CFD Online Discussion Forums

CFD Online Discussion Forums (
-   STAR-CCM+ (
-   -   moving object in a pool (

JohnAB July 25, 2013 17:34

moving object in a pool

I have a simple question:

I have a region 1 (fluid, free surface, Physics 1, mesh 1, like a box half filled with water) which is like a pool, i.e. there is no flow and nothing is moving, and the whole thing is fixed.
What I want to do is to import a body that would be partly submerged and move in the pool. The water in the pool would then react to that and we would see some little waves.
This body is not like a boat, the water has no influence on its motion, it's completely predefined (therefore I cannot use the DFBI model).

Should I import this body as a new region or a part within region 1 ? If it is a part within region 1, how can I make this part move but not region 1 ?

I imported it as a new region (physics 1, mesh 2), was able to move it and give it the trajectory I want in the pool, but the water does not react at all.
I tried to define a new physics continuum (solid, physics 2) as well, without more success.
It looks like the water completely disregards the moving object.

The rotation turbine tutorial does not help either...

Thanks for your help

JohnAB July 25, 2013 20:18


I have just tried to let this object drop into the pool, using DFBI method, just to see if at least this works.
The object goes through the pool without even doing anything, like it is in a complete different world.
So I guess the issue is how I imported that object and that it shouldn't be defined as a new region, right ?

But then how can I solve my problem ? I tried to import it as a part, but I could not make it move...


siara817 July 26, 2013 07:08

There is a sample in tutorial simulating a boat.
Try to search Boat in Head Waves in the tutorial.

JohnAB July 26, 2013 11:54


thanks for your answer. Unfortunately, even if I follow every step of the tutorial (I have read it hundreds of times) it still does not work, maybe because I am not using head wave but a field function for the water, and maybe because in this tutorial the boat is imported with the rest of the geometry at once, and that in my case I have my pool and my object as two seperate models/meshes...

Maged_CFD July 26, 2013 14:12


You need to import your solid body into parts, create a block around it, and then subtract the solid body from the block. The resulting part that contain the surface of the solid body should be used as the overset region (Assign Parts to Regions).

This will give you a similar setup as in the Lifeboat tutorial. However, in your case, you should define a Motion of type Rotation and Translation, rather than the DFBI motion used in the Lifeboat tutorial.

Check the user guide for more details on setting up the overset region: Modeling Physics > Using Overset Meshes > Preparing Overset Regions

JohnAB July 26, 2013 14:47


Thanks! I will try to explore that right now. There is another thing I forgot to precise, I'm using Star CCM+ version 6, and there is no overset possibility in that version (I believe it was put into v7 and followings, not v6).

Another question, if I do what you say, won't my pool (the whole domain) move as well ? Because in the DFBI tutorial, the boat moves, but I believe that the whole domain as well (i.e. the walls are moving like the boat), and I do not want my pool to move, I just want my object to move in the fixed pool. And again, I do not think I can do overset in version 6...

Henry Arrigo July 26, 2013 16:44

Hi John
the process is like this, first you should subtract your body from the domain. you can do this in STAR-CCM+ itself or by a CAD modeler and then import the resulting geometry into STAR-CCM+. Doing so you will have a single region. To move the object you can use Morpher. If you use this option you don t need to have two regions, it completely definable with a single region. In this case STAR-CCM+ moves the object by deforming the mesh.
There is just one problem: I implied this procedure one time but i m not sure that the software exactly impose the predefined motion, but you can try your case. Maybe i did something wrong.

JohnAB July 31, 2013 17:43

Maged_CFD, Henry,

I have decided to install Star CCM+ 8.04 and was able to do what Maged said, like in the lifeboat tutorial. I have a very simple geometry which is:

region 1: a box, half-filled with water, set as my "background".
region 2: Overset, a simple small cube half submerged inside that box (actually a subtract block - cube). This cube would be my moving element that would translate from one point to another.

I imported my cube as a part, created the box around it, made sure there is enough space between the edges of the cube and the edges of the block so there is no problem with the acceptors cells. I subtracted the cube from that block and assigned that block to a new region called Overset.

When I check the cell status, everything is fine, like said in the help "preparing overset regions".

However, like in this same help page, I get the "failed to cut hole in region 1" error.
My geometry is so simple that I don't think I made any mistake following the lifeboat tutorial, and the base sise of my background mesh and my overset mesh are the same, which should not cause any problem I guess.

Do you have any idea why I get this error message ?

Roman August 20, 2013 03:02

Hi John

I know I am kind of late for this, but have you created an interface between background and overset regions? To do this mark both regions, right click on them, create interface, overset mesh. Now your regions should communicate properly.


JohnAB August 21, 2013 17:49


thanks for you advice, but yes that is one of the things I have done (I followed the tutorials). However, in my case I am able to make this work a very small scales (order of magnitude: cm, which is small for a real pool...), but then when I go bigger (order of magnitude: meter) and increase the size of the mesh proportionally, it does not work anymore... It still says "failed to cut whole in [background] region". I tried to refine the mesh a little bit, no success...

Roman August 22, 2013 05:25

This sounds like a problem with the overset interface. It usually spits out the same error if you try to right click and initialize the interface manually. This is probably due to coarse mesh?

Another suggestion would be to double check that your overset box and your cube are actually in separate boundary's in "region 1" and that overset boundary is set to "overset mesh" type.

Also I often find that grid size does not scale well when going from small to big, you often have to refine more in "Full scale" simulations to better capture free surface of the water and object interaction.

Any chance for a screenshot of the grid?

All times are GMT -4. The time now is 06:34.