Help with a Filter Cleaning Simulation

[samuel.arismendi]

First of all hi!

I am part of an students group at the Hochschule Bremen in Germany and we are using the Studnet Version of Autodesk Simulation CFD. The project we were tasked with implies cleaning cylindrical filters using a strong blow in the opposite direction of the normal air-flow. We haven´t been able to work out a Transient simulation (I believe that´s because of the intensive calculations and our computers are not up to it) so we decided to work with Steady State simulations. I´m adding on to this Post images the basic geometry. I´ll also try to write down all important info as well.

As seen on the images, the montage is a duct of 900 mm of diameter, the filter (which was broke into 4 pieces in order to examine it more meticulously) and a little tube from which the air blow comes every time that we detect a high pressure drop between both ends of the duct (which means that the filter is getting too dirty). During its normal operation, the air flows from the wide end (atmospheric pressure) to the narrow end (vacuum between 0 and -600 Pa) at a known rate (1783 m3/h). In order to establish the material of the filter we ran a lot of simulations using the following boundary conditions:

Wide end: Pressure (gage) 0 Pa
Narrow end: Volumen Flow Rate 1783 m3/h
Tube: closed (no conditions)

The idea was to play with the properties of the material until obtaining around -600 Pa of pressure drop. This was not possible so we got stuck with the values that worked best (shown on one of the images)

We are comparing 4 different pieces intended to deliver the air-blow to the filters wall so that it cleans the filter uniformly. Simulations that include these pieces are going to be compared with one another to determine which distributes the air best. Boundary conditions for said simulations were set as follows:

Wide end: Pressure (gage) 0 Pa
Narrow end: Pressure (gage) -600 Pa
Tube: Mass Flow Rate 520 g/s (going in) ; Pressure (gage) 1 bar

The problem comes here. After doing lots of simulations we have encountered divergence many times and also significant inconsistencies on the Summary in regard of the mass balance. Although we understand that a retain error tolerance is needed, we are talking about 60% of error. That is just too much to ignore.

We are using ADV2 and ADV5, Compressible Flow and a Turb./Laminar Ratio = 10000.

We would like to know if is there anything else that we could be doing in order to improve the quality of the simulations (other than making a finer mesh, we are already testing that). Also we are already working with just a quarter of the whole thing using the Slip/Symmetry Boundary Condition. Could we be making some kind of conceptual mistake?

Thanks for your help.

*** Simulation CFD Summary File Output ***

Simulation CFD 2014 (Cardinal Release) [20130301]

Job Name = Scenario 1 Date created: Thu Feb 13 09:06:04 2014

*** Analysis Information
Steady State is ON
Compressible Flow is ON

*** Field Variable Results Summary For Iteration 1000

Var Mean at Max at Min
Vx Vel +1.94909e+003 8950 +1.81270e+005 9324 -9.89405e+004 mm/s
Vy Vel +8.24601e+003 8982 +3.03199e+005 1563 -4.88992e+004 mm/s
Vz Vel -1.85880e+003 22874 +8.93656e+004 9405 -1.77118e+005 mm/s
Press +9.28559e+003 1624 +1.66837e+005 9358 -1.02933e+004 N/m^2
Temp +2.35700e+001 102 +2.68500e+001 8982 -3.20099e+001 C
TurbK +1.59563e+008 1997 +5.76382e+009 101 +1.81700e-008 mm^2/s^2
TurbD +1.23648e+012 23755 +7.83405e+013 33 +1.11792e-012 mm^2/s^3
Scal1 +0.00000e+000 102 +0.00000e+000 1656 +0.00000e+000
PTotl +9.95075e+003 9421 +1.68852e+005 9358 -1.02933e+004 N/m^2
EVisc +1.20796e-002 1797 +6.78070e-001 6928 +0.00000e+000 g/mm-s
ECond +1.22390e-002 1797 +6.81025e-001 6928 +0.00000e+000 W/mm-K
Dens +6.84392e-004 6928 +7.83300e-003 9358 +1.05729e-006 g/mm^3
Visc +1.65852e-005 102 +1.81700e-005 6928 +0.00000e+000 g/mm-s
Cond +4.87355e-003 6928 +5.44000e-002 1656 +2.56300e-005 W/mm-K
SpecH +9.56987e-001 102 +1.00400e+000 6928 +4.65000e-001 J/g-K
Emiss +9.12777e-001 102 +1.00000e+000 6928 +0.00000e+000
Transmiss +0.00000e+000 0 +0.00000e+000 0 +0.00000e+000
WRough +0.00000e+000 102 +0.00000e+000 1656 +0.00000e+000 mm
SeeBeck +0.00000e+000 0 +0.00000e+000 0 +0.00000e+000 V/K
GenT +4.68369e+003 23724 +6.02388e+005 6928 +3.16228e-002 1/s

