Hi,

When i ran a steady flow simulation in Fluent, the solution converged after 60 iterations. Then i tried to plot the various parameters like velocity vectors, contours etc. When I selected the surfaces that I wanted these to be plotted on, Fluent just crashed (i.e. just vanished from the screen). Why does this happen?

I ran the same case again. This time I got convergence after 70 iterations. Again, it crashed when i tried to plot something. I ran the case again, and this time convergence was obtained after 90 iterations. Then crashed.

I'm wondering why the solution is converging at a different iteration each time. And why does it crash?

Any suggestions?

Thanks

Hi!

do NOT use the convergence criteria, Fluent provides! There are fluctuations in the residuals, so the value, that is given as criteria can be reached earlier, but without real convergence.

For monitoring convergence, use a point monitor. Choose a value, that is interesting (e.g. velocity or temp) at a characteristig point (e.g. boundary layer) and monitor that point (solve - monitor- surface).

So, if that value is convergent (and the residuals as well), the solution is convergent!

Best wishes

Ralf

Hi Ralf,

Thanks for the note. Suppose I choose velocity at the wall as the point of interest. How do I know that the residuals at that particular point has converged too? Does the same apply for the case of unsteady velocity also?

Another question- I want to specify the pressure outlet as the boundary condition for the outlet face. This is to be retained at atmospheric pressure. Hence I just retained the default values. Is this right?

Thanks, Vidya

Hi Ralf,

Following your suggestion, I tried to monitor the velocity at the inlet and outlet. I specified 100 iterations to begin with. The input BC was a steady velocity of 0.175 m/s at the inlet and the outlet is maintained at atmospheric pressure. But after 10 iterations, Fluent crashed i.e. vanished from the screen.

Any suggestions?

Thanks, Vidya

I tried to use the surface monitors panel....... but only get some plots where the graph just stays at zero. I wwent to Solve- Monitors- Surface.

Then selected the surface where I want to monitor the centerline outlet velocity, and checked the option for iterations. Also checked the 3 boxes nearby (WRITE, etc).

Even then, Fluent just keeps on iterating forever and these plots stay put at zero. Then finally Fluent crashes.

Where am I going wrong?

If Fluent is actually shutting down on you, then you have a system problem. Could be your computers, could be how Fluent is setup. When a model goes bad, Fluent's solution diverges, but Fluent remains open.

If Fluent is remaining open, then you need to investigate the flow field and understand where the problem is. Look at velocity vectors on the cross section, and is flow even going in the right direction?

You monitored velocity on a surface? If that surface is a wall, then of course it's going to give you 0 velocity, because the default wall is a no-slip condition. Create points, lines, or surfaces within the flow field. If it's not a wall, then the monitor is showing you that there is a problem with your flow field. The monitor tells you what the flow is doing, so if the velocity is 0 there, then you have no velocity there... something's wrong with your setup.

You really need to get into bad solution and look at the flow and understand what Fluent thinks is going on. Until you figure that out, you're never going to be able to fix the problem.

Hope this helps, and good luck, Jason

Can you explain what you meant when you asked to create points or surfaces within the flow field? Do we have to create additional surfaces in Gambit? Or Fluent?

I still keep getting a value of 0 everywhere. I set the reference pressure to zero and the outlet static pressure also to 0, just to test. But no success yet.

Create the points or surfaces in Fluent (they're all available under the Surface menu at the top of the Fluent window). Use these surfaces for your monitors.

If you're getting a value of 0 everywhere, then your setup is wrong, but from your previous posts, it sounded like you were monitoring velocities at the wall, which as I said will be 0. Make sure you're monitoring velocities within the flow field. Pressures and temperatures can be monitored at a wall, but velocity can't (definition of a no-slip condition... V @ wall = V of wall = 0 for non-moving surfaces).

Still, the fact that Fluent keeps vanishing from your screen is a bigger problem than your setup. You can't evaluate anything if Fluent just disappears. You need to talk to your tech support (either at Fluent, or whomever installed Fluent on your system) and get them to straighten it out. Now if you're running a batch script and it has an exit command, then that's what's causing it and you should run Fluent manually and interactively, at least until you get a proper solution. Otherwise it sounds like Fluent is crashing on it's own, and its either an installation problem or a system problem, and you need to get it fixed.

Hope this helps, and good luck, Jason

Hi Jason,

I checked with our system administrator and ensured that there's no problem with any of the computers or Fluent installation. Earlier, I used to get the divergence error:

Error: divergence detecetd in AMG solver: y- momentum

But this no longer appears.

