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

Grid Orientation on Injector Internal Flow Simulation

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 12, 2021, 03:16
Default Grid Orientation on Injector Internal Flow Simulation
  #1
New Member
 
Omer Faruk
Join Date: Nov 2019
Posts: 7
Rep Power: 3
Spacebox is on a distinguished road
Hello everyone,

Due to the Cartesian-cut cell meshing strategy in CONVERGE, grid orientation difference can be seen for each nozzle on the injector. To solve this issue, in some case, rotating computational domain will not be helpful. Therefore, In think that inlaid mesh implementation would be needed to reduce nozzle-to-nozzle variation error caused by grid orientation. In that sense, I am wondering how to implement surface inlaid mesh on the nozzle or sac region.

I checked cylinder and euclidean shape in converge studio but there is not showing any surface strategy.

Thanks for your help
Spacebox is offline   Reply With Quote

Old   April 12, 2021, 10:02
Default
  #2
Senior Member
 
ksrivast's Avatar
 
Kislaya Srivastava
Join Date: Sep 2017
Location: Convergent Science, Northville MI
Posts: 110
Rep Power: 5
ksrivast is on a distinguished road
Hello Omer,

To create a surface/boundary-layered mesh along your nozzle and sac boundaries, you have the following options :
1. Use the "Extrusion" Inlaid mesh tool in STUDIO. You would need to ensure the triangulation on the boundaries would be suitable to create a good extruded surface mesh from it. For more details on this, please refer to our Inlaid Mesh advanced training slides or our CONVERGE STUDIO manual.
2. You can directly import an ASCII Plot3D grid file in STUDIO, generated from an external mesh tool, to use as an inlaid mesh within CONVERGE. More details in our STUDIO manual.
3. If you have a mesh generated from an external tool in any other format (ex, CGNS), please get in touch with support@convergecfd.com and we might have some scripts to assist you with converting your mesh into a STUDIO readable surface file.

With respect to the grid orientation issues you're facing in your simulations, you might want to also consider further refining your default CONVERGE Cartesian mesh (either by fixed embedding or AMR) which can significantly reduce such grid effects.

Hope this helps.

Sincerely,
__________________
Kislaya Srivastava
Research Engineer | Applications
CONVERGECFD
ksrivast is offline   Reply With Quote

Old   April 13, 2021, 05:26
Default
  #3
New Member
 
Omer Faruk
Join Date: Nov 2019
Posts: 7
Rep Power: 3
Spacebox is on a distinguished road
Quote:
Originally Posted by ksrivast View Post
Hello Omer,

To create a surface/boundary-layered mesh along your nozzle and sac boundaries, you have the following options :
1. Use the "Extrusion" Inlaid mesh tool in STUDIO. You would need to ensure the triangulation on the boundaries would be suitable to create a good extruded surface mesh from it. For more details on this, please refer to our Inlaid Mesh advanced training slides or our CONVERGE STUDIO manual.
2. You can directly import an ASCII Plot3D grid file in STUDIO, generated from an external mesh tool, to use as an inlaid mesh within CONVERGE. More details in our STUDIO manual.
3. If you have a mesh generated from an external tool in any other format (ex, CGNS), please get in touch with support@convergecfd.com and we might have some scripts to assist you with converting your mesh into a STUDIO readable surface file.

With respect to the grid orientation issues you're facing in your simulations, you might want to also consider further refining your default CONVERGE Cartesian mesh (either by fixed embedding or AMR) which can significantly reduce such grid effects.

Hope this helps.

Sincerely,
Hello Kislaya,

Thanks for valuable response,

Regarding the refining default mesh, I have used the enough mesh size such as 10um for nozzle, 20um for sac region that has been already implemented in the previous study done in Argonne National Lab using CONVERGE. In this case, even though mass flow rate is almost identical for each hole, TKE distribution is quite different and provide different flow characteristics due to grid orientation. When I refined the mesh using 5um, the result also similarly appears. But it was supposed to be somehow identical for each nozzle.

What I experienced with extrusion section in converge studio is only for boundary layer, not creating extra surface on the nozzle with different type of mesh. If I am wrong, pls let me know how to use extrusion for new surface creation.

Therefore, it looks like among the suggested 3 options, only way is to use the other application to get surface mesh and load it to make homogeneous mesh for each hole. Is there any free meshing application which easily exports plot3d format?

