CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   ANSYS Meshing & Geometry (http://www.cfd-online.com/Forums/ansys-meshing/)
-   -   [ANSYS Meshing] Multiple meshes for FLUENT (http://www.cfd-online.com/Forums/ansys-meshing/113381-multiple-meshes-fluent.html)

AntonZ44 February 18, 2013 20:35

Multiple meshes for FLUENT
 
Hi all,

I have a CAD assembly of five parts I can get to DM/ICEM. Three need to become "rotating" walls in FLUENT and two need to be stationary.

I am familiar with enclosing parts in a fluid then subtracting (boolean etc). However, subtraction from the fluid domain means I cannot later select faces by part, to name as "rotating" or "stationary".

I believe there is a way to do what I need using multiple meshes but can't find any documentation on it or similar. I have exhausted every avenue I can think of. I don't understand what is required of both meshes. (I am familiar with read->case and zone->append).

I can generate a fluid volume and subtract (and name), say, my moving parts. Should my second mesh then be my other parts with a fluid enclosure around them? Or does the second mesh need to be a thin wall solid? Or, most likely, am I totally on the wrong track?

Could anyone be as kind as to explain briefly what needs to be done?

Regards,
Anton

stuart23 February 19, 2013 09:49

Hi Anton,

Tmerge is a handy utility for Fluent which appends two meshes together. The programming just concatenates meshes, and will not check for shared faces or create interfaces etc. You must ensure that both meshes have been created relative to the same coordinate system before merging.

The command to start Tmerge on 14.0 is as follows. I have not yet looked to see if Tmerge is included in 14.5. The programming might take a long time to run, just wait. Even for large meshes (100M+), the memory use is still about 7MB, but the time taken increases with model size.

ansys_inc/v140/fluent/utility/tmerge14.0/lnamd64/tmerge_3d.14.0.0 -p -v 1st_input.msh 2nd_input.msh output.msh

AntonZ44 February 19, 2013 10:07

Quote:

Originally Posted by stuart23 (Post 408731)
Hi Anton,

Tmerge is a handy utility for Fluent which appends two meshes together.

ansys_inc/v140/fluent/utility/tmerge14.0/lnamd64/tmerge_3d.14.0.0 -p -v 1st_input.msh 2nd_input.msh output.msh

Thank you very much for your answer.

I read a bit about Tmerge (and Tgrid)...

What would the two mesh files I feed in to Tmerge look like?

For example
Mesh 1 - fluid enclosure with solid stationary parts
Mesh 2 - solids of rotating parts

or

Mesh 1 - fluid enclosure with stationary parts subtracted
Mesh 2 - custom shape enclosure of my rotating parts

or

Mesh 1 - my fluid box
Mesh 2 - my moving parts as solids
Mesh 3 - my stationary parts as solid

or..?

Thanks so much for your time
Anton

stuart23 February 19, 2013 10:22

Anton, this smells like some sort of turbomachinery, am I correct?

If your geometry is rotor-stator-rotor-stator, you should mesh all of the fluid domains separately and then merge them together at the end.

Taking one step back, I do not see why it is necessary for you to create desperate meshes for each cell zone, you should be able to do this by using material points in different zones in ICEM, or by creating desperate bodies in DM (use "add frozen" function)

I hope this helps, both ways get you to the same end result, however not using Tmerge would seem to be the simplest option.

Stu

AntonZ44 February 19, 2013 10:42

1 Attachment(s)
Thanks again buddy.

If it was rotor-stator-rotor I'd have no problem as the boundary between each region I'm trying to model would just be a plane normal to the shaft of my turbomachinery.

I've attached a stp of my CAD which is a wheel. The rim+tires, hub and rotor should be rotating about the x axis through 0, 0, 0. The caliper and upright parts need to be stationary.

As you can see, the boundary between all my parts is more complicated so it's more difficult to subtract these parts from a a enclosure to THEN manually select walls of the fluid to group.

stuart23 February 19, 2013 10:54

Sorry Anton, I am typing on my phone which doesn't have any CAD package installed (...yet). Can you upload a pic?

If you can find a surface of revolution about the rotational axis that you can use to divide the rotating and stationary domains, you can use that as your interface. With the interfaces defined, you could then use the frozen or transient rotor approaches.

Obviously the rotor/caliper contact is the most difficult to divide. Do you have a rotor that is a surface of revolution (i.e. constant axissymmetric cross section)? If so, the rotor could be defined in the stationary frame but just given a moving wall boundary condition.

