CFD Online Discussion Forums (https://www.cfd-online.com/Forums/)
-   CFX (https://www.cfd-online.com/Forums/cfx/)
-   -   find choking range in orifice (https://www.cfd-online.com/Forums/cfx/114083-find-choking-range-orifice.html)

 omidiut March 5, 2013 02:08

find choking range in orifice

Hi all
I'm trying to simulate flow in orifice plate. How can i find when orifice will be choked? for capture choking steady state solution is better or transient solution?

Best regards

 oj.bulmer March 5, 2013 07:39

Not too much experience with this, but from what I read, a choked flow is a flow where, for fixed inlet pressure, any decrease in outlet pressure will not result in increase in mass flow rate. Now, this should involve series of simulations to find this minimum outlet pressure.

I would start with steady compressible flow (ideal gas density, since choked flow velocities reach Mach 1 region) with relatively coarse mesh to simulate the initial physics to get it right. Once you get an approaximate outlet pressure beyond which any decrease will not result in significant increase in mass flow, you may want use a proper refined mesh and then choose pressures close to this value to get even better estimation for the threshold pressure.

In case if you find the solution not converging to your satisfaction, you may want to try transient. But it would be cheaper to use steady state solution to arrive at approaximate range of choking outlet pressure, before switching to transient.

Regards
OJ

 ghorrocks March 5, 2013 19:57

You should be able to estimate the choking pressure using simple compressible flow analytical equations.

 omidiut March 6, 2013 02:13

Thank you for your replies dear oj.bulmer and ghorrocks

i'm trying to investigate some parameters such as thickness of orifice(or length of orifice), multi holes orifice, multi stage orifice, and simple compressible flow analytical equations are not usefull.

What is the accurate or valid boundary condition? i use inlet pressure and outlet pressure to compare massflow rate at each boundary but overflow errors accure, when i use massflow rate in inlet boundary and pressure outlet convergence reach difficultly but maximum mach number is 4.5.

inlet pressure is 150 bar with massflow rate 5.71 kg/sec and outlet pressure is 7 bar.

i trying to simulate it as transient method but overflow errors accures.

Best regards.

 ghorrocks March 6, 2013 18:37

The best boundary condition for this type of simulation is a total pressure inlet and a pressure outlet. But convergence of these type of simulations is tricky, use a bit of local tiem scale factor to start off and after it has converged a little switch to physical time step.

 oj.bulmer March 7, 2013 05:50

Glenn,

I have a fundamental query about local timescales.

I learn that for the local timescale, it is the number of cells that intersect a typical flow path from the inlet to the outlet that is significant. For subsonic flow speeds, pressure information propagates upstream from the outlet to the inlet.

The CFX manual only warns about using the local timestep because you need to ensure you have run for enough iterations to reach a steady solution and for all the boundary information to have propagated throughout the mesh. A local timestep of 5 with 80 iterations implies that the maximum distance any information could have travelled across the mesh is 5*80 = 400 cells.

If this is the case, and if we are working with a mesh of, say 3 million, would local timescales be any economical?

OJ.

 ghorrocks March 7, 2013 18:03

Yes, I frequently use local time scale for tricky to converge simulations, especially transonic ones. Your understanding of local time scale does not seem correct - local time scale simply uses a time scale set at each element (Courant number I suspect) and that means high courant number elements get a small time step to aid convergence and low courant number elements get a bigger time step to speed convergence, up until all elements are running with a similar courant number. There is nothing special about solutions wandering upstream or downstream or anything like that.

The implications of this variable time step is that some parts of the flow may have only advanced a very small amount of time, but the rest of the flow has advanced a lot. So things which often take a while to converge in physical time (eg heat balance) will be inaccurate. To fix this you run a few time steps of physical time stepping at the end to make sure everything has run a minimum amount of physical time.

 oj.bulmer March 8, 2013 08:49

Quote:
 Your understanding of local time scale does not seem correct
Am sorry I didn't make myself clear and I agree, the unintended interpretation of my statement may make it seem like imbecilic. I read this reference:

Van Doormaal, J. P., and G. D. Raithby. "Enhancements of the SIMPLE method for predicting incompressible fluid flows." Numerical heat transfer 7.2 (1984): 147-163.

The manual explains about the non-uniform timescale spatially (depending upon courant number and all) as you mentioned but doesn't go deep. The paper above explains it to a bit more extent. I was contemplating on the whole situation as follows:

Typically with physical timestep, as I understand, the solver proceeds with pseudo transient manner. Essentially, for smaller timestep, the coeffocient will be large and solution will be slow, universally.

With local timescale, as I interpret, the pseudo transient approach is abolished and the coefficient is modified as:

The term , now gives a CFX timestep as and thus incorporates the temporal aspect.

