Mesh Control

[Anonymous]

Hi,

I have issue regarding mesh control. I have test data Flow rate vs Pressure drop. I want to find the opening of check valve. With formula I have find out the opening but in simulation when I use the calculated opening I get different pressure drop. When discussed, my colleague (who is CFD specialist but uses Ansys) told me, that in the valve there is rubber membrane, so formula might give you some value but in reality it will be different. So he advised me to change opening value in simulation till I get the pressure drop value which matches with test data and that will be correct opening. So, I am changing the opening of valve (+/- the calculated one) by keeping flow rate constant and checking the pressure drop. Now, as one can understand it will take lot of time for trial and error. So, I did the adaptive meshing for calculated opening find out potential areas where mesh should be fine. I did this, because model is very complex and number of cells are more and it takes lot of time for simulation. With adaptive I can go 1 original and next one after that cell count increases so much that laptop hangs. So, I want fine mesh only in region of interest and coarse in other.

What I want to achieve I have explained in images which one can found in zip file. I am also sharing cfz file so that you will get idea of geometry. I want to control cell size radially on circular portion of membrane. I have done following things and I am talking about effect of various settings on small gap meshing and not about meshing effect on other areas:

1) I tried to define region with auto and manual meshing. Problem is number of cells increased too much in both cases even if other areas I keep coarser. I did not get spacing finer in radial direction the way I got with adaptive mesh (please see the image for understading my requirement)

2) I tried to select respective surface and edges of the surface I am interested in and applied finer mesh still radially the mesh size is coarse.

3) I tried Surface Growth (1.05) , fluid gap (3), volume growth (1.1) one option alone and combinations also. Still generated mesh looks the same as mesh generated with default option in the interested area.

Thanks in advance! As one post said Autodesk should include Circular option for Region to control mesh size. Now I also feel the need of this option.

Best Regards,

Rajdeep Rajput

[Anonymous]

Or is there any way so that one can define the region where mesh should be adapted in adaptive meshing and other regions should remain as it is? So, the number of cells will not increase too much.

[Jon.Wilde]

Hi,

Have you tried giving that surface (assuming this is 3D) a uniform mesh?

Where is thie curve on your model? I can't find it at all.

Thanks!

Jon

[Anonymous]

Hi,

Please hide the surface shown in picture. Then, you could be able to see the curved surface I am talking about. In second image, its been marked with

color of selection.

When I try uniform mesh the number of elements increases so much that to create mesh it takes forever. RAM is 8GB and processor is i5 2.6GHz (physical 2 cores logical 4 cores).

Regards,

Rajdeep

[Jon.Wilde · Accepted solution]

Also - you only have 1 Gap Element set within the Advanced setting - try 3

Looks pretty cool to me 🙂

This is the Auto Mesh with that curved surface given a refined uniform mesh.

[Anonymous]

I have already tried gap element option. Is not there any way that  adaptive mesh option should refine the mesh only in that area and remaining should be as it is so that computer with nominal hardware configuration should be able to simulate complex parts? In that case, number of elements will not increase exponentially, which is now happening.

[Anonymous]

Hi,

Mesh issue is solved. I used manual mesh. The trick is I have to select curved surface and adjacent surface to give small element size (See attached images). Curved surface alone does not give desired result. In manual mesh, I select surved surface defined element size 0.05 and adjacent surface as 0.1. Then I created box in all critical regions to refine individually. For complete Volume Element size = 1. And box for this curvature region element size = 0.1 and other areas I kept around 0.4.

Now number of elements are large but not too large, as laptop can handle it.  

Thanks for the help.

Regards,

Rajdeep Rajput

[Jon.Wilde]

Hi, I would stick to what I shared, the mesh in those images has a boundary layer that is very thick. Compare the mesh you have to the image above - an Auto mesh is fine but then just refine the curved surface with a 'uniform mesh' - looks really nice.

It isn't possible to to use Adaptive mesh locally, but CFD should only refine where it is needed. You could try enabling 'allow coarsening' so CFD can reduce the mesh where it can.

Personally I just do a quick manual check, check this out: Manual Mesh Sensitivity Study

[Anonymous]

Okay. I will try with autosize and manual mesh independence study.

The other point that you said about adaptive meshing. I indeed checked that box "Allow Coarsening". But, the thing is adaptive mesh still refines the mesh everywhere, In my case, the pipe diameters is changing it will refine in that area also. May be those area also have pressure gradients. But, more effect is causing due to curvature surface and small gap for air to flow. So, when one wants to save time just to get quick and approximate idea about how valve opening affecting the pressure dropone should be able to control that area. In my case that gap is playing crucial role in pressure drop calculation other areas are not affecting that much as their dimensions are greater than small gap. That gap is just 0.054mm.

