Problem with topoSet

wtjhaha · May 25, 2015, 22:00

Hi all,
I am meshing a tube with a glass cover outside the tube, and I use the topoSetDIct to set the region of the air and the tube.But there is a bug when running topoSet.

Code:

--> FOAM FATAL IO ERROR: 
attempt to read beyond EOF

file: /home/wtj/OpenFOAM/wtj-2.3.1/run/tube1/system/topoSetDict.actions at line 34.

And this is my topoSetDict

Code:

/*--------------------------------*- C++ -*----------------------------------*\
| =========                 |                                                 |
| \\      /  F ield         | OpenFOAM: The Open Source CFD Toolbox           |
|  \\    /   O peration     | Version:  2.3.1                                 |
|   \\  /    A nd           | Web:      www.OpenFOAM.org                      |
|    \\/     M anipulation  |                                                 |
\*---------------------------------------------------------------------------*/
FoamFile
{
    version     2.0;
    format      ascii;
    class       dictionary;
    object      topoSetDict;
}

// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

actions
(
    // Air
    {
        name    air;
        type    cellSet;
        action  new;
        source  cylinderToCell;
        sourceInfo
        {
            p1(0 0 0);
	    p2(0 0 0.5);
            radius 0.017;
        }
    }
    {
        name    air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set air;
            
        }
    }
    

    // Tube
   
    {
        name    tube;
        type    cellZoneSet;
        action  clear;
        
    }

    
    {
        name    tube;
        type    cellSet;
        action  add;
        source  cellToCell;
	sourceInfo
	{
		set air;
	}
        
    }
    {
        name    tube;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set tube;
           
        }
    }
);

// ************************************************************************* //

Anybody can help me with this problem? I am stuck in it for several weeks and I really need help!

Nicole · May 27, 2015, 06:54

Hi,

I have not seen your error message before. Are you by any chance using blockMesh to mesh your domain?

zfaraday · May 27, 2015, 08:22

I'm not sure what this error means, although I think I had to face it in the past. However, by reading your topoSetDict file I saw something weird that can be causing the problem, or maybe can cause another problem instead. First of all, you are creating a cellSet named air which is a cylinder. After that it is converted into a cellZone. The next step consists in the creation of another cellSet called tube with the same cells that make up the air cellSet, next you convert it into another cellZone with the result of two diferents cellZones made up with the same cells... I'm not sure if it can be done...I think that if a cell already belongs to a cellZone it cannot be part of another cellZone.

As per my experience I think you may have missed a step in your topoSetDict, namenly the step when you invert your selection in odrer to select all the cells that don't belong to the air cellSet to create the tube cellSet. Am I right?

Hope it helps.

Alex

wtjhaha · May 27, 2015, 21:01

Quote:

Originally Posted by zfaraday

I'm not sure what this error means, although I think I had to face it in the past. However, by reading your topoSetDict file I saw something weird that can be causing the problem, or maybe can cause another problem instead. First of all, you are creating a cellSet named air which is a cylinder. After that it is converted into a cellZone. The next step consists in the creation of another cellSet called tube with the same cells that make up the air cellSet, next you convert it into another cellZone with the result of two diferents cellZones made up with the same cells... I'm not sure if it can be done...I think that if a cell already belongs to a cellZone it cannot be part of another cellZone.

As per my experience I think you may have missed a step in your topoSetDict, namenly the step when you invert your selection in odrer to select all the cells that don't belong to the air cellSet to create the tube cellSet. Am I right?

Hope it helps.

Alex

Thank you for your reply, and I changed my topoSetDict, but unfortunately, it still doesn't work.
This is my new topoSetDict, is there still problems there?

Code:

actions
(
    // Air
    {
        name    air;
        type    cellSet;
        action  new;
        source  cylinderToCell;
        sourceInfo
        {
            p1(0 0 0);
	    p2(0 0 0.5);
            radius 0.017;
        }
    }
    {
        name    air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set air;
            
        }
    }
    

    // Tube
   
    {
        name    tube;
        type    cellZoneSet;
        action  clear;
        
    }

    
    
    {
        name    tube;
        type    cellSet;
        action  invert;
    }
    {
        name    tube;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set tube;
           
        }
    }
);

Thanks again!

wtjhaha · May 27, 2015, 21:08

Quote:

Originally Posted by Nicole

Hi,

I have not seen your error message before. Are you by any chance using blockMesh to mesh your domain?

Thanks for your reply, but I am sorry I didn't really catch you. So can you explain for me in a common way?

zfaraday · May 28, 2015, 04:57

Quote:

Originally Posted by wtjhaha

Thank you for your reply, and I changed my topoSetDict, but unfortunately, it still doesn't work.
This is my new topoSetDict, is there still problems there?

