[dbagtbag]

Hey,

I'm conducting a study of the intake charge as the a cylinder engine breathes during its intake cycle. The way I have the simulation set up right now I have two domains, the intake and the cylinder crown, and the cylinder itself, which will be host to mesh deformation. To preserve an acceptable mesh density as the piston descends, my idea was to initially mesh the cylinder into hundreds of layers of elements. That way as the piston descends I will still have an acceptable number of elements to capture what is going on in the piston.

However, in the ANSYS mesh, Although I apply mapped face meshing and get a nice grid on the cylinder wall, the thin layers I see on the surface don't propagate inside. Is there a way to allow the surface mesh to penetrate throughout the domain or is remeshing the only way to handle large geometry changes like this?

Any help or suggestions are welcome.

All the best,

Yu

[ghorrocks]

Can you post an image of the problem?

[dbagtbag]

Sure.

I've been doing a lot of reading and trial and error and I've decided to try out the ICEM Remesh because it seems like a more logical solution after thinking about it a little bit more. I figured its better to have elements of consistent geometry rather than stretching many layers of pancaked elements as the piston moves.

I've attached a image of my mesh generated using ICEM. The purple is the cylinder wall and the orange is the piston. I've managed to get the re-Mesh process underway but I get this message after the mesh has been generated:

+================================================= ===================+
| ****** PROBLEM REPORT ****** |
|--------------------------------------------------------------------|
| Subsystem: Input and Output |
| Subroutine name: ErrAction |
| Severity level: Fatal Error |
| Error message number: 001100279 |
|--------------------------------------------------------------------|
| Message: |
| |
| REDHDR: locating dataset failed: what=G/NAMEMAP where=EVERY |
| |
| |
| |
| |
| |
+================================================= ===================+
WARNING: CFXSTP, Regression check error.

This is what my remesh setup looks like:

The geometry file is the tin generated when I exported the ICEM mesh to FLUENT format.

Body is the entire fluid domain, intake and cylinder. This is a single domain case.

Thanks,

Yu

[ghorrocks]

Your first post asked about the inflation layers not propogating into the mesh. Your second post asks about a different error. What is your question? If it is the first then please post an image of the cross section of the mesh you do get.

[dbagtbag]

It is the second. I apologize for the confusion.

I've been putting off learning icem remeshing because I never really liked to work with ICEM but I figured that it would be something worth figuring out and getting good at for my own sake so I decided to switch methods.

[ghorrocks]

ICEM is a much more powerful mesher so time spent learning it is time well spent in my opinion.

I have no experience in remeshing in ICEM so cannot help you much. A few other members on the forum have experience in this area so they might be able to help you.

But as a side issue, my PhD thesis was in using CFX for IC engine modelling. Here is the link if it is of interest to you: http://hdl.handle.net/2100/248 As this work is over 10 years old I did not use any remeshing, it was complex enough getting the thing to work at all on the software available at the time even without remeshing.

[dbagtbag]

I think so too, and I guess I'll have to wait and see if anyone has any suggestions then.

Meanwhile I'm reading through your thesis and its very interesting. Will need to put it down for tonight because its a thesis and they are lengthy (you would know you wrote it). Rotary valve engines being such a rare breed is difficult to find information on. I've always wondered why the industries haven't taken up the idea. It seems to be a more sound engineering solution than poppet valves and I'm sure the challenges can be overcome with good research.

cheers,

Yu

[ghorrocks]

We did overcome the technical challenges See http://home.people.net.au/~mrbdesign...utoTechBRV.pdf

What killed the project was political, not technical.

[dbagtbag]

Ghorrocks thats a brilliant article. The particular engine I'm working on happens to be a very high rpm engine as well, 17000+rpm =)

So I've been screwing around a little bit more with ICEM and because the locating dataset failed message was rather familiar I thought it was due to the remeshed mesh not getting back to CFX. I added a number of lines to my replay script to change the working directory of the script to where I store my mesh and tin files.

