CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   CD-adapco (http://www.cfd-online.com/Forums/cd-adapco/)
-   -   CCM+ Solution 11% higher than measured intake port flow - what are we doing wrong? (http://www.cfd-online.com/Forums/cd-adapco/69147-ccm-solution-11-higher-than-measured-intake-port-flow-what-we-doing-wrong.html)

DBurns October 13, 2009 11:58

CCM+ Solution 11% higher than measured intake port flow - what are we doing wrong?
 
The model is a 4-valve motorcycle intake port for FSAE competition. The port is symmetrical and is modeled using only half the geometry with the valve at peak lift. -6975 Pa on Pressure Outlet boundary and 0 Pa on Stagnation Inlet boundary.

The mesh:
~770,000 cell polyhedral mesh. In the valve clearance area the cell size is .25mm. All surfaces adjacent to the valve and valve seat are marked in order for mesh to capture discreet angles. Largest cell in mesh is 6mm. Using 2-layer prism layer with absolute height value of .5mm and default growth rate.

The models:
Segregated k-e turbulence model with default values for everything except turbulence specification in Initial Values which is k-e.

The solution:
Started with First Order for Segregated Pressure, Temp and Wall Treatment for 1000 iterations then switched to Second Order for another 1000 iterations. Residuals dropped nicely, Mass Flow monitor on Pressure Outlet boundary stabilized very quickly (albeit high). After about 600 iterations the Continuity residual flat-lined while all other residuals continued to drop. The highest residual after 600 iterations was 5.0E-04. Stagnation Inlet velocity is 0.4 m/s.

The Mass Flow rate is 11% higher than measured data using the same test conditions. This seems to be a classic case of creating an impressive, colorful CFD presentation that is incorrect! To our inexperienced eyes it seems like everything is right. What should we do to diagnose the disparity between measured and predicted results?

kyle October 13, 2009 18:43

11% difference between experiment and simulation is not a huge difference. A few things you can try...

- Check the y+ values around the valve. If they are very high you could be over-predicting the friction there. If they are over 300 then reduce the prism layer thickness or add additional layers to the valve boundaries.

- Vary the turbulence intensity and length scale at the inlet. If you are just using default values here then you are way too low. Try a few different values to see how dependent your solution is on the inlet turbulence values.

- If your simulation is running smoothly, then ignore the residuals. They are only helpful for unstable simulations. You should create a monitor and plot for the mass flow through the port, and watch this plot to determine convergence.

- Mesh density studies are very easy in Star-CCM+. To check the dependency of your solution on cell size, change the base size of your mesh by +-20% or so and see if you get the same solution.

Pauli October 13, 2009 20:53

Are you modeling the flow bench? In other words, does you CFD model have all the geometry of the flow bench at least up to the points where pressure is measured? If not, why do you expect an accurate correlation?

How does your correlation change as you sweep flow rate or valve lift? Answers here can provide useful clues.

In my experience, Kyle's comments are spot on. What is y-plus? What is turbulent to laminar viscosity ratio at the inlet BC?

DBurns October 14, 2009 00:12

First off, Thanks Guys for your helpful advice. I really appreciate it.

With all parts displayed the highest Y+ value is ~57. After scouring these boards I realize how important the Y+ metric is. How/where can I learn more about how to interpret Y+ values? Can you recommend a book or website (or more advice :))?

The Turbulence Specification was K + Epsilon and I used an excel spreadsheet to calculate the initial values. Since my original post, I've switched that to the default setting of Intensity and Viscosity Ratio (default values).
Quote:

If you are just using default values here then you are way too low.
I'll try varying them to see the changes they make. Thanks

Quote:

You should create a monitor and plot for the mass flow through the port, and watch this plot to determine convergence.
We set up a plane that intersects the valve seat. Should we set up a monitor and plot using that plane? We have done some grid independence work by varying the base value. Actually, that is the first thing we tried when we observed the disparity between measured and predicted.

Quote:

Are you modeling the flow bench? In other words, does you CFD model have all the geometry of the flow bench at least up to the points where pressure is measured?
The model is as close to the flow bench as we can get with the exception of a settling tank. We just extended the cylinder 5 diameters to prevent recirculating flow at the outlet boundary. We did this to cut down on mesh size and solution time. The inlet uses a hemispherical boundary whose radius is 5 times the largest dimension in the port opening. The transition from hemisphere to port is a radius entry that matches the plate used to test the head.

Quote:

How does your correlation change as you sweep flow rate or valve lift?
We haven't done any other valve lifts. We thought that the largest valve gap would probably be the most accurate. After we get this lift point straightened out we will vary lift and see how it compares. Is this good practice?

Thanks again!

kyle October 14, 2009 10:04

Quote:

Originally Posted by DBurns (Post 232511)
The Turbulence Specification was K + Epsilon and I used an excel spreadsheet to calculate the initial values.

I think you might be misunderstanding something here, or just your terminology might be wrong. The initial turbulence values have no bearing on your solution... this is just the initial guess that the solver starts with. What is important is the turbulence values at the inlet boundary. I am not sure if by initial you mean the values at the inlet boundary.

11% may be the best you will see. Your expectations for CFD may be too high. It would not be uncommon to calibrate a simulation like yours by fudging the inlet pressure to get the expected flow rate. In my opinion, CFD is most useful for predicting how well one design will preform in relation to another. Precise predictions for a single design are unlikely.