Code:

actions
(
    // Air
    {
        name    air;
        type    cellSet;
        action  new;
        source  cylinderToCell;
        sourceInfo
        {
            p1(0 0 0);
	    p2(0 0 0.5);
            radius 0.017;
        }
    }
    {
        name    air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set air;
            
        }
    }
    

    // Tube
   
    {
        name    tube;
        type    cellZoneSet;
        action  clear;
        
    }

    
    
    {
        name    tube;
        type    cellSet;
        action  invert;
    }
    {
        name    tube;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set tube;
           
        }
    }
);

Thanks again!

Well, that's not exactly what I was suggesting... You have to invert your selection once you have selected the cells you want to dismiss. It would be something like:

Code:

actions
(
    // Air
    {
        name    air;
        type    cellSet;
        action  new;
        source  cylinderToCell;
        sourceInfo
        {
            p1(0 0 0);
	    p2(0 0 0.5);
            radius 0.017;
        }
    }
    {
        name    air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set air;
            
        }
    }
    

    // Tube
   
    {
        name    tube;
        type    cellZoneSet;
        action  clear;
        
    }
        
    {
        name    tube;
        type    cellSet;
        action  add;
        source  cellToCell;
	sourceInfo
	{
		set air;
	}
        
    }
    
    {
        name    tube;
        type    cellSet;
        action  invert;
    }
    {
        name    tube;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set tube;
           
        }
    }
);

I haven't checked if the sintax of the invert action is correct, it may be wrong...

BTW, you should be more accurate in your questions in order to make it easy for the other users to help you, for instance you may have added the error message in your last post.

Regarding the question that @Nicole is pointing out, it's easy to understand, he/she is only asking if you created your mesh using blockMesh. However, if you didn't understand the question you may not even know what blockMesh is, so we can deduce that you meshed your geometry with other tool, did you?

Regards,

Alex

wtjhaha · May 28, 2015, 05:12

Quote:

Originally Posted by zfaraday

Well, that's not exactly what I was suggesting... You have to invert your selection once you have selected the cells you want to dismiss. It would be something like:

Code:

actions
(
    // Air
    {
        name    air;
        type    cellSet;
        action  new;
        source  cylinderToCell;
        sourceInfo
        {
            p1(0 0 0);
	    p2(0 0 0.5);
            radius 0.017;
        }
    }
    {
        name    air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set air;
            
        }
    }
    

    // Tube
   
    {
        name    tube;
        type    cellZoneSet;
        action  clear;
        
    }
        
    {
        name    tube;
        type    cellSet;
        action  add;
        source  cellToCell;
	sourceInfo
	{
		set air;
	}
        
    }
    
    {
        name    tube;
        type    cellSet;
        action  invert;
    }
    {
        name    tube;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set tube;
           
        }
    }
);

I haven't checked if the sintax of the invert action is correct, it may be wrong...

BTW, you should be more accurate in your questions in order to make it easy for the other users to help you, for instance you may have added the error message in your last post.

Regarding the question that @Nicole is pointing out, it's easy to understand, he/she is only asking if you created your mesh using blockMesh. However, if you didn't understand the question you may not even know what blockMesh is, so we can deduce that you meshed your geometry with other tool, did you?

Regards,

Alex

Thanks Alex,
I created my mesh using blockMesh, and it was posted in my first thread. I didn't post the error message for it was the same with the one I posted in my first thread. I am sorry for not claimed it. The error message is

Code:

--> FOAM FATAL IO ERROR: 
attempt to read beyond EOF

file: /home/wtj/OpenFOAM/wtj-2.3.1/run/tube/system/topoSetDict.actions at line 34.

    From function ITstream::read(token&)
    in file db/IOstreams/Tstreams/ITstream.C at line 83.

FOAM exiting

And I want to know what is the sintax of the invert and how can I check it? I am a greenhand in both OpenFOAM and English writing. So I am very eager for your help.
Best Regards.
And thanks again.

Nicole · May 28, 2015, 05:22

Hi,

I am definitely not as skilled with this as Alex, so I can't help you with the invert, but we found a really simple way to do this using blockmesh.

Firstly, when you define your hex blocks in blockMeshDict you simply define the "zone name" for example:

Code:

hex (1  0  9  12 16 15 24 27) Air (10 10 10) simpleGrading (1 1 1) //0

Then, in toposet all you need to do is this:

Code:

    // air
    {
        name    Air;
        type    cellSet;
        action  new;
        source  zoneToCell;
        sourceInfo
        {
            name "Air";
        }
    }
    {
        name    Air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set Air;
        }
    }

And you can do this for all of the zones to regions. I am not sure if this will work for you (I am a novice myself), but it worked really easily for us.

