[nickjuana]

Using PV^gamma= constant, I got pressure value. For 15 compression ratio I got pressure value 45 bar. I know initial pressure(P1), initial volume(V1), final volume(V2) and from above equation I got final pressure. Inside the cylinder, pressure would be around 45 bar before Ignition.

[ghorrocks]

In that case you are comparing against analytical values.

I have done this sort of modelling before with CFX and got within 1% of the analytical values so if you set it up correctly it can be done very accurately.

I recommend you draw a simple box with a hex mesh and a laminar flow model. Then you will be a good analog to the analytical equation and when you get this workign well you should be within 1%. You do not need a fine mesh, a 10x10x10 mesh will be fine so the simulations will run in seconds. But you will need to adjust convergence and time step parameters until you get sufficient accuracy.

[nickjuana]

Then how will I get other results If I use laminar model. My main aim is to compare squish, TKE, Turbulence. If I do what you said I will get required pressure but there are also other factors I need.
Does CFX simulates real compression and not idealised isentropic compression ?
You want me to change properties of Air Ideal gas..?

[ghorrocks]

You missed my point. I recommend you do a simple benchmark case where you can run it quickly and when it is working properly you should get very accurate answers to the analytical solution. When you know how to get this simple benchmark case accurate then you use the same method on your real case and the compression modelling should be accurate.

Does CFX simulates real compression and not idealised isentropic compression ?

CFX models whatever you set it up to model. You can use real gas models, ideal gas, gas mixtures or anything you want.

You want me to change properties of Air Ideal gas..?

You use the gas model appropriate for the gas you are modelling.

[nickjuana]

what I meant is does pressure rise is more because of the property of the gas..?

[nickjuana]

Now I am doing simulation with flat piston with only 37 thousand elements. Now you want me to change turbulence model to laminar and see what happens, correct..?

[ghorrocks]

what I meant is does pressure rise is more because of the property of the gas..?

Different gases will have different pressure rises. Look up isentropic exponent, or this: http://en.wikipedia.org/wiki/Polytropic_process

Now you want me to change turbulence model to laminar and see what happens, correct..?

If you are having accuracy problems the first thing you do is check you can get a basic model right.

Just checking - you took the reference pressure into account when you did this, did you?

[nickjuana]

Yes initial pressure is 1 bar I took

[ghorrocks]

The initial pressure is 1 bar gauge, with a 1 atm reference. So your initial pressure is 201.3 kPa. Is that what you mean? Because that is what your CCL says you modelled.

[nickjuana]

No.... During suction air will be at 1 bar pressure. 1 bar pressure is compressed. I think I have made mistake in that .
Can you please say how you got 201.3 KPa ?

[nickjuana]

I gave reference pressure as 0 atm. Now I am getting 36.5 bar but required is around 44 bar. What should I do now..?

[ghorrocks]

You don't want to use 0 reference pressure. If it starts at 1 atm pressure then use 1 atm as the reference pressure with 0 Pa initial pressure.

What equation did you use to calculate the expected pressure? What polytropic coefficient did you use?

[nickjuana]

PV^gamma=constant
gamma=1.4

[ghorrocks]

OK.

My recommendation is already stated: draw a simple rectangular box and compress that. Determine what convergence criteria, time step size and everything else you need to get this accurate and then use these settings on your more complex model.

[nickjuana]

How to get turbulent intensity in CFX post..?

[ghorrocks]

That's the turbulent kinetic energy variable.

[nickjuana]

I used tetra mesh to run a case, after 100 iterations the solver stopped saying that
+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Overflow |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Stopped in routine FPX: C_FPX_HANDLER |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+
I have checked boundary conditions with already corrected case and it is also converging
Cant find where the problem is..?

[ghorrocks]

This is an FAQ: http://www.cfd-online.com/Wiki/Ansys...do_about_it.3F

But in this case I would suspect the mesh quality got bad enough to cause problems. Have a look at the way your mesh squashes up as it moves.

[nickjuana]

Total iterations is 400 and solver has ran more than 100 iterations then also there is a problem with the mesh..?
Tetra mesh quality it was minimum 0.3

[ghorrocks]

This is a moving mesh simulation - so the mesh changes as the simulation proceeds.

Tet meshes do not squash very well with mesh motion. Hex meshes do this much better as long as the mesh is stacked in the direction of motion.

Please post as image of a cross section of your mesh shortly before it crashes.