Do I need a wider box?

tyw7 · February 22, 2019, 18:25

Attached is the pressure plot of the farthest wall. Do I need a bigger box?

I am calculating the lift on a wing and not quite sure if a bigger box is needed. I am already 3x the wingspan

ghorrocks · February 23, 2019, 03:27

While a bigger box will help (it always helps), I suspect correcting your boundary conditions is the more fundamental problem. Are your top and bottom faces walls or symmetry? You should either make it a translational periodic pair or make it part of the inlet.

tyw7 · February 23, 2019, 06:02

All 4 faces are set as symmetric. Is that wrong?

Picture shows the furthest most side wall.

ghorrocks · February 23, 2019, 17:28

What 4 faces are symmetric? What are the other faces? The picture shows the side wall furthest from what?

Please explain what you are doing.

tyw7 · February 23, 2019, 17:32

See attachment. The unshaded are all symmetric.

It's a half wing attached to the wall right most wall.

ghorrocks · February 24, 2019, 04:38

Your diagram is not very clear but hopefully I can guess what you mean.

I think my post #2 is talking about the correct issue, refer to that.

tyw7 · February 24, 2019, 06:27

I'm not quite sure what you meant as part of the inlet? Should the top and bottom, let's call this the roof and floor, to be inlets?

ghorrocks · February 24, 2019, 17:28

Assuming your inlet is defined as a velocity with a magnitude and direction defined, and your outlet is an outlet or opening with 0 relative pressure, and domain is a box and your flow is from left to right:

Then a good way to define this is to have the right face as your outlet and all other faces (left, top, bottom, front, back) set as inlet.

This allows you to change the angle of attack in the inlet and not see the effects you show in your first post.

tyw7 · February 24, 2019, 17:29

So no walls?

ghorrocks · February 24, 2019, 23:24

That's right. The 6 sided box has 5 sides as inlets and 1 side an outlet.

tyw7 · February 25, 2019, 03:17

What's the advantage of this vs the traditional 4 wall approach?

ghorrocks · February 25, 2019, 04:46

I don't think you could call the "4 wall approach" traditional as it is not recommended in most cases

You can't model varying angles of attack with a single mesh in the approach you are using, but my suggestion allows it. That sounds like a pretty clear advantage to me.

urosgrivc · February 25, 2019, 04:49

What makes you think that a 4 wall approach is more traditional.

Usually, a physical test in the wind tunnel has 4 walls, as it is not possible to make a physical tunnel without any walls.

And this is bad actually, imagine an aeroplane flying through the air, are there really 4 walls there ??

This is, or can be, an advantage of CFD ower physical wind tunnels actually as in a lot of cases we do not want the influence of the walls on our results.

It depends of course if this is appropriate for your case or not:
If you are doing a direct comparison of CFD versus wind tunnel tests, then I would include the walls, to make the simulation as close to real measurements as possible.

But if you want true data of let us say drag coefficient of a plane flying in the air than you have the ability in numerical simulation to actually do it better and not have the influence of the walls.

tyw7 · February 25, 2019, 04:49

How would varying angle of attack work? And got any tutorial for the 4 inlet approach?

urosgrivc · February 25, 2019, 05:00

It is simple

At the inlet, you can select in which direction the flow is going
If the flow is only in let us say X direction than the angle of attack is 0°
but if you have velocity in X and Y direction than this inlet velocity angle is the new angle of attack vhich is not 0° anymore.
And you have to account for this change for the force of drag and lift evaluation, of course,
it is best to make expressions with sin or cos functions to do all the work for you,
So you only bother with degrees of rotation.

And your domain shape can be optimised for this (because of the sharp angles and interfering inlets), This is why you are able to see CFD simulation of wings in Elliptical domains also

tyw7 · February 25, 2019, 05:02

Ah gotcha. And I'm assuming they're coupled together ie all considered 1 inlet?

Like in the boundary conditions, you model the 4 sides as a single inlet rather than separate inlets?

urosgrivc · February 25, 2019, 05:33

Yes these can be considered as one inlet

There is an even simpler method for Angle control though
I actually like this one better, far less work and no cos, sin functions..
Here it is:

You can Transform the mesh in the CFXpre,
If you add rotation, this can rotate the mesh of the whole domain by some degree
So you can have a fixed inlet velocity vX and forces and all will be according to the initial coordinate system

tyw7 · February 25, 2019, 10:37

PS do you have any reference regarding the 5 walls?

This is for a university project and every decision should be backed up.

ghorrocks · February 25, 2019, 18:31

Have a look in the literature. Most far field simulations are done this way. The "C-grid" approach is a common one which is similar but uses a structured mesh.

tyw7 · February 25, 2019, 18:32

What's the name of the approach? I had a Google and couldn't find anything relevant.

PS I tried that method and got some weird pressure stripings.