Thanks for your help
Spacebox is offline   Reply With Quote

Old   April 13, 2021, 10:12
Default
  #4
Senior Member
 
ksrivast's Avatar
 
Kislaya Srivastava
Join Date: Sep 2017
Location: Convergent Science, Northville MI
Posts: 110
Rep Power: 5
ksrivast is on a distinguished road
Hello Omer,

I'm afraid I don't fully understand your question. By surface mesh, do you mean the triangulation/quadrangulation on the nozzle boundaries to extrude a good boundary layered mesh from? You are right, that the extrusion tool in STUDIO is for creating boundary layer type inlaid meshes. But there is a precursor step typically involved before you use the extrusion tool. You are required to re-create the surface triangulation on the boundaries so as to have a good "surface mesh" to extrude from. This can be done in "Geometry > Create > Triangle > Refine Triangles > Quadrangulate surface". Or you can also generate a suitable triangulated surface as an STL file from certain CAD packages.

If however, you require a volume mesh for the entire nozzle/sac volume, then it would be easier to create it externally.

Sincerely,
__________________
Kislaya Srivastava
Research Engineer | Applications
CONVERGECFD
ksrivast is offline   Reply With Quote

Old   April 14, 2021, 02:12
Default
  #5
New Member
 
Omer Faruk
Join Date: Nov 2019
Posts: 7
Rep Power: 3
Spacebox is on a distinguished road
Hello Kislaya,

Thanks for your responses. Really appreciated.

Due to the mentioned several options and parameters for inlaid mesh strategy, I confused and wanted to clear my problem one more time.

The main question is how I can evenly distribute the mesh in each nozzle to avoid hole-to-hole variation error. To make the question more understandable, I showed mesh distribution of 5-hole injector in the sac region. As you can see, the hole aligned with the x-axis has straight mesh distribution, others have inclined one. Therefore, flow characteristics were generated differently in each hole. But this is not correct. In that sense, I was told that inlaid mesh would be an option to solve this problem. In here, which method of inlaid mesh needs to be used to solve this issue? Using Extrusion after creating good surface for each nozzle through Geometry > Create > Triangle > Refine Triangles > Quadrangulate surface method would be helpful? I am not sure about that because it only affects boundary layer not a default mesh orientation. In that sense, I would like to know what I need to do precisely. Addressing the correct direction is important.

If there is no possible solution in converge studio, then I need to focus on how to import mesh externally rather than spending more energy on inlaid mesh.

Thanks for your support.

Best regards
Attached Images
File Type: jpg Grid Orientation.jpg (138.3 KB, 14 views)
Spacebox is offline   Reply With Quote

Old   April 14, 2021, 13:22
Default
  #6
Senior Member
 
ksrivast's Avatar
 
Kislaya Srivastava
Join Date: Sep 2017
Location: Convergent Science, Northville MI
Posts: 110
Rep Power: 5
ksrivast is on a distinguished road
Hello Omer,

I gather you require a volume mesh, within the entire nozzle volumes, with all cells aligned with their respective nozzle directions. Currently, there is no straight forward approach to create volume meshes which are bounded by complex surfaces through STUDIO. It would be easier to create it externally.

You can also compromise, and still go with the boundary-layer extrusion mesh approach, and have the total distance large so that the boundary aligned cells fill up most of the nozzle volume. You will still have our normal cartesian mesh in the center of the nozzle volume.

If you'd like assistance with creating inlaid meshes in STUDIO, please reach out to us at support@convergecfd.com. Please use your official email for all correspondence with Convergent Science. Please mention your request, attach your surface file/case setup and add the cfd-online thread, as reference.

Sincerely,
__________________
Kislaya Srivastava
Research Engineer | Applications
CONVERGECFD
ksrivast is offline   Reply With Quote

Old   April 26, 2021, 09:48
Default
  #7
New Member
 
Omer Faruk
Join Date: Nov 2019
Posts: 7
Rep Power: 3
Spacebox is on a distinguished road
Hello again Kislaya,

Thanks for the advice and support regarding inlaid mesh.

Applying large boundary layer distance actually work fine to reduce to hole-to-hole error and obtain identical flow structure for each hole. With this strategy, however, 3-hole nozzle and 5-hole nozzle has a similar flow characteristic.
As well known that this result is not realistic. In particular, turbulence inside the hole must be somehow different due to different sac flow structure. In other words, I can not see the hole-number effect on the flow characteristics. Is this lack of CFD for internal flow simulation or missing sth in the set up? it would be great if you help me out in this issue.