Otherwise, I think you might be looking at a transient model with mesh morphing... This should only be considered as a last ditch effort (IMHO)

Stu

AntonZ44 February 19, 2013 12:53

1 Attachment(s)
Quote:

Originally Posted by stuart23 (Post 408753)
Sorry Anton, I am typing on my phone which doesn't have any CAD package installed (...yet). Can you upload a pic?

Here you go. My part in DM surrounded by an enclosure.

I need to define/named select the boundary of my fluid based on which part of my model the fluid touches.

I don't know how to do this:

If I subtract the shapes from my enclosure, I can only select boundaries *of the fluid enclosure* so would need to select each face by part manually/individually.

Leaving my solid in the enclosure doesn't seem to work either, I can then select my parts and the walls of my parts... but these are not the same as the fluid walls, right? It seems to be the interfacing between the walls of my solid and walls of my fluid that I'm clueless with here.

Any thoughts?

stuart23 February 19, 2013 19:09

Anton,

Just downloaded and opened your geometry. Looks very nice!

I'm not sure what the goal of your simulation is, but all of the rotating parts are surfaces of revolution, so you could apply a moving boundary condition. If you want to do conjugate eat transfer, you should be able to define the rotor solid domain as a rotating domain. Then add a heat source at the calipers face to heat both objects.


Stu

AntonZ44 February 19, 2013 20:32

Quote:

Originally Posted by stuart23 (Post 408862)
Anton,

Just downloaded and opened your geometry. Looks very nice!

I'm not sure what the goal of your simulation is, but all of the rotating parts are surfaces of revolution, so you could apply a moving boundary condition. If you want to do conjugate eat transfer, you should be able to define the rotor solid domain as a rotating domain. Then add a heat source at the calipers face to heat both objects.


Stu

Thanks :)

Not worried about heat transfer for now.

I can apply a moving boundary condition but only know how to do that for the entire assembly. *I don't know how to split up the boundaries such that FLUENT allows me to set one set of boundaries as rotating and another as stationary.*

Does this make sense? Sorry, I really feel I'm miscommunicating the problem here despite my best efforts!

stuart23 February 20, 2013 08:11

Hi Anton,

I managed to create a really cool transient conjugate heat transfer simulation using your geometry. If you're lucky, I will upload it.

Assuming you are using Ansys Meshing, you need to create Named Selections to specify the different surfaces. Once specified, you can define the rotating parts as rotating walls. You must define a point and direction for the rotational axis. Fluent calculates your rotation from this using the right hand rule. I also defined the ground as a translating wall so that the velocity at the contact patch was the same as the velocity on the ground.


If you do go down the heat transfer path, you need to use a Dirichlet BC, not a Neumann like I first did! If you try to dump all the energy from the vehicle kinetic energy through the boundary condition (constant heat flux), the temps near the surface approach 1000C! You can either use a constant surface temp, or interface with a solid zone for conjugate heat transfer. I took this approach, and created a volume source to generate the heat in the solid domain (rotor).

Stu

AntonZ44 February 20, 2013 08:40

Quote:

Originally Posted by stuart23 (Post 408984)
Hi Anton,

Assuming you are using Ansys Meshing, you need to create Named Selections to specify the different surfaces. Once specified, you can define the rotating parts as rotating walls. You must define a point and direction for the rotational axis. Fluent calculates your rotation from this using the right hand rule. I also defined the ground as a translating wall so that the velocity at the contact patch was the same as the velocity on the ground.


That sounds absolutely awesome!

This is the bit I'm having difficulty with. I'm subtracting my solid from my fluid volume. When I subtract the solid I lose my named selection of the parts!

Meanwhile, if I leave my solid in, surrounded by a fluid, then I still can't get the fluid walls as named selections. I can set up my parts as named selections. But these selected parts are treated seperately to the fluid boundary where the fluid meets these selected parts, they're different and I can't set properties for the part.

Maybe the easiest thing would be for you to just upload the DM and mesh files so I can see how your named selections are set up :D

Thanks so much for your time, what you've done sounds unbelievably cool!

Anton

azna February 23, 2015 15:30

Hi,

Im trying to use Enclosure option in Ansys workbench (Fluent), however After I generate Enclosure, I can't select the main body which is inside this. I need to define inside body as a inlet and solid walls, however it's impossible to select faces, can anybody help me with this ?

Thanks


All times are GMT -4. The time now is 19:45.