It crashed again a little while ago.

Lol... you gotta love the computer gods... they're "infallible". Reminds me of a quote from the Simpsons from when they went to Itchy and Scratchy land... "Nothing could possibli go wrong... possibly go wrong... huh, that's the first thing that's gone wrong"

Contact your tech support at Fluent directly and ask him for a list of reasons why Fluent would simply close. If divergence isn't on that list (which I already know it isn't) then you can go back to your sys admin and say "Fluent crashes... it shouldn't... these are some possible reasons, but we need to fix this"

Have you tried running a similar sized (similar sized = same number of cells) case that doesn't diverge? Does that case remain open or does it close down too? It could be a memory problem if you've never run a case this large before...

I'm assuming that Fluent actually disappears... don't close it if Windows says it's "not responding"... Fluent sometimes goes off to think, and Window's doesn't realize it, but it shouldn't close Fluent... it may give a window that says "Not responding", but that's different.

Jason

I tried running the same case on different machines........ and the same thing happens. The divergence issue props up only if I'm using the unsteady velocity inlet condition. But if I use the steady velocity input condition, it just goews on computing forever, as I saud earlier.

Sometimes, I get the FLUENT NOT RESPONDING messsage, I waited for some time, and still the same message existed. So I closed it down. Yet, at other times (while running the same case), it just disappears without any indication.......only the command prompt remains (since I fired Fluent from the command prompt).

What is this weird thing about?

I just reran my case........ for the umpteenth time today. This time I removed the cylinders (that were causing other problem that I talked about) and ran the steady case with just the valve model. It converged after 59 iterations....... but when I asked it to plot the pressure contours (or even grid for that matter) on all the surfaces at the same time (i.e. inlet, outlet, wall, interior)...... Fluent again goes on thinking (hibernates), then gives the FLUENT NOT RESPONDING message. I waited for some time, for it to come back up, but it didn't and I ultimately lost patience and closed it down. Is it hibernating because of the complex grid? Or memory problems?

Then when I tried the same case with the unsteady velocity using the UDF, after just 3 iteration got an error message:

Error: Divergence detected in AMG solver: x- momentum.

Now what could be the reason for this?

Our system administrator found no plausible cause for Fluent to shut down, he said I'm the first one to report such a problem...... so he doesn't have an answer either. Fluent Tech support hasn't replied to this question of mine.

Thanks, Vidya

Well, I don't have experience with UDFs, so it could be something about it that's causing Fluent to shut down on you.

When you want to plot contours on "everything" DO NOT plot them on "interior"... this is going to plot the contours on every cell's face within your mesh and Fluent will take a while. Only plot on surfaces (i.e. inlet, outlet, cylinder walls, valve walls, and any surfaces you've created within the flow field). I don't even know why Fluent includes the "interior" option to plot on, but I guess they have their reasons. If you're running on a your local machine, bring up the Task Manager (Typically you can hit Ctrl-Alt-Delete, and then it'll either bring it up automatically or you have the option of selecting the Task Manager instead of logging off of the machine... if this doesn't work... if it's not there, ask your sys-admin how to find it) and check the Performance tab to see if the machine is plugging away at the problem. If your processor is running at high capacity, then Fluent is still thinking, so give it time... if it's not thinking, then Fluent is a lost process and can be killed. It could've gone into swap space (reading/writing from the HD) when it's trying to compute all of the colors on all of the faces... plus depending on your video card, you're relying completely on your main RAM and Processor, which is already loaded with the grid and solution, to process all of the contours. Just don't plot on "interior" and you should be alright.

Converging in 69 iterations... not likely... that means your convergence criteria is too loose. Go to Solve->Monitors->Residuals and change the convergence criteria, or turn it off (the check marks next to the Residual Values... you still want to plot them, you just don't want Fluent to assume the model's converged). You should really be monitoring flow field values to judge convergence. Make a point on the centerline of your flow field and monitor pressure and velocity at that point. Monitor drag on all of your walls. Monitor Average, Maximum, and Minimum pressure on your valve system. Create a few more points where the flow is going to be difficult to converge and monitor pressure/velocity there as well. Residuals don't mean much. Especially when you're having problems like you're having. You need to pay attention to the flowfield and learn what you can about it.

Diverging when you're using your UDF says one of two things to me... bad UDF, or bad time step size.