Thanks in advance
Best Regards
Spacebox is offline   Reply With Quote

Old   April 26, 2021, 10:49
Default
  #8
Senior Member
 
ksrivast's Avatar
 
Kislaya Srivastava
Join Date: Sep 2017
Location: Convergent Science, Northville MI
Posts: 110
Rep Power: 5
ksrivast is on a distinguished road
Hello Omer,

We would first recommend you to perform a grid independence study to ensure you have enough refinement to capture an accurate solution, if you haven't done this already. Your results can improve by improving your near-wall solution. Make sure the near wall treatment for your simulation is suitable for the y+ values you are seeing. If your y+ values are higher than the recommended range, refine your wall grid spacing. If your y+ values are too low, you can employ scalable or enhanced wall functions which work better with low y+ values. We also have different turbulence models you can investigate.

Hope this helps.

Sincerely,
__________________
Kislaya Srivastava
Research Engineer | Applications
CONVERGECFD
ksrivast is offline   Reply With Quote

Old   April 27, 2021, 09:38
Default
  #9
New Member
 
Omer Faruk
Join Date: Nov 2019
Posts: 7
Rep Power: 3
Spacebox is on a distinguished road
Hello Kislaya,

Thanks for prompt reply.

Actually mesh refinement has already been validated using the previous case before creating the BL on each hole. In that case, I used 10um as min mesh size without BL. This strategy was also used in many studies in literature. But after adding BL thickness on nozzle I further decreased min. mesh size down to 5um to create more smooth transition from center mesh to BL mesh. I generated the BL initial distance from 1um to 5um using 15 layer. With this conditions, results shows the similar trend of validated case in terms of velocity and mass flow rate. However, in terms of turbulence, huge difference is seen. This comparison was done using rotated 4-Hole nozzle with 10um and 4-Hole Nozzle with BL. Also, results shows that even without BL case, y+ was max. around 100, after adding BL y+ became max. around 7. For both case, y+ is within recommended range.

Turbulence is govern by the hole inlet flow structures which are generated in the sac volume. What I realized that 3-Hole and 5-Hole injector case somehow inlet flow structure is all identical in the peak needle lift. If flow enters the hole in same manner, generated TKE would be identical. This is the problem.

I hope I clearly explained the current issues.

In the mean time, I will also investigate SST model and see whether it would capture the difference in turbulence or not.

Thanks for your help in advance.

Best regards,
Omer
Spacebox is offline   Reply With Quote

Old   April 30, 2021, 13:01
Default
  #10
yli
Member
 
Yanheng Li
Join Date: Jan 2016
Location: Convergent Science, Madison WI
Posts: 33
Rep Power: 7
yli is on a distinguished road
Hi, Omer,

Please see these two slides from our inlaid mesh advanced training course, hope it can help. If you need more explanation, feel free either ask here, or register for our advanced training course, or contact support@convergecfd.com to let some one assist you.



Quote:
Originally Posted by Spacebox View Post
Hello Kislaya,

Thanks for your responses. Really appreciated.

Due to the mentioned several options and parameters for inlaid mesh strategy, I confused and wanted to clear my problem one more time.

The main question is how I can evenly distribute the mesh in each nozzle to avoid hole-to-hole variation error. To make the question more understandable, I showed mesh distribution of 5-hole injector in the sac region. As you can see, the hole aligned with the x-axis has straight mesh distribution, others have inclined one. Therefore, flow characteristics were generated differently in each hole. But this is not correct. In that sense, I was told that inlaid mesh would be an option to solve this problem. In here, which method of inlaid mesh needs to be used to solve this issue? Using Extrusion after creating good surface for each nozzle through Geometry > Create > Triangle > Refine Triangles > Quadrangulate surface method would be helpful? I am not sure about that because it only affects boundary layer not a default mesh orientation. In that sense, I would like to know what I need to do precisely. Addressing the correct direction is important.

If there is no possible solution in converge studio, then I need to focus on how to import mesh externally rather than spending more energy on inlaid mesh.

Thanks for your support.

