CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CFX (http://www.cfd-online.com/Forums/cfx/)
-   -   Manifold transient simulation (http://www.cfd-online.com/Forums/cfx/76312-manifold-transient-simulation.html)

Attesz May 21, 2010 08:43

Manifold transient simulation
 
1 Attachment(s)
Deart CFX users,

I have simulation problem with a simple manifold with butterfly valve. I get this error message:


+--------------------------------------------------------------------+
| ERROR #001100279 has occurred in subroutine ErrAction. |
| Message: |
| Floating point exception: Zero divide |
| |
| |
| |
| |
| |
+--------------------------------------------------------------------+

+--------------------------------------------------------------------+
| Writing crash recovery file |
+--------------------------------------------------------------------+

Details of error:-
----------------
Error detected by routine POPDIR
CRESLT = ILEG

Current Directory : /FLOW/NAMEMAP

+--------------------------------------------------------------------+
| An error has occurred in cfx5solve: |
| |
| The ANSYS CFX solver exited with return code 1. No results file |
| has been created. |
+--------------------------------------------------------------------+

I've modified the timestep, without result.

Attachment 3469

There was 2 tact, and exactly at the beginning of the third one, the solver failed. What can cause this error?

I can send more information if needed.

Thanks in advance,

Attila

ghorrocks May 22, 2010 06:58

What is causing the flow cycle?

If it got through 2 cycles and crashes on the third cycle I suggest it is an area of numerical instability which finally got too much on the third go. Try double precision solver or making the timestep smaller just at that point in the cycle.

Attesz May 22, 2010 07:11

Hello Glenn,

it is an internal combustion engine's manifold. The cycles comes from a 1D simulation program. I try your suggestions, thank you!

Attila

ghorrocks May 22, 2010 07:22

OK, thanks. Then the convergence problem is almost certainly associated with the coupling to the 1D model. I think I have already said my recommendation is just to model the entire manifold in CFX, then you don't have any coupling issues.

I have done a lot of IC engine modelling, my early work is summariesed in my PhD thesis (http://hdl.handle.net/2100/248) but I have developed that work extensively since then in CFX5 and considered but abandoned the idea of coupling to 1D models.

Attesz May 22, 2010 07:55

Yes, it would be the best to simulate the entire manifold, but this is a university study, and we have very limited PC capacities. So remeshing the combustion chamber etc. is out of the question. Anyway, It was a good practise in transient simulations. There is a good-looking video about it: ...

Your PHD work is very detailed, thanks for it, I hope I will have time in summer to read it. I'm going to be a PHD too...

Best Regards,
Attila

Attesz May 22, 2010 08:29

Quote:

Try double precision solver
Seems to be working, the third cycle has already started. Thanks again!

ghorrocks May 23, 2010 18:49

From your animation I can see you have no inflation layers. You will need them to get good flow resistance.

Also if you want to get a good reflection off the end of the inlet manifold you need to model the inlet filter, ducting at least to the inlet trumpet and in some cases beyond. When I was modelling racing engines I had to model the entire inlet manifold, the plenum over the inlet trumpet (it was a dyno test lab) and 5m of lab air ducting to get the inlet manifold wave right.

Based on your inlet manifold wave your engine is running VERY slowly. The inlet manifold wave has died out before the next cycle comes around.

Attesz May 24, 2010 04:56

Quote:

From your animation I can see you have no inflation layers. You will need them to get good flow resistance.
I have inflation layers. We wanted to use wall function, but because of the low flow velocities, we get low yplus. So yes, the boundary mesh is could be better, but we have not enough computational capacity to increase the mesh sizes. And of course, we have the air filter housing etc. what we can not take into account unfortunately.

My task was only to build up the simulation, so I have no information about the engine operating conditions. The maxmimum mass flow in the manifold is about 4 g/s, is it too low? These comes from a 1D simulation (GT power). The RPM is about 3000. Otherwise, I also expected bigger waves...

Regards,
Attesz

ghorrocks May 24, 2010 07:03

Quote:

I have inflation layers.
I can't see them in your animation. This means they are far too small and the transition from the prisms to the tets will be terrible. You need a much coarser prism layer so the transition to tets is closer to a 1:1 volume ratio.

Quote:

but because of the low flow velocities, we get low yplus.....but we have not enough computational capacity to increase the mesh sizes.
Because your prisms are too fine. Make them coarser. But if you use the automatic wall functions it can handle large or small y+ just fine so it is recommended. I am talking about making your mesh coarser, not finer.

Quote:

And of course, we have the air filter housing etc. what we can not take into account unfortunately.
Then forget about trying to model the inlet manifold wave. Unless you get the entire inlet manifold correctly modelled you will not get the wave correct.

What are you trying to achieve with the simulation anyway?

4g/s=0.004kg/s=0.003m^3/s=3l/s. At 3000rpm that means you engine capacity is 60cc, assuming it is a 2 stroke running at 100% volumetric efficiency (or 120cc for a 4 stroke). But you mention this is a max flow so the average will be less than this. Looks like you are modelling a very small engine. Small engines don't generally run this slowly. Are you sure it will be running this slowly? The only engines I know of like this are mileage marathon engines to get maximum fuel efficiency.

Attesz May 24, 2010 08:53

We are trying to get the pressure loss of the butterfly valve. We made steady state simulations with constant mass flow rates, but in low mass flows there was high differencies between CFD and measures (measures was already made with constant mass flows). I want to investigate the transient phenomenon of the flow with transient simulation, but there are not any measures to validate it.

Anyway, the engine capacity is 400ccm, it is 4 stroke with 70% volumetric efficiency. So at max 3000 RPM the max mass flow is 8.5 g/s, with full opened butterfly valve. The engine runs on part load operation, so comes lower mass flows. The values are not calculated by me, so I'm not sure yet they are correct. The RPM should be lower.

ghorrocks May 24, 2010 18:31

I see. The butterfly valve will dramatically affect the inlet manifold wave, and this is not only a flow resistance thing, it is a pressure wave reflection thing. That means obtaining a "pressure loss" is not really meaningful as it is only part of its effects.

Attesz May 25, 2010 07:28

I have checked the RPM-s and I thought it right, it is lower so the sucked total mass is higher. So this work was a good practice only.
Next time I will be smarter :)

Thanks for your suggestions, Glenn!

Attila

ghorrocks May 25, 2010 19:03

Do the conversion from cc/RPM to kg/s in CEL. You can enter all the variables in their native units and that helps to reduce conversion errors.


All times are GMT -4. The time now is 12:17.