CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   Inlet Velocity in CFX (https://www.cfd-online.com/Forums/cfx/67140-inlet-velocity-cfx.html)

 aeroman August 5, 2009 10:08

Inlet Velocity in CFX

OK..I've been through the documentation and believe I have exhausted all other references and I have a question.

I am wanting to have an initial constant inlet velocity for a given time and then have the inlet velocity change with respect to the net forces acting on an obstruction in the x direction in the domain.

To expand, I have water entering an air domain with a velocity of say 10 m/s. Then, when the water reaches the obstruction, I am wanting to implement v=dtstep(g-(netforce/mass))-Vold. Essentially, I am describing the movement of the obstruction by varying the inlet flow.

I have tried to carry this out a few ways with no success. First, I defined an initial inlet velocity of 10 m/s and then specified the velocity at the inlet as Vnew, where Vnew was Vnew=dtstep(g-(force_x()@wall)/Mass)-probe(u)@monitorpoint. The mass is the mass of the obstruction defined by the volume and density. I put the monitorpoint in line with the obstruction in the farfeild (i.e. far enough away so as not to pick up velocity fluctuations due to the obstruction). Further, I tried putting the obstruction right at the inlet and at a distance from the inlet. Where the obstruction was right at the inlet, I put the monitor point at the inlet. Rather than using a monitor point, I have also tried using areaave and found that because the velocity fluctuates about the obstruction, average velocity at the inlet is affected.

I have also tried splitting up the domain into subdomains, whereby I have an inlet domain and a domain with the obstruction in it. I had hoped that I could use the inside()@subdomain to maintain a constant velocity until the water reached the obstruction domain, but it would appear that I was mistaken in the correct usage of this function (I think).

Because I am interested in large relative displacements and an accurate solution at the wall and thereafter, I am unable to just move the obstruction by deforming the mesh (and hence, use the mesh displacement for Vold, like in the FSI valve tutorial). I suspect that the CFX expression language can be used for this, I'm just lost as to how I can implement it. Any suggestions would be greatly appreciated.

 aeroman August 5, 2009 10:13

whoops

Note: I put the equations in backwards they are Vold+dtstep(g-(f/m)).

 ckleanth August 5, 2009 12:33

what if you use the subdomain to freeze the velocity of your phase at a spesified location (a bounding box with x,y,z relations)? you can write the ccl to have this freezing effect to capture your moving obstruction

(that is if I understood what you want to do...) why you change the inlet velocity anyway? whats the physical problem?

 aeroman August 5, 2009 12:48

hmmm

I'm not sure what you mean however. Lets say I have two subdomains 1 is an inlet domain and the other has the obstruction at the interface between the two domains. If I give the inlet domain a constant fluid velocity I can somehow freeze the inlet domain and begin recalculating flow velocity as the fluid enters the obstruction domain?

 ckleanth August 5, 2009 12:59

i still dont get what you want to do.. have any pics/schematic of the problem?

 aeroman August 5, 2009 13:01

physical problem

I got a little trigger happy with the submit button and didn't answer your question. The physical problem is an object entering the water with a given velocity. I want to change the inlet velocity since the velocity of the object will decay with time due to the net forces acting on it. It is important to the body entry dynamics that I model this velocity accuratly.

 aeroman August 5, 2009 13:11

Model

1 Attachment(s)
Please find attached a picture of the CAD model. the circular region is modeled as a no slip wall. the left wall is the inlet, the upper and lower walls are free slip walls. and the right wall is the opening.

 ckleanth August 5, 2009 18:55

well why not using the immersed solids?

if the mesh movement is not imposed and using mesh deformation the only forces acting on the object for example on x direction is: mass * X dot = fluid force X ;cant you do something similar as shown in the example found in the cfx manual?

if the mesh movement is imposed its pretty easy :confused:

 ghorrocks August 5, 2009 20:58

Hi,

Yes, I would consider using immersed solids with the 6DOF solver for this. Also in your original approach be careful about specifying a varying inlet velocity to model the body motion. This approach means you are using an accelerating frame of reference but the acceleration terms are not in the model - this can potentially cause errors.

Glenn Horrocks

 aeroman August 6, 2009 13:42

Thanks

I will have acess to V12 this tuesday and will use the immersed solids model as you recommend. This has been advised to me in a previous thread (thanks Glen). I see what you mean about the errors, I managed to fix the problem for the tme being, but am looking forward to using the 6dof solver in V12 (no doubt you will be hearing from me when I open that can of worms!!)

Thanks again

P.S. I now have a deep and profound interest in "hooning the chuffer"...:D

 aeroman August 6, 2009 14:13

one more question

Just one more quick question. In version 12 cfx mesh movement is carried out by compressing and stretching the mesh about the body. In fluent, the cells are removed and replaced as the body translates. For my problem, it would be a massive help if the cells could be removed and replaced since I need to travel many diameters to capture the physics of interest. I know I need to read up on this, and I will, but does V 12 CFX handle dynamic meshing like in fluent?

 aeroman August 6, 2009 14:24

ok, I answered my own question. immersed solids does not need to deform the mesh. I knew I should have read before writing.

But now I have another (less ignorant) question, for my ball moving from air into water the resolution of seperation at the wall and downstream turbulance is what I am wanting to model (mostly). From what I have read immersed solid solver does not solve near wall turbulant conditions. I'm not sure if I am understanding this correct, but it would seem that if I need an accurate simmulation of the seperation and turbulance aft of the ball/cylinder/obstruction, a solution of near wall turbulant conditions is important :confused:.

 ghorrocks August 6, 2009 18:42

Yes, you are correct. The immersed body model is not good at capturing accurate boundary layer flows. If the details of the boundary layer flow is important then immersed solids is not a good approach and you need to look at the moving mesh approaches.

Glenn Horrocks

 All times are GMT -4. The time now is 20:05.