Hope this helps, and good luck, Jason

I just ran the case again after creating a point and 2 lines to monitor on the flow domain. But these plots just stay at zero throghout the computation. The y- axis values are all zero. Then after 100 iterations, there was an error message that says that Fluent received a fatal segment access violation. Now, what's wrong and where?

Regarding the UDF- I had some engineers from Fluent check the UDF earlier on. They ran it on their test model and confirmed that it was working fine. I gave it a time step size of 0.01 with 400 time steps. This would complete 2 cycles of the pulsatile waveform.

Thanks, Vidya

A point and 2 lines within the flow field are coming up with zero velocity... there's something wrong with your setup.

How big (# of cells) is your model? Do a search on the forum for Fatal Segment Access Violations to see if there's more info available.

You need to use the visualization tools in Fluent to look at the model and figure out why that velocity is zero. You're trying to push flow in the inlet, but for some reason it's not letting it go anywhere. Look at pressures, velocities, etc. and understand what Fluent thinks is going on. You may want to run the model for 50 iterations or so and try to get it at a point before it closes on you.

What are you using for a solver, what solver settings have you chosen, what fluid properties are you running, what did you use for your initialization, are there any other models you're using?

Jason

The only boundary conditions that I specified are a steady inlet velocity of 0.175 m/s at the inlet and OUTFLOW for the outlet. All the remaining regions are Wall. There are some regions where I gave the BC as INTERIOR.

After stopping the iterations at some point, I get some plots of velocity vectors, pressure contours at some of the surfaces....... there's nothing that plots on the outlet.....is this because the computation is still incomplete?

I'm using Segregated, laminar flow, node based, set all the initial velocities (X,Y,Z) to zero, presure at atmospheric, material properties are that of blood (density = 1050 kg/m3 and viscosity =0.004 kg/m-s).

With just the valve and leaflets I have a littlet over 41,100 nodes. If the cylinders are included, the number of nodes are 1.24 million....... just two cylinders are contributing so many nodes, and that's the reason I wanted to shorten the length of the inlet cylinder. But I wonder why that would cause the errors while computation.

Thanks, Vidya

Try the following

1. Increase iterations per timestep 2. Decrease time step 3. Start solution from inviscid and once u get a converged solution change to laminar. 4. Reduce the pressure and momentum under relaxation factors to 1/3rd the default values 5. Reduce the skewness of the mesh.(<0.95 preferably)

I'm worried about the Interior definitions. I have a feeling that your geometry coming out of Gambit is the problem. I think the faces between your cylinder and your volume with the valve isn't really connected. If this is the case, then these faces would really be treated as walls, and therefore you would have a giant wall blocking all of your flow. This could cause the problems with convergence, this could also explain why there's no flow at the exit. You can go into Gambit and manually connect these faces. Or you can use the "Interface" BC instead... if you chose the "Interface" BC, then you have to define your interface in Fluent as well (Define->Interfaces).

Also, an initialization of zero explains why you were getting "converged" results in 50 or 60 iterations... your initial guess was far from the reality of the flow (based on your BCs) that it was easy for the residuals to drop the default 10^-3, even though a true solution wasn't being reached...

For a steady-state solution, I would initialize the whole flow field based on the inlet velocity and pressure. Once you initialize, use the fmg-initialization to get a better initialization (the TUI command is: "solve init fmg y"... check out the Fluent manual and play around with the TUI if the short-hand doesn't make sense... actually you can go even shorter with "s i fmg y").

I think you need to be comfortable with the steady-state solution before you ever go into the unsteady solver. If you can't get a reasonable run out of the steady state (a truly unsteady problem may never converge, like large separation regions and such... that's why I say "a reasonable run" instead of "a converged solution"... but divergence and zero velocities at the outlet mean you're not getting a reasonable run), then I don't see how you could get the unsteady to work.

Such a large mesh within cylinders, but such a small mesh near the geometry of interest seems very odd... can you send me pictures of the mesh? Also, send me pictures of the flow field. I might be able to point out the problems if I have pics.

Hope this helps, and good luck, Jason

OK, Jason. I'll send you the pics. Do you want the Gambit pics or those of the volume mesh obtained from Tgrid?

Let me know and I'll send them to you. Should I send them to your yahoo id?

Thanks, Vidya

How does the logic of using Inviscid flow help? I'm modeling human blood flow, and blood is viscous (I'm using a viscosity of 0.004 kg.m-s) and also the no- slip condition is to maintained at the walls.

the mesh skewness is about 0.75. I also changed the interior regions with BC Interior.