Regards,
Nicole

alexeym · May 28, 2015, 05:42

Hi,

Maybe I am late but the problem is in missing space between p1 and (0 0 0). You see, p1 is a label and it should be separated from the vector it labels

The same thing with p2.

zfaraday · May 28, 2015, 06:19

Quote:

Originally Posted by Nicole

Hi,

I am definitely not as skilled with this as Alex, so I can't help you with the invert, but we found a really simple way to do this using blockmesh.

Firstly, when you define your hex blocks in blockMeshDict you simply define the "zone name" for example:

Code:

hex (1  0  9  12 16 15 24 27) Air (10 10 10) simpleGrading (1 1 1) //0

Then, in toposet all you need to do is this:

Code:

    // air
    {
        name    Air;
        type    cellSet;
        action  new;
        source  zoneToCell;
        sourceInfo
        {
            name "Air";
        }
    }
    {
        name    Air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set Air;
        }
    }

And you can do this for all of the zones to regions. I am not sure if this will work for you (I am a novice myself), but it worked really easily for us.

Regards,
Nicole

Wow Nicole!! Your post really shocked me...

I totally agree with you with the first part of your post, defining your regions in blockMesh can ease the topology definition of your geometry. However, I don't get the second part... when you define your regions by naming the blocks in blockMesh you don't need to use topoSet because both actions have the same aim: to create cellZones. Thus, it makes no sense to me what you suggested because after you have named the blocks in blockMesh, the cells within the blocks become cellZones with the same name. Then, if you look at the topoSetDict you proposed, what you are doing is taking the cellZones created with blockMesh so as to create a cellSet and, after that, you take this cellSet to convert it AGAIN into a cellZone!!

Btw, is it correct to use quotation marks to encolse the name within when you define the name of the zone to be converted into a cellSet? Just asking... I'm not sure about it..

@alexeym: Thanks to point out that it only was a dumb mistake! :P Typical when you are new in this world, all of us have passed through it! I didn't even realised about this "little" mistake...

Regards,

Alex

Nicole · May 28, 2015, 06:26

Hi Alex,

Thanks for the advice. I did this a while ago and it worked pretty well. Next time I work on a multiregion system I'll try without topoSet. Thanks!

wtjhaha · May 28, 2015, 21:19

Quote:

Originally Posted by alexeym

Hi,

Maybe I am late but the problem is in missing space between p1 and (0 0 0). You see, p1 is a label and it should be separated from the vector it labels

The same thing with p2.

What a silly mistake I have made... Thank you for your help! It confused me a lot for a long time!

wtjhaha · May 28, 2015, 21:20

Quote:

Originally Posted by Nicole

Hi,

I am definitely not as skilled with this as Alex, so I can't help you with the invert, but we found a really simple way to do this using blockmesh.

Firstly, when you define your hex blocks in blockMeshDict you simply define the "zone name" for example:

Code:

hex (1  0  9  12 16 15 24 27) Air (10 10 10) simpleGrading (1 1 1) //0

Then, in toposet all you need to do is this:

Code:

    // air
    {
        name    Air;
        type    cellSet;
        action  new;
        source  zoneToCell;
        sourceInfo
        {
            name "Air";
        }
    }
    {
        name    Air;
        type    cellZoneSet;
        action  new;
        source  setToCellZone;
        sourceInfo
        {
            set Air;
        }
    }

And you can do this for all of the zones to regions. I am not sure if this will work for you (I am a novice myself), but it worked really easily for us.

Regards,
Nicole

Thank you for your advice! I will try it later on.

wtjhaha · May 28, 2015, 22:23

Quote:

Originally Posted by zfaraday

Wow Nicole!! Your post really shocked me...

I totally agree with you with the first part of your post, defining your regions in blockMesh can ease the topology definition of your geometry. However, I don't get the second part... when you define your regions by naming the blocks in blockMesh you don't need to use topoSet because both actions have the same aim: to create cellZones. Thus, it makes no sense to me what you suggested because after you have named the blocks in blockMesh, the cells within the blocks become cellZones with the same name. Then, if you look at the topoSetDict you proposed, what you are doing is taking the cellZones created with blockMesh so as to create a cellSet and, after that, you take this cellSet to convert it AGAIN into a cellZone!!

Btw, is it correct to use quotation marks to encolse the name within when you define the name of the zone to be converted into a cellSet? Just asking... I'm not sure about it..

@alexeym: Thanks to point out that it only was a dumb mistake! :P Typical when you are new in this world, all of us have passed through it! I didn't even realised about this "little" mistake...

