Edit in Command Editor", there is a CCL parameter named "Nearest Node Number". If you want to extract this value in a script, simply use the getValue PowerSyntax command, for example: !$nearestNode = getValue("Point 1","Nearest Node Number"); !print "$nearestNode\n"; The above script will extract the nearest node number and print it to the standard output. As for setting your reference pressure at a node, I don't recommend it. You are contraining the continuity equation too much and are better off defining a proper pressure boundary condition. Regards, Robin 
Re: Please help me out: linear solver Overflow
Hi Robin, Cheers for the Pointers, I'll make sure we modify the models in future. Bob

Re: Please help me out: linear solver Overflow
Hi Bob,
I have just learned that you will be able to set the reference pressure at a location in space (X,Y,Z) in version 5.7. Regards, Robin 
Quote:
I am simulating a closed Tank, but I always get an overflow error after some iterations. I would like to know how can I fix this problem. Could it be caused by the pressure initialization? The solver set zero pressure to the first node of the mesh. I really appreciate your help. 
It's more likely that you simply have a poor initial condition and it is difficult for the solver to get started. As you've noted, CFX will automatically set a pressure level by default if it isn't set by a boundary condition, so that is unlikely to be causing you problems. Consider whether or not you can create a better initial condition, and if you can't, try reducing the timescale factor or physical timescale you are using by a couple orders of magnitude to try to ease the solver in. Once it is running and converging slowly but smoothly you can increase the timescale.

All times are GMT 4. The time now is 07:07. 