# normal shock in convergent-divergent nozzle

 Register Blogs Members List Search Today's Posts Mark Forums Read

December 17, 2016, 13:27
normal shock in convergent-divergent nozzle
#1
New Member

Fabio
Join Date: Dec 2016
Posts: 4
Rep Power: 2
Hi, I'm new here.

I'm writing because I have a problem with a simulation.
Considering air flowing through a convergent-divergent nozzle having a circular crossectional (attached mesh image), I simulated a subsonic flow in the converging section and a supersonic flow in the diverging without problems.
You can see project datas below.

The variation formula with axial distance from the throat is

A = 0.1 + x2; -0.5 < x < 0.5

The stagnation pressure p0 at the inlet is 101325 Pa.
The stagnation temperature T0 at the inlet is 300 K.
The static pressure p at the exit is 3738.9 Pa.
The model is considerated inviscid.

As result, I need to have a normal shock in the diverging section, but the datas that I obtained are not considerable. In fact, if the static pressure at the exit is:
- set between 34000 Pa and 45000 Pa, the residuals go to infinite;
- greater than 45000 Pa, the residuals oscillate between 1 and 10^-3 or 10^-2 (I have been waiting even for 10thousands iterations!)

In particular, in the last case (p_outlet>45000), if I plot mach number contours I see a normal shock in the diverging section.

How is it possible if the residuals tend to zero? Is it trustworthy?
Furthermore, I tried to plot the mass flow rate and it has unusually oscillation that are not stabilising to the project flow rate.

In the text below I have reported the fluent's settings and boundary conditions (Not reported settings are set as default datas)

Solver - Density Based, Axisymmetric
Energy Equation - ok
Model inviscid
Material is ideal gas air
Operating pressure is 0

Boundary conditions

inlet - pressure inlet with
Gauge Total Pressure 101325 Pa
Initial Gauge Pressure 99348 Pa
Normal to boundary
T=300 K

The outlet section setting are those that cause me the problem (obviously pressure outlet and normal to boundary)

Solution controls

Second order upwind
courant number - 5
Flux Type Roe-FDS

Attached there are residuals, mass flow rate and mach number contours relative to a simulation with 60000 Pa as pressure outlet.

Thanks for availability!
Attached Images
 residuals.jpg (72.4 KB, 18 views) massflowrate.jpg (59.0 KB, 14 views) machnumber.jpg (53.0 KB, 26 views) mesh.jpg (47.5 KB, 21 views)

 December 17, 2016, 19:54 #2 Member   Join Date: Jun 2011 Posts: 83 Rep Power: 8 Why do you have the flow as inviscid?

 December 18, 2016, 12:51 #3 New Member   Fabio Join Date: Dec 2016 Posts: 4 Rep Power: 2 Ah you're right... I've been really foolish. Thank you so much for the advice. In the first simulation (p_outlet=3738,9 Pa) I thought it was reasonable to use the inviscid flow, but clearly it can't work with a slower flow. Anyway, the laminar model solves only some of my problems relatively the normal shock, residuals and mass flow rate. In fact, simulating flows with over 40000 Pa, as pressure outlet, everything goes fine and as result I clearly can see a shock wave at the diverging section. Although it works accurately, when I set pressure outlet between 32000 and 40000 Pa, the residuals go to infinite. I think that it’s undesirable effect of numerical errors caused by the shockwave moving close the exit section. According to you, is this reasonable? What do you think i could do to solve the last problem?

 December 20, 2016, 16:42 #4 Senior Member   Lucky Tran Join Date: Apr 2011 Location: Orlando, FL USA Posts: 1,919 Rep Power: 26 I think this is fairly typical behavior. 1) The axisymmetric solver is prone to numerical instabilities. You might have more stable results with a 3D mesh (but with some loss of accuracy because you won't be able to impose the axisymmetric condition in 3D). 2) For large driving pressure ratios the shock sits far in the diverging section of the nozzle and everything is ok. But for mild pressure ratios the shock wants to sit near the throat and the shock varies wildly iteration to iteration. Also, the shock shape is not the normal shock you get in 1D but a curved Mach disk. The mesh needs to be contoured to this shape (or fine enough resolution) to be able to resolve the shape of the Mach disk or the disk will get jumping around. The edges of the disk want to anchor at the throat but the center of the disk wants to sit at a lower position. It's pretty tough to simulation these borderline flows, you have to tinker a bit with the settings.

 April 1, 2017, 07:14 #5 New Member   Kiran Stephen Join Date: Oct 2016 Posts: 2 Rep Power: 0 You'd have to use a bigger domain involving the free stream and far field in order to get the close solution, also the mesh should be constructed such that the walls y+ values are close to 1. A turbulence model like k-omega could give you exact solutions regarding the mach number profile and a fairly accurate approximation of the shock location.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post Hrishikesh Main CFD Forum 12 June 25, 2016 02:06 SonicGhoul FLUENT 2 May 8, 2016 05:16 CFDnewbie147 OpenFOAM Native Meshers: snappyHexMesh and Others 1 October 22, 2013 09:53 ookalkan CFX 0 January 31, 2011 18:12 Franny Main CFD Forum 13 July 7, 2007 15:57

All times are GMT -4. The time now is 02:11.