*** Openings ***

*** Inlet 1 ***

Surface ID = 1

Node near Minimum X,Y,Z of opening = 3

Minimum X,Y,Z of opening = 4.679623, -452.000000, -15.401036

Mass Flow In = 129 g/s
Volume Flow In = 5.40241e+007 mm^3/s
Reynolds Number = 321493
Inlet Bulk Pressure = 100000 N/m^2
Inlet Bulk Temperature = 20.5735 C
Inlet Mach Number = 0.306949

Total Mass Flow In = 129 g/s

Total Vol. Flow In = 5.40241e+007 mm^3/s

*** Outlet 1 ***

Surface ID = 29

Node near Minimum X,Y,Z of opening = 5855

Minimum X,Y,Z of opening = 149.331165, 810.000000, -340.182132

Mass Flow Out = 19.0295 g/s
Volume Flow Out = 1.6173e+007 mm^3/s
Reynolds Number = 2973.52
Outlet Bulk Pressure = 0 N/m^2
Outlet Bulk Temperature = 26.85 C
Outlet Mach Number = 0.000463154

*** Outlet 2 ***

Surface ID = 10

Node near Minimum X,Y,Z of opening = 2503

Minimum X,Y,Z of opening = 127.107490, -402.000000, -119.028511

Mass Flow Out = -64.2868 g/s
Volume Flow Out = -5.49581e+007 mm^3/s
Reynolds Number = 16196.4
Outlet Bulk Pressure = -600 N/m^2
Outlet Bulk Temperature = 26.8281 C
Outlet Mach Number = 0.00800776

Total Mass Flow Out = -45.2573 g/s

Total Vol. Flow Out = -3.87851e+007 mm^3/s

*** Statistics for Velocity Magnitude ***

Value Range [mm/s] Percent Volume
0.000000 - 17195.218140 98.971278
17195.218140 - 34390.436279 0.567195
34390.436279 - 51585.654419 0.325985
51585.654419 - 68780.872559 0.111507
68780.872559 - 85976.090699 0.011176
85976.090699 - 103171.308838 0.005024
103171.308838 - 120366.526978 0.002716
120366.526978 - 137561.745118 0.001785
137561.745118 - 154756.963258 0.001146
154756.963258 - 171952.181397 0.000269
171952.181397 - 189147.399537 0.000353
189147.399537 - 206342.617677 0.000394
206342.617677 - 223537.835817 0.000121
223537.835817 - 240733.053956 0.000082
240733.053956 - 257928.272096 0.000101
257928.272096 - 275123.490236 0.000250
275123.490236 - 292318.708376 0.000174
292318.708376 - 309513.926515 0.000154
309513.926515 - 326709.144655 0.000259
326709.144655 - 343904.362795 0.000032
Mean Value = 11984.753156 , Standard Deviation = 41728.816263

*** Sum of Fluid Forces on Walls ***
ShearX, PressX = 10224 7.0283e+008 microNewtons
ShearY, PressY = 1.6792e+005 4.8293e+007 microNewtons
ShearZ, PressZ = -9378.6 -7.0282e+008 microNewtons

*** Analysis Statistics:

Input: 6 seconds
Analysis: 2710 seconds
Output: 1 seconds
Total: 2717 seconds

Master process dynamic memory 71 Mbytes
Slave process 0 dynamic memory 47 Mbytes
Slave process 1 dynamic memory 45 Mbytes

[Jon.Wilde]

Hi Samuel,

I have a few comments to make, firstly have you looked up compressible analyses within our help?

We should run with Mass flow or Total pressure at the inlet, along with a Total Temperature ideally.

Typically we would assign an unknown to an outlet when we have a compressible model, although I confess I am unclear exactly where your air is entering and leaving.

What were your flow rates before running compressible?

It looks as though you may be able to run a 2D ayisymmetric model here? These are usually faster and because of the high levels of mesh we can use, more accurate.