Essentially, the factor E multiplies the timescale for cell, . A factor of 5 would mean for a single iteration of timestep, the solution will travel 5 times faster than when time step is for a particular cell. Thus solution propagates farther (400 cells) for less no. of timesteps (80 iterations), provided they are of similar refined size etc.

Now the catch is, for very fine grids, and near boundary layers etc, the solution slows down significantly. So even factor 5, 10 etc takes eons for larger meshes. The situation is aggravated with highly skewed cells. Thus I was thinking, is it worth it for large unstructured meshes?

Sorry for being elaborate. I may be wrong and perhaps obvious, but then I was lost in thoughts. And sharing might help bring some clarity :)

 ghorrocks March 9, 2013 02:34

* CFX is a coupled solver and does not use SIMPLE. Your analysis is based around a SIMPLE solver.
* CFX uses a multigrid solver which achieves rapid convergance (most of the time :) ) even on fine grids
* CFX is pretty robust against skewed cells.

So your analysis is not very relevant to CFX.

 oj.bulmer March 9, 2013 09:13

Agreed, I understand it is a coupled, and hence rapid (relatively smaller iterations) solver as compared to segregated solvers. But I was just getting my head around the implementation of local timescale factor in CFX, and not trying to generalize the CFX's solving algorithms. Recall that CFX did have a default SIMPLEC based solver previously. Is it fair to say that though they changed it to multigrid coupled solver later, they retained the implementation of local timescale factor (perhaps as illustrated in the paper about SIMPLE algorithm)?

Also, I agree it handles skewed cells pretty well compared to FLUENT, but these have very high ap value and hence a reasonable value of E is yet not enough to advance them in time as we'd wish, again in the context of local timescales. We still assemble the implicitly coupled linear equations to solve, but then, the pace of solution in its entirety, is limited by these slow fine regions. Especially if you have relatively non-uniform mesh, switching to physical timescale earlier than appropriate time will still pour convergence difficulties :)

 ghorrocks March 10, 2013 07:29

CFX3 and 4 used SIMPLEC as a default solver. CFX5 (which is the first in the current series of solvers) used the fundamental solver technology developed in TASCFlow (ie coupled solver). CFX has had multigrid linear solvers for all releases I can recall. SIMPLE, SIMPLEC or any of its derivatives is not an available option in any recent CFX releases.

 omidiut March 11, 2013 08:19

I use local time scale and overflow error doesn't appear. convergence is too difficult. by local time scales in order 0.01 there is a notification about high mach number about 400 with small time scale this notification does not appear. after convergence i probe massflow rate at inlet and outlet boundary...these are equal...but how can i understand flow is choked or not?
I would like to study the effect of thickness and bore size of orifice on choking range of it with constant mass flow and pressure at inlet boundary....

Best regards.

 ghorrocks March 11, 2013 17:42

Local time scale factors of 5 are the range you normally use. If you are using 0.01 with Mach 400 somehwere then soemthing is seriously wrong with your setup.

If you have a transonic simulation then you will need very good mesh quality. Can you post a picture of your mesh?

Even better, put the residuals in the results file and use them to indentify where in the simulation the high residuals occur. That shows you what area you need to improve - by meshing the area better.

 omidiut March 12, 2013 01:34

1 Attachment(s)
Thank you for your attention dear Glenn
attached file is a picture of mesh, there is about 462235 element.

There is a pipe with 82.804 mm diameter and orifice with 17.14 mm bore diameter. thickness of orifice is about 12.7 mm. Upstream pressure is 150 bar and down stream pressure is 7 bar. mass flow rate of CH4 is 5.712 kg\s.

setup of this problem seems to be simple, have you any comment about it?

Best regards.

 ghorrocks March 12, 2013 07:04

I presume this simulation is axisymmetric? You should model a thin wedge in that case. Shame CFX does not have a true 2D model like Fluent, that would be very useful for this case.

You may need to extend the downstream boundary further downstream at this Mach/Re number. The separation is going to be huge and you probably have back flow where you currently have it.

 omidiut March 12, 2013 07:26

With better mesh quality i can finally improve rate of convergence. Know my basic question is: How can i find flow is choked of don't? if not how can i find choking range to study effect fo other parameter on choking?

Best regards.

 ghorrocks March 12, 2013 07:28

Increase the pressure ratio. If the flow rate does not change it is choked.

 omidiut March 12, 2013 07:30

Yes it is axisymmetric , but for include turbulence effect i simulate whole 3 D of model. the max. of mach number is 4.58. i haven't any data about experimental investigation and don't know is this mach number is physically correct or not.

 omidiut March 12, 2013 07:31

Quote:
 Originally Posted by ghorrocks (Post 413384) Increase the pressure ratio. If the flow rate does not change it is choked.
How much increase it? decrease only downstream pressure?

 oj.bulmer March 12, 2013 07:56