[williamscn]

Hello

I am running the damBreakFine case. When I run:
setFields . damBreakFine
I get following error:
--> FOAM FATAL IO ERROR : size 2268 is not equal to the given value of 7700

How to do with this?

Thanks

[williamscn]

I got the problem.
Thanks

[rmorgans]

From memory, this is something to do with not copying gamma.org to gamma (check out the Allrun script).

Rick

[student0815]

Hi,

I got the same problem.

Followed instructions as told in the tutorial, but the same error occures.

Unfortunately no solution is given in this thread.

Anybody who can help?

Greetz

[bigphil]

I assume you have sorted the problem but for anyone else who has the same problem, you must copy gamma.org over gamma
ie cp 0/gamma.org 0/gamma
and type yes when it asks if you want to overwrite 0/gamma.

gamma starts off as a file with patch conditions (zeroGradient,symmetry,empty), then when setFields is run it reads this file and overwrites it with what I'm guessing is the values for the internal cells and the patches values are at the bottom.

So if you want to run setFields again (like if you changed your mesh) then you should copy gamma.org to gamma. gamma.org is a copy of the original gamma.

Hopefully this will help somebody.
Philip

[idrama]

Hey there!

the copying help.

cheers,

Claus

[bigphil]

Hi Claus,

As far as I know, the origin of the error is that the mesh (or mesh density) has been changed since the 'setFields' was last ran.

Is it the 'damBreak' case you are trying?

When you copy 'damBreak' from the '$FOAM_TUTORIALS/interFoam/' directory, you run 'blockMesh' first and then 'setFields', does 'setFields' work fine then?

Are you then changing the mesh density?

If you now run 'setFields' you will get the error above, so assuming 'gamma.org' was not altered, if you 'cp 0/gamma.org 0/gamma' then when you run 'setFields' it will work (I had a quick go with damBreak now and after copying the gamma.org file then 'setFields' works without the error).

In case 'gamma.org' was for some reason altered, just get it from $FOAM_TUTORIALS again ie 'cp $FOAM_TUTORIALS/interFoam/damBreak/0/gamma.org 0/gamma'


Hopefully this helps,
Btw I am assuming you are using the 'damBreak' case, let me know if the above doesn't help of if you are using a different case,

Philip

[Linse]

Though it might be necromancy to get back a thread nobody posted in for that long a time:

I do not remember which one it actually was, but one of the two things happened:
Either the files in the "polyMesh" directory remained the same and deleting those (make a copy of your blockMeshDict and do rm casename/constant/polyMesh/* ) helped.
Or it was necessary to renew the files of the variables in the casename/0 directory, as these are altered by earlier setFields-commands. Again: Keep a copy of the original files (before altering them with setFields) and just make "rm casename/0/*".

In both cases you have to copy back the "old" files to the directory where they are needed. If you then do a "blockMesh -case casename" and a "setFields -case casename" everything should be okay again.

In case I forget, remind me via private message, and I will upload a small script I wrote for these things...