DBurns October 14, 2009 11:29

I understood you correctly but maybe I did a poor job of explaining myself. I used the spreadsheet to calculate initial values in the physics continuum to avoid seeing pressure/temp/viscosity warnings at the beginning of the simulation. I used the same values for the inlet boundary conditions.

Absolute accuracy is not the main goal. The goal is to learn from this experience. I've gotten more from your advice than I have spending hours pouring over the User's Guide. Don't get me wrong - the User's Guide is essential but it is also very valuable to get get advice on a particular application. The tutorials were very helpful.

Do you have any advice for interpreting Y+ values? What should they be?

kyle October 14, 2009 12:11

There is not a whole lot to interpret with y+. If the values are between 30 and 300, then you are done with y+ and you can move on. If you want to push it then you can go between 11 and 1000. The reason that this matters is pretty complicated, but it would be covered in any decent textbook on CFD, turbulence or viscosity.

DBurns October 14, 2009 16:30

As far as I've tested, the mass flow rate does not seem to be affected much by varying Turbulence Intensity and Viscosity Ratio values. I changed them by orders of magnitude and they end up with virtually the same result. I read in the User's Guide where they do not recommend using the TI/TVR or TI/Length Scale specification if the inlet Boundary initializes at 0 Velocity. The Velocity on my inlet boundary is 0.4. I switched the Turbulence Specification back to K + Epsilon and I'm moving on.

Thanks for all the help.

Maddin October 20, 2009 05:07

I wouldn't use the k-e modell, use k-omega SST.
Y+ value I would bring under 1... calulator you find in the cfd-online links -> there you only calulate the thickness of the first layer, with the stetch factor you can calulate you prism layer thickness.
The pressure is a little bit high, most flow bench work with 5000Pa.
How do you set your gas properties?

On the Length Scale etc. I never had to change something. Use a extrusion on inlet and outlet to solve the problem with the velocity profile. In the interface you could check the pressure drop in the extrusions.

DBurns October 20, 2009 13:38

Thank you, Maddin, for your valuable insight. I am exploring the options you've outlined. Can you explain your recommendations a little more in detail? I'm just beginning my journey in fluids!

I used Ideal gas. 6975 Pa is equal to 28 inches of water which is what the engine shop tested our head at.

Thanks again!

Maddin October 20, 2009 13:57

Sorry, it's not my day. Sure 10",20" or 28"WC are standard on a flow bench. I think it's only a question of the size of the channels which you use... or?
The modell question is a little bit difficult. Some guys use k-e, I prefer k-w SST because I have k-e and k-w wilcox together, as far as I know. I also do this very long ;)
Ideal gas, ok. But I would modify the gas properties to sutherland and thermodynamic polynom.
The pressure I would ramp via a field function for 50-100steps and I would do it in 2nd order from beginning. -> the residual maybe makes problems because of the normalization, take them off for a real look on them.
With extrusions a mesh size of 2 mio. cells isn't too fine.
When you want I can take a look on you sim-file.

DBurns October 20, 2009 15:03

That would be great if you could look it over and critique our model. How shall I get the file to you? Do you have an ftp? I'll have to pass it by the team but I don't expect any problems.

Maddin October 20, 2009 15:22

Via ICQ as compressed file. Maybe without volume mesh.
I have 4.04.011...
You have pm.

/edit: One point... the stagnation inlet is better for high mach numbers maybe you should use also a pressure outlet as a inlet. The error "reversing flow" is no problem.

AndyR November 27, 2009 12:58

Missing Delta P
 
Ultimately if you are overprediciting flow , you are under predicting Delta P. So think about where you might not be capturing pressure drop fully

One error source is time accuracy. The flow behind the valve is unlikely to truly be steady and symmetric. While the bulk of the pressure drop is surely the upstream port and valve, the test measures all the delta p, including that in the cylinder volume. That loss could certainly be on the order of 5%, 10% might be high, but not impossible.

Look at some contour and vector plots at your entrance region. Does the BL growth seem plausable?? Is it possible you are getting a slightly lower entrance loss?

Look for seperation or recirculation zones that seem poorly resolved. This could also result in missing DP. I would think with some care you should be able to get to within a 5% value, which would be predictable from a trending standpoint.

Good Luck
- Andy R

Maddin December 4, 2009 04:59

I had looked into his sim-file. He had used only 2 layers. After some modz the sim works quite good when I understand him right.

DBurns December 6, 2009 15:52

Yes, Maddin got us very close to measured data. (176.93 g/s measured vs. 176.43 predicted)
  • He had us switch from k-e to k-w SST, used 5 boundary layers instead of 2
  • Start out 2nd Order using a pressure ramp for the first 500 iterations and a relaxation ramp on the first 10
  • Changed the viscosity to Sutherland's Law
  • Added extrusions that were 10 layers thick on the inlet and outlet boundaries
With his help we were able to make some simple modifications to the valve and valve seat and realize those flow improvements on the flowbench. THANK YOU MADDIN!

Maddin December 7, 2009 05:10

No problem. Without extrusions I think it would also work but I alwasy use them *g*


All times are GMT -4. The time now is 13:34.