So, I thought adaptive mesh should have such option of controlling particular regions.

Anyways I will do what you suggested. I hope with 0.7 refinement number of elements do not increase too much.

Regards,

Rajdeep Rajput

[Jon.Wilde]

This is a nice idea for our Idea Station if you have time to suggest it 🙂

[Anonymous]

Hi,

I read your article about manual mesh sensitivity study. My question is after cloning and refining the mesh with 0.7 refinement iterations should be started from 0 or from iteration of the last study.

I have already started from last iteration of the previous cycle. But, I want to be sure and may be you can edit that article to make it more clear.

Regards,

Rajdeep Rajput

[Jon.Wilde]

Good idea, it doesn't really matter though. CFD will start over or interpolate results and continue, which is faster depends on the model size 🙂

[Anonymous]

Hi,

Could you please send me detail settings fro above image or screen shot of meshing tab from design study bar? I could achieve refine curved surface but I have few elements between curved and straight surface and in above image that you have shared has more elements and very close to each other. I have set gap elements to 3 still it is the same problem.

Regards,
Rajdeep Rajput

[Jon.Wilde]

Sure - I did this:

1. Select just the surface
2. Press 'uniform'
3. Refine the mesh with the slider bar (not sure what value now)
4. Press Apply
5. Press Spread Changes
6. Generate the Mesh to see if you actually need a finer mesh setting

Remember also to press the 'Apply' button with the '!' sign after changing and Surface and Gap Refinement settings.

Thanks,

Jon

[Anonymous]

Hi Jon,

I am doing the same thing. But still the mesh that you created has very small and uniform elements; while the mesh I am creating is looking robust. Please see the attached image and notice the difference between your mesh and mine then you will understand what I am talking about.  My mesh settings can be seen on left. The gap elements are 5 now.

One strange thing I noticed. I am using Catia. So, for CFD I am using directly CATPART. When I use CATPART directly, GAP ELEMENT option does nothing means I do not get finer mesh. Then I downloaded the ZIP which I have attched here and did the same thing what have you done and then I get finer mesh like in image (still not satisfactory as your mesh looks far better). I do not know why it happens. There is one article also which says "Gap Refinement Meshing is only available for 3D Acis-, Parasolid-, and Granite (Pro/Engineer)-based models." Is it so? Check below link for the above statement.

http://help.autodesk.com/cloudhelp/2014/ITA/SimCFD/files/GUID-7BFD671B-B6BA-4E6A-A67D-5DA51A3BC0AD.h...

Last important question, when we click on surface and gap refinement button and go to advanced settings to change Gap Elements to 3, then there appears small triangle with '!' sign for REFINE BUTTON. You said in the last post "Remember also to press the 'Apply' button with the '!' sign after changing and Surface and Gap Refinement settings." So, should I left the sign as it is and press apply directly or should I first click on Refine button make that triangle sign disappear and then press Apply? Because, right now what I did was I clicked on Refine Button after I get that triangle sign made that triangle sign disappear and then pressed apply.

[Jon.Wilde]

Sorry - yes use the 'Refine' button where the '!' is.

I used 3 Gap Elements. How about launching into Sim Studio first so that it works? (I think you will need CFD 2016 for this though).

Or use it to save out a .sat file and read that into CFD?

I did only use your 6lpm CFZ before though.

Hope that is useful,

Jon

[Anonymous]

I have CFD 2016 Installed. But, when I try to simulate at License check it fails. I tried everything but no solution to license problem. But 2015 works fine so I reinstalled 2015. Will meshing between 2015 and 2016 differ even if settings are kept same?

[Jon.Wilde]

Sounds like you need a new 2016 licence file - I suggest a post in the licencing forum 🙂

For 2015 though, yes I think you should be OK. There are typically subtle changes but in both versions you should be able to get great results!

[Anonymous]

Hi,

I tried exactly the way you instructed. I applied those settings on 6LPM CFZ and I also tried same settings by converting that File to SAT using Sim Studio. Still I get mesh like shown in figure. On left hand side one can see mesh settings. Gap Elements 3. Could you please do meshing again on 6LPM CFZ that I have attached in the very first message and then share that CFZ with me? I will just generate mesh and will see if there is problem with CFD or RAM or some hardware thing?

Thanks in advance!