Regards,

Alex

Thanks a lot! It's really kind of you to give me a lot of help in my OpenFOAM study!

alexeym · May 29, 2015, 02:13

Quote:

Originally Posted by wtjhaha

What a silly mistake I have made... Thank you for your help! It confused me a lot for a long time!

In fact I would not call it "silly mistake" but "shitty, useless error message". Instead of limiting search range by sourceInfo sub-dictionary and failing with "p1 was not found", OpenFOAM decides to read till the end of the file.

Rasmusiwersen · October 3, 2019, 06:01

Holy moly...

My error was somewhat the same as most recently suggested- Missing ";" in the end of each line (except sourceInfo) caused the same problem for me.

I know the post is hold, however this hopefully helps whoever might have the same problems.

/Rasmus

May 27, 2015, 08:22		#3
zfaraday Senior Member Alex Join Date: Oct 2013 Posts: 337 Rep Power: 21	I'm not sure what this error means, although I think I had to face it in the past. However, by reading your topoSetDict file I saw something weird that can be causing the problem, or maybe can cause another problem instead. First of all, you are creating a cellSet named air which is a cylinder. After that it is converted into a cellZone. The next step consists in the creation of another cellSet called tube with the same cells that make up the air cellSet, next you convert it into another cellZone with the result of two diferents cellZones made up with the same cells... I'm not sure if it can be done...I think that if a cell already belongs to a cellZone it cannot be part of another cellZone. As per my experience I think you may have missed a step in your topoSetDict, namenly the step when you invert your selection in odrer to select all the cells that don't belong to the air cellSet to create the tube cellSet. Am I right? Hope it helps. Alex __________________ Web site where I present my Master's Thesis: foamingtime.wordpress.com The case I talk about in this site was solved with chtMultiRegionSimpleFoam solver and involves radiation. Some basic tutorials are also resolved step by step in the web. If you are interested in these matters, you are invited to come in!

May 28, 2015, 05:22		#8
Nicole Member Nicole Andrew Join Date: Sep 2014 Location: Pretoria, South Africa Posts: 58 Rep Power: 11	Hi, I am definitely not as skilled with this as Alex, so I can't help you with the invert, but we found a really simple way to do this using blockmesh. Firstly, when you define your hex blocks in blockMeshDict you simply define the "zone name" for example: Code: hex (1 0 9 12 16 15 24 27) Air (10 10 10) simpleGrading (1 1 1) //0 Then, in toposet all you need to do is this: Code: // air { name Air; type cellSet; action new; source zoneToCell; sourceInfo { name "Air"; } } { name Air; type cellZoneSet; action new; source setToCellZone; sourceInfo { set Air; } } And you can do this for all of the zones to regions. I am not sure if this will work for you (I am a novice myself), but it worked really easily for us. Regards, Nicole

October 3, 2019, 06:01	Another "silly mistake"	#16
Rasmusiwersen Member Rasmus Iwersen Join Date: Jan 2019 Location: Denmark Posts: 81 Rep Power: 8	Holy moly... My error was somewhat the same as most recently suggested- Missing ";" in the end of each line (except sourceInfo) caused the same problem for me. I know the post is hold, however this hopefully helps whoever might have the same problems. /Rasmus

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
UDF compiling problem	Wouter	Fluent UDF and Scheme Programming	6	June 6, 2012 04:43
Gambit - meshing over airfoil wrapping (?) problem	JFDC	FLUENT	1	July 11, 2011 05:59
natural convection problem for a CHT problem	Se-Hee	CFX	2	June 10, 2007 06:29
Adiabatic and Rotating wall (Convection problem)	ParodDav	CFX	5	April 29, 2007 19:13
Is this problem well posed?	Thomas P. Abraham	Main CFD Forum	5	September 8, 1999 14:52

May 27, 2015, 06:54		#2
Nicole Member Nicole Andrew Join Date: Sep 2014 Location: Pretoria, South Africa Posts: 58 Rep Power: 11	Hi, I have not seen your error message before. Are you by any chance using blockMesh to mesh your domain?

May 28, 2015, 05:42		#9
alexeym Senior Member Alexey Matveichev Join Date: Aug 2011 Location: Nancy, France Posts: 1,930 Rep Power: 38	Hi, Maybe I am late but the problem is in missing space between p1 and (0 0 0). You see, p1 is a label and it should be separated from the vector it labels The same thing with p2.

May 28, 2015, 06:26		#11
Nicole Member Nicole Andrew Join Date: Sep 2014 Location: Pretoria, South Africa Posts: 58 Rep Power: 11	Hi Alex, Thanks for the advice. I did this a while ago and it worked pretty well. Next time I work on a multiregion system I'll try without topoSet. Thanks!