Then it gave me this:
+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| ANSYS CFX Solver Input File does not exist |
+--------------------------------------------------------------------+


+--------------------------------------------------------------------+
| The following user files have been saved in the directory G:/Ansys |
| Temp/Cylinder Head Airflow_4832_Working/dp0/CFX-3/CFX/Work1/Copy |
| of CFX New_001: |
| |
| temp.fbc, temp.uns, cfx5mondata.out, tetra_cmd.log, temp.fbc_old, |
| 16_newmesh_01.mesh.log, temp.fbc_dfupdate, |
| cfxpre_engine_error.log, 16_oldmesh.res, 16_remesh.out |
+--------------------------------------------------------------------+

Does anyone know anything about this or any details on how the relevant files are managed during the remeshing process?

best,

Yu

[dbagtbag]

I know I'm bumping a old thread but I figured it out so I'm going to put the important things that I realized to make it work here. Its for future reference of anyone whos having similar problems.

For ICEM Remeshing, you need to do be very strict about the following:

Define ALL of your parts in ICEM. This includes the body of the model in question. When I was first racking my brain over the error message

REDHDR: locating dataset failed: what=G/NAMEMAP where=EVERY

It was simply because I let the mesher create the body, and it was named CREATED_MATERIAL_XXX whenever the remesher ran. This does not work and you need to give it a part name so it can reference it any time.

You don't need to include the export mesh command in the replay file.

Another reason I was getting errors was because I included the export mesh command in my replay file, seeing that you could specify different mesh formats when specifying your remesh configuration. This will work if you remesh once, but will not for subsequent remeshes because of the way CFX handles the files that come out of the replay scripts.

Make sure your units are correct

CFX and ICEM both require unit specification. The geometry scale option can provide some scaling but in my experience this option has given me trouble. The easiest thing to do is make sure all the units from model creation to solver are consistent.

Hope this helps some people out.

Best,

Yu

[MaBe]

G'day mates,

my Name is Marius and I would like to know, if you really understood and solved this problem because I'm also simulating a cylinder flow and i got the same Error.

This is what my out file says:
************************************************** *********************
Solver ANSYS CFX supports unstructured mesh.
Loading /ansys_inc/v161/icemcfd/linux64_amd/icemcfd/output-interfaces/cfx5.bcinfo
Current solver is ANSYS CFX
Solver ANSYS CFX supports unstructured mesh.
Saved family boco data to ./temp.fbc
Writing domain "./temp.uns" ...
Done saving domain file.
Exit from ICEM CFD
Batch run of "/home/mabe/work/Workstation/20150729_001/C1_001.dir/meshUpdate.pre" failed due to the following errors:

-- WARNING -- This results file contains multiple meshes. The latest mesh will be loaded, which will be the deformed mesh for a case that includes Mesh Deformation. If the original undeformed mesh is required, you should load the case file (.cfx) or the CFX-Solver input file (.def) instead.


-- ERROR --
The location of domain "Flow Domain 1" is invalid:
Region "Assembly" is not recognised.
************************************************** ****************************************



Solver Error:


Job started: Wed Jul 29 12:49:52 2015

+================================================= ===================+
| ****** PROBLEM REPORT ****** |
|--------------------------------------------------------------------|
| Subsystem: Input and Output |
| Subroutine name: ErrAction |
| Severity level: Fatal Error |
| Error message number: 001100279 |
|--------------------------------------------------------------------|
| Message: |
| |
| REDHDR: locating dataset failed: what=G/NAMEMAP where=EVERY |
| |
| |
| |
| |
| |
+================================================= ===================+
WARNING: CFXSTP, Regression check error.

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| Error interpolating results onto the new mesh: |
| /ansys_inc/v161/CFX/bin/linux-amd64/double/solver-pcmpi.exe exited |
| with return code 1. |
+--------------------------------------------------------------------+



The job stops just one crank angle after starting.




I don't know what to do. Do I have a bad mesh? Why does it say "Region Assembly is not recognized"? I normaly don't have this Region/Part.

I also tried a smaller timestep and and a smaller remesh criterion (Orthogonality Angle Minimum <5°).

Does anyone know about this Problem? This is driving me nuts....

Many thanks in advance for your reply!

Cheers Marius

[ghorrocks]

It sounds like a problem with remeshing and the part names you have defined.