CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > CFX

Manifold transient simulation

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

Reply
 
LinkBack Thread Tools Display Modes
Old   May 21, 2010, 08:43
Default Manifold transient simulation
  #1
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
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.

curves.jpg

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
Attesz is offline   Reply With Quote

Old   May 22, 2010, 06:58
Default
  #2
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   May 22, 2010, 07:11
Default
  #3
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
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
Attesz is offline   Reply With Quote

Old   May 22, 2010, 07:22
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   May 22, 2010, 07:55
Default
  #5
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
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

Last edited by Attesz; May 26, 2010 at 07:39.
Attesz is offline   Reply With Quote

Old   May 22, 2010, 08:29
Default
  #6
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
Quote:
Try double precision solver
Seems to be working, the third cycle has already started. Thanks again!
Attesz is offline   Reply With Quote

Old   May 23, 2010, 18:49
Default
  #7
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   May 24, 2010, 04:56
Default
  #8
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
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
Attesz is offline   Reply With Quote

Old   May 24, 2010, 07:03
Default
  #9
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   May 24, 2010, 08:53
Default
  #10
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
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.
Attesz is offline   Reply With Quote

Old   May 24, 2010, 18:31
Default
  #11
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Old   May 25, 2010, 07:28
Default
  #12
Senior Member
 
Attesz's Avatar
 
Attesz
Join Date: Mar 2009
Posts: 355
Rep Power: 8
Attesz is an unknown quantity at this point
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
Attesz is offline   Reply With Quote

Old   May 25, 2010, 19:03
Default
  #13
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 10,824
Rep Power: 85
ghorrocks has a spectacular aura aboutghorrocks has a spectacular aura aboutghorrocks has a spectacular aura about
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.
ghorrocks is offline   Reply With Quote

Reply

Tags
divide by zero, manifold, transient

Thread Tools
Display Modes

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 Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
intake manifold simulation uday Main CFD Forum 6 December 21, 2009 02:39
initial conditions for transient simulation littlelz CFX 2 February 5, 2009 06:56
Transient simulation and sliding mesh problems alige FLUENT 0 May 8, 2006 03:51
Transient simulation - pressure shifted Eric CFX 1 February 14, 2006 13:42
Charts for transient simulation Anurag CFX 2 March 28, 2005 12:09


All times are GMT -4. The time now is 02:53.