Best regards
Attached Images
File Type: jpg Screenshot from 2021-04-30 11-59-27.jpg (136.0 KB, 4 views)
File Type: jpg Screenshot from 2021-04-30 11-59-31.jpg (122.1 KB, 6 views)
__________________
Yanheng Li
Research Engineer-Applications

CONVERGECFD
yli is offline   Reply With Quote

Old   April 30, 2021, 13:14
Default
  #11
New Member
 
Omer Faruk
Join Date: Nov 2019
Posts: 7
Rep Power: 3
Spacebox is on a distinguished road
Dear Yanheng Li,

Thanks for sharing the material. I have already had this inlaid mesh advance course file. I somehow managed inlaid mesh issue.

Now, I am expecting to receive a response related to my last post regarding turbulence in the nozzle flow. I even sent email support@convergecfd.com for this issue.
I hope you could give me some direction.

Thanks again for your kind support.
Best Regards
Omer
Spacebox is offline   Reply With Quote

Old   May 3, 2021, 11:23
Default
  #12
yli
Member
 
Yanheng Li
Join Date: Jan 2016
Location: Convergent Science, Madison WI
Posts: 33
Rep Power: 7
yli is on a distinguished road
Hi, Omer,
Are you using RANS?Which model? What is your away-from-the wall grid resolution looks like? And what is the last layer of inlaid mesh(adjacent to the Cartesian grid) 's resolution looks like?

Quote:
Originally Posted by Spacebox View Post
Dear Yanheng Li,

Thanks for sharing the material. I have already had this inlaid mesh advance course file. I somehow managed inlaid mesh issue.

Now, I am expecting to receive a response related to my last post regarding turbulence in the nozzle flow. I even sent email support@convergecfd.com for this issue.
I hope you could give me some direction.

Thanks again for your kind support.
Best Regards
Omer
__________________
Yanheng Li
Research Engineer-Applications

CONVERGECFD
yli is offline   Reply With Quote

Old   May 3, 2021, 23:32
Default
  #13
New Member
 
Omer Faruk
Join Date: Nov 2019
Posts: 7
Rep Power: 3
Spacebox is on a distinguished road
Hello Yanheng Li,

Thanks for your response.

Yes, it is a RANS simulation using RNG k-epsilon model.
Regarding the BL resolution I have attached an image. I hope it would help for you.

As I explained previously, I used this thick boundary layer to reduce the hole-to-hole error by creating more homogenous mesh distribution for each hole based on the suggestion given another research engineer here. I did also mentioned here that 5um Cartesian mesh size was used in the center to make a smooth transition between inlaid mesh and cartesian mesh.

From my point of view, this is not a BL issue. Before using inlaid mesh strategy, I used only Cartesian-mesh for simulation. In this case, 10um mesh size in nozzle and sac was used. In cartesian mesh case, if you aligned one hole in same-axis for 3-hole and 5-hole injector, you can achieve identical mesh distribution in this hole and easy to compare the results. The results shows that even though some difference is seen in velocity between two injector at the nozzle exit, turbulence (TKE) is quite identical. Same trend was seen using BL strategy as well. Therefore, turbulence difference is not seen in the injectors, especially hole center. Basically, this is the issue.

Look forward to hearing from you soon

Best Regards
Omer


Quote:
Originally Posted by yli View Post
Hi, Omer,
Are you using RANS?Which model? What is your away-from-the wall grid resolution looks like? And what is the last layer of inlaid mesh(adjacent to the Cartesian grid) 's resolution looks like?
Attached Images
File Type: jpg inlaid mesh BL.jpg (88.7 KB, 5 views)
Spacebox is offline   Reply With Quote

Reply

Tags
grid orientation, inlaid mesh, internal flow

Thread Tools Search this Thread
Search this Thread:

Advanced Search
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 Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
Problem with FsiFOAM simulation of beams (2-4 beams) in a steady simple shear flow Aliiiii OpenFOAM Running, Solving & CFD 1 February 27, 2019 12:26
Problem with grid convergence for turbulent flow around cylinder aakie OpenFOAM Running, Solving & CFD 3 November 13, 2018 04:39
parametric study in flow simulation topaz FloEFD, FloWorks & FloTHERM 1 July 13, 2015 08:50
Differences and functions of Solidworks Simulation and Solidworks Flow Simulation? alpharays Main CFD Forum 0 April 19, 2012 03:13
fluid flow fundas ram Main CFD Forum 5 June 17, 2000 21:31


All times are GMT -4. The time now is 13:51.