Hi all. I kept on getting this error message. I checked the boundaries many times to locate where the problems may be - but failed. For your info, I am using inlets, outlet (with fixed flow rate) and (static) pressure boundary conditions. There should not be any outflow on the pressure BC, it is there just to indicate the surface is open/expose to atmospheric/ambient pressure. Can somebody please give me a hint on what should I be looking for?

*** WARNING #001 *** FLUID INFLOW DETECTED AT SOME OUTFLOW BOUNDARIES WHERE MASS FLUXES ARE FORCED TO ZERO.

IF THIS CONDITION PERSISTS, YOUR RESULTS MIGHT BE WRONG

THE OUTFLOW BOUNDARY MIGHT NOT BE WELL SPECIFIED OR THE GRID MIGHT BE TOO COARSE NEAR THE OUTFLOW BOUNDARY

Many thanks.

Shazlan

Found out that I have cracks in my model. What is the simplest way for me to fix this? I tried vmer with a tolerance of .01 and doesnt work.

If there may be some other errors which leads to the above warning messages (and hence, diverging solution) which I kept on getting, please let me know.

Help is very much appreciated! Shazlan

Are you using a trimmed mesh? If that is the case, you will most likely have your cracks in regions where you don't have a one-to-one cell connectivity. You have to deal with it by generating couples between those cells. Your problem with the outlet-BC might not be related to the cracks (but you should still solve this problem). A cause for this problem can be a recirculation zone at your BC. Try extruding the mesh at the outlet. Or if you get this error message at the beginning of your calculation, just wait a few iterations and it might just go away.

Good luck,

Volker

Honestly, I am not sure what type of mesh I am using. The grid/mesh was preproduced in Gridgen. Anyway, I fixed the crakcs by going back to Gridgen and did some neccessary changes. The cracks are now gone but there are a few more other errors appeared when I used the Check Grid >> Check All option. They are aspect ration, internal angles, internal face angles and I believe it is the small surface area. My next question is are those errors critical error? or those errors are setting dependant errors (I use all the default 'checking' option in Star-CD) and hence can be ignored? Please advice.

Thanks and have a nice day!

OK, if you used an automatic mesher, you will most likely have a tet-mesh (trimmed meshes are a prostar speciality and can be produced in proam). The errors you are getting relate to your cell quality. They are not necessarily knock-out problems like left-handed or concave cells. Nevertheless, you should check where they are and how many cells have a poor quality. Some of the problems can be ignored (e.g. aspect ratios in fine wall boundary cells). You can still try and work with your mesh or you go back and generate a better mesh. Usually that means a finer and larger mesh, extra work and longer computing times. If your mesh isn't a complete desaster, I would give it a go and see if it converges and gives you realistic results. In the mean-time you can generate the better mesh.... Don't forget to extrude your outlet in Star. You can do that by generating shells on your outlet and then use the command vcextrude. After that, you have to do a vmerge and relocate your outlet boundary.

Good luck,

Volker

Dear Volker, I did not get what do u mean by 'Extrude outlet in star'. why do we need to extrude? Hope u provide me some details on that so it will clarify me better.

One more thing,Is vcextrude available in GUI menus?

Regards, Suresh