February 23, 2019, 17:28		#4
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	What 4 faces are symmetric? What are the other faces? The picture shows the side wall furthest from what? Please explain what you are doing. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 24, 2019, 04:38		#6
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Your diagram is not very clear but hopefully I can guess what you mean. I think my post #2 is talking about the correct issue, refer to that. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 24, 2019, 17:28		#8
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Assuming your inlet is defined as a velocity with a magnitude and direction defined, and your outlet is an outlet or opening with 0 relative pressure, and domain is a box and your flow is from left to right: Then a good way to define this is to have the right face as your outlet and all other faces (left, top, bottom, front, back) set as inlet. This allows you to change the angle of attack in the inlet and not see the effects you show in your first post. aero_head likes this. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 24, 2019, 23:24		#10
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	That's right. The 6 sided box has 5 sides as inlets and 1 side an outlet. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 25, 2019, 04:46		#12
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	I don't think you could call the "4 wall approach" traditional as it is not recommended in most cases You can't model varying angles of attack with a single mesh in the approach you are using, but my suggestion allows it. That sounds like a pretty clear advantage to me. aero_head likes this. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 23, 2019, 03:27		#2
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	While a bigger box will help (it always helps), I suspect correcting your boundary conditions is the more fundamental problem. Are your top and bottom faces walls or symmetry? You should either make it a translational periodic pair or make it part of the inlet. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

February 23, 2019, 06:02		#3
tyw7 Member Thu Win Join Date: Apr 2017 Posts: 70 Rep Power: 9	All 4 faces are set as symmetric. Is that wrong? Picture shows the furthest most side wall.

February 24, 2019, 06:27		#7
tyw7 Member Thu Win Join Date: Apr 2017 Posts: 70 Rep Power: 9	I'm not quite sure what you meant as part of the inlet? Should the top and bottom, let's call this the roof and floor, to be inlets?

February 24, 2019, 17:29		#9
tyw7 Member Thu Win Join Date: Apr 2017 Posts: 70 Rep Power: 9	So no walls?

February 25, 2019, 03:17		#11
tyw7 Member Thu Win Join Date: Apr 2017 Posts: 70 Rep Power: 9	What's the advantage of this vs the traditional 4 wall approach?

February 25, 2019, 04:49		#13
urosgrivc Senior Member urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 365 Rep Power: 11	What makes you think that a 4 wall approach is more traditional. Usually, a physical test in the wind tunnel has 4 walls, as it is not possible to make a physical tunnel without any walls. And this is bad actually, imagine an aeroplane flying through the air, are there really 4 walls there ?? This is, or can be, an advantage of CFD ower physical wind tunnels actually as in a lot of cases we do not want the influence of the walls on our results. It depends of course if this is appropriate for your case or not: If you are doing a direct comparison of CFD versus wind tunnel tests, then I would include the walls, to make the simulation as close to real measurements as possible. But if you want true data of let us say drag coefficient of a plane flying in the air than you have the ability in numerical simulation to actually do it better and not have the influence of the walls. aero_head likes this.

February 25, 2019, 05:00		#15
urosgrivc Senior Member urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 365 Rep Power: 11	It is simple At the inlet, you can select in which direction the flow is going If the flow is only in let us say X direction than the angle of attack is 0° but if you have velocity in X and Y direction than this inlet velocity angle is the new angle of attack vhich is not 0° anymore. And you have to account for this change for the force of drag and lift evaluation, of course, it is best to make expressions with sin or cos functions to do all the work for you, So you only bother with degrees of rotation. And your domain shape can be optimised for this (because of the sharp angles and interfering inlets), This is why you are able to see CFD simulation of wings in Elliptical domains also

February 25, 2019, 05:02		#16
tyw7 Member Thu Win Join Date: Apr 2017 Posts: 70 Rep Power: 9	Ah gotcha. And I'm assuming they're coupled together ie all considered 1 inlet? Like in the boundary conditions, you model the 4 sides as a single inlet rather than separate inlets?

February 25, 2019, 05:33		#17
urosgrivc Senior Member urosgrivc Join Date: Dec 2015 Location: Slovenija Posts: 365 Rep Power: 11	Yes these can be considered as one inlet There is an even simpler method for Angle control though I actually like this one better, far less work and no cos, sin functions.. Here it is: You can Transform the mesh in the CFXpre, If you add rotation, this can rotate the mesh of the whole domain by some degree So you can have a fixed inlet velocity vX and forces and all will be according to the initial coordinate system

February 25, 2019, 10:37		#18
tyw7 Member Thu Win Join Date: Apr 2017 Posts: 70 Rep Power: 9	PS do you have any reference regarding the 5 walls? This is for a university project and every decision should be backed up.

February 25, 2019, 18:31		#19
ghorrocks Super Moderator Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 17,703 Rep Power: 143	Have a look in the literature. Most far field simulations are done this way. The "C-grid" approach is a common one which is similar but uses a structured mesh. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Getting started with CyclicAMI	Algebraist	OpenFOAM	4	February 11, 2019 01:39
Initial values and boundary condition for LES simulation of a box	SaddamH	OpenFOAM Running, Solving & CFD	1	July 31, 2018 02:21
I get different results when I scale the 'falling box' tutorial	Hossein1	FLUENT	7	August 19, 2017 02:52
[DesignModeler] simply model, empty box	conquer	ANSYS Meshing & Geometry	0	March 28, 2014 18:26
Immersol Simulation of a Heated Box	Dong	Phoenics	0	March 2, 2006 21:20