Hello! I have a problem with star_cd. When I check for the illegally placed boundaries, a message of error appear. How can I display the wrong boundary? Bye

Usuall behaviour for all check routines in Prostar (including boundary check) is to place failed entities in the set. So just enable boundary plot and press plot. But it can happen so that your illegal boundary can't be displayed at all.

when you write geom file,prostar will put ill-defined boundaries in a bset. You have to do "bdisplay,on" and "cplot".

Thank you for your help, I'll try to do it tomorrow. Bye.

Other question for you: My model have some cracks (about 1000); I'd like to display it and correct. How can I get it? Thank you in advance.

Best regards

Do a "live,surface,create" on the fluid cells,and plot the newly created shells. You will see a lot of floating cells. These cells sit on the cracks.

Thank you for you help and your hints, but I have created the shell as you have said and there are also cracks. I have used this procedure:

-I check the crack with the command "check tool" and I have put this cells in a newset, after that I have displaied this with command "cplo".

-I have used the command "live surface create" and I have created a new set of cells but there are the equal number of crack as at the start of this procedure. Why?

Thank you in advance. Bye

what i said in my second post is just to identify the cracks. It does not fix the cracks. you have to know how the cracks are created. There are a lot of possibilites. For example, the vertices are not merged or the cpmatch couples are missing, etc.

I have found the cracks, about 1789. I have marged the vertex and now there are problems with the couple.

In your opinion, which kind of procedures you can use.

Thank you in advance. Bye

What did you do to get so many cracks? I have never been able to create a single one. What type of meshing did you use?

Do you still have cracks after merging the vertices?

I would delete the couples with problems (maybe after trying to merge the couples), do a check for cracks and create new couples on the cells with cracks.

regards,

Volker

you can try the following: 1.cpmerge,all 2.cpcheck,,cpset,,news,,fix

Thank you for your help, I'll try to do it next week.

In the meantime I'm trying to do a run in parallel mode with star_hpc but I have found a problem with view factors. The error say:

"beam tracking is not supported in parallel - exiting", for 4 time, in fact I have decomposed the geometry file for 4 processors.

The file .vfs must be created as a serial run after that I have put it on the directory that star_hpc has created.

Have you any idea?

Thank you in advance.

Hallo Massimo!

To get sure that star-HPC doesn't try to compute the view factors once again, you should split the .pst file and perform a restart-run. Moreover the .vfs file should be cpied into each one of the 4 subdirectories.

Bye

marco

Eh, if I'm not mistaken, solution for radiation problems is not yet available for STAR-CD in parallel, not even on their latest (as of this time of writing) v3.15 STAR. I remember it is mentioned in the release notes or something. I suppose you can perform the flow calculations in HPC first and then try and do a restart run on a single CPU but with rad effects.