Kind regards,

Jon

[samuel.arismendi]

Hi Jon!


Yes, we have been reading the help sites but we could have missed something useful so we will check it again. About the simulation, we haven?t run any simulations with the incompressible flow option. The air comes from the small tube in the front. In reality the mass flow rate is about 520 g/s but since we are simulating just 1/4 of the model, it is set at 129 g/s. The sucction at the narrow end doesn?t stop during the cleaning process (which only takes about 0,2 seconds) but to avoid any extra turbulence, we decided to just let it open with a known pressure (-600 Pa). So far "unknown" hasn?t been helpful. Usually we find divergence faster using an "unknown" openning. Also we have been trying to create the 2d model but have been unable to determine how to build the model in Inventor.


Thanks for your time!


Samuel

[OmkarJ]

Few comments:

1) Your BCs are not exactly clear, where are inlet, outlet1 and outlet2? Where exactly is the filter?

2) How have you determined the resistance coefficient for the filter (1000)? If the flow takes place only radially through the filter, have you considered using a surface resistance? Things will be lot more easier and lighter then.

3) Even if your physics is such that compressible flow is justified, I would first run the simulation with incompressible flow first. Step up the physics one by one, instead of throwing all in at once. You may want to use a coarser mesh for this experimentation. Once you see that everything works and you get a convergence, you can move to the finer mesh to have accurate results.

4) I agree with Jon, 2D simulaton makes sense here if geometry is radially symmetric. You need to create a sketch of the geometry  on XY plane in Inventor, patch it to create surface and export it to SimCFD.

[samuel.arismendi]

Hi and thank you for your comments!

So, allow me to reply on the same order:

1) I?m adding some pics to help clarify the case.

2) We took the same assembly and ran it under the first round of BC described on the oppening post. We did that several times varying the coefficients as we went along. Under those conditions, air should flow from the wide side (the one in the right, named "outlet 1" on the pictures) to the narrow side (the one in the left, named "outlet 2" in the pictures). Maybe we should clarify that in this case, said openings are not named "outlets" on the summary since it is a totally different situation. The goal was to obtain a pressure drop of around -600 Pa between the atmosphere and the side under vacuum. On the real facilities, the system measures the pressure drop through the filter until reaching -600 Pa, when the cleanning operation takes place. About that is worth mention that we failed to obtain those -600 Pa. We were able to obtain about -500 Pa where every time we raised the coefficient again, the software would throw divergence at us.

3) I guess you are correct. That is a practice we haven?t picked up just yet. We will try.

4) Yes. As said, we knew that a 2D model was possible, however we couldnt find in the help page how to take a CAD sketch and jump to the SimCFD. We will try it out. ??
[cid:b839ea95-eb0b-4126-9825-db4098ee6a41][cid:a739e08c-2810-4ade-a713-7db2d9b95e53][cid:9e26b148-bcd9-4f8f-838c-c2ac012a8636][cid:2fa66eb6-bd89-40a9-90d2-302d124a1b25]

[samuel.arismendi]

Here are the images!

[samuel.arismendi]

and a last pic

[OmkarJ]

I know that new users get befuddled on the 2D case since there isn't much abut it in the documentation. I have created a simple tutorial quickly to help understand the import of the CAD. You can refer to this tutorial as well: http://help.autodesk.com/view/SCDSE/2014/ENU/?guid=GUID-17530C86-1491-4C26-B509-81E55786DC12

Give it a shot with surface resistance instead of volume resistance in 3D (or edge resistance instead of surface reisstance in axisymmetric). IT is more simplistic but probably a bit easier for convergence.

[samuel.arismendi]

I would like to thank everybody who has replied to this post! The simulation in 2D is working now although the results are quite dificult interpret or explain. I´ll add a picture. The filter is broken in 4 parts. We made it so we could read the average preassure over the superficial area on each part and evaluate how well distributed was this preassure drop. We found that in the case of the picture, it was quite well distributed, however the mass-flow going across each secction was different (significantly so). We got the readings on the mass-flow using the bulk calculator on "Planes" along the x axis. For example, for Part 1 we check the massflow at the entrance of the filter and at the end of part one, make the subtraction and whatever mass missing is going through the filter. If you guys have heard something related, please let me know. It´s just a little counter-intuitive to think that the same material with the same pressure drop has different mass-flow-rates.

Again Thank you very much.