Problems with volume defining
 

Hi,

I'm new to using ANSA and I'm having problem with defining volume for volume mesh. It's an external aero case. Model has some closed volumes that are separate from car body - rear wing stand, side mirror, radiators etc. This volumes are detected easily. Than there's main volume and it's bounds are defined by car body, wheels and wind tunnel walls - for whatever reason this main area can't be defined. Things warked fine with external aero tutorial but here...

Any suggestions on what I'm doing wrong here?

http://www.cfd-online.com/Forums/<a ...psmvbs3nvm.jpghttp://i1370.photobucket.com/albums/...psmvbs3nvm.jpg

Highlighted in wight are volumes that are defined - all of them are not in contact with tunnel walls. Why I can't define the main volume? It didn't work after creation of layers and later (attached image) I decided to try to define it before creating layers (simplier model) but it didn't help. I would think that this geometry is not fully closed and that's why it can't be defined as volume but I can't find any openings - all bounds are yellow...

Thanks
Ted

Problem solved!

Thanks :)

Well... I was too quick to say that problem is solved :) It did work before creating layers - I could define main fluid volume (tunnel around car) but it fails to define it after layers creation.

Thanks
Ted

Hi Ted
You seem to have made a nice surface mesh there!!

Some suggestions

1) The main volume must be detected and defined AFTER layers generation
2) Before layers try the following
Switch to display mode Mesh Check Gaps (this is at the right end of the bottom buttons) This should show you in Red and openings in the mesh
3) Check also if there is an opening using Isolate>Short Path>Leak
Select a point inside the volume and confirm
4) Check also for duplicate elements Check>Duplicate

Let me know how it goes

Vangelis

Hi Vangelis,

Thank You! I really appreciate your help!



I was trying to define main volume before layers after I failed to define it after layers creation – in search to isolate the problem and find out at which step it pops up. It did help to find initial problem – I had to reconnect car body to symmetry plane – bounds where yellow but still there was a problem. Deleted sym plane, made a new surface for sym plane and re projected car body bounds on sym plane and after that I could define main volume to confirm that there are no leaks. Than I started adding layers but this time I first added layers to road and rear wing – I could still define main volume. Than I tried to add layers to car body and after that I could not define main volume. Than I tried to do as you suggested in another thread – open sets and click on collapsed areas to make them visible, than define volume and it seem to be working.



I would like to ask for more details on that point – making collapsed/excluded areas visible before defining main volume. What I did is just click them so they become visible, than Define->OK. Than I could define main volume.



I will fallow your suggestions and report here.

Thank you!
Ted

Hi Ted

Which ANSA version are you using?

A suggestion, when you grow layers, grow them all in one step
Do not grow the layers in steps (first road, then vehicle for example)
as there may be issues with connection of layers at the sides.

Best regards
Vangelis

Many thanks for your help and suggestions!

v 15.3.1 here

I will report on my progress with this model.

Thanks
Ted

Since v15.2.4 there is no need to hide anything prior to Volume Detection.
Just have ALL visible (Macros and FE-mod mesh)

Let me know if there is an issue

Still having problems here...

Can't define main volume after layers creation (it was working if I only grew layers on rear wing for example)

I did check (before layers) for leacks - no common path found, no duplicate elements either.

Really I'm bit lost here... Seems like I'm missing something very simple.

Is there any possibility that you can take a look at my file? (I can upload it and send you its link)

Thanks
Ted

Have you checked that all Faces are properly oriented INWARDS?
Gray inside the volume?

Of course I can,
If you want send the link as a message

Many thanks! Uploading now.

Yes - definately all yellow facing outwards and grey inwards. As I sayd - it has no problem defining volume before layers are added.

Thanks
Ted

Vangelis,

Just sent you a PM with a link. Please let me know if link is working for you.

Thanks
Ted

Hi Ted

I have a couple of questions.
1) Your model has baffles or zero-thickness walls.
You can identify them if you have the whole model
visible and press
Isolate>Baffles from the top buttons.
You therefore need to be careful where you grow layers from. Usually for baffles you grow layers from both sides.
2) I also think that you should close the large radiator volume
in the symmetry plane. I assume you want to mesh it for porous
medium modelling.
3) why are the tyres not connected to the wheels?
4) For which solver do you want to mesh this and how many elements do you want to have approximately?
5) There are also some needle faces, use Check Geometry to find them and delete them.

To answer your questions:


1. I defined buffles individually because I thought that I do want to grow layers in both directions for PID’s Turning_vanes and RearFlares but for Hood, Front bumper IC_inlet, IC exit, radiator inlet, radiator exit I thought that I only need layers on the positive (grey) side – because I thought that those areas under the hood would not have a large influence of overall lift/drag. I would love to learn what you think regarding those (underhood) surfaces – is it really needed to grow layers on both sides?


2. I will close radiator volume – thanks!


3. Well… that wasn’t my idea J but my friend (he’s ANSYS CFX trainer at local ansys office) suggested that there’s relatively large pressure difference on inside (under the car) and outside of wheels. He felt that it’s important to simulate the gap between brake rotor and wheel.


4. I would prefer to mesh this for CFX.
Initially I would like to have approximately 14-18000000 elements for initial run on 32Gb machine. But later when I see that there are no glitches etc. I would like to make a mach more refined model – I’m promised time on large cluster (2Tb) so I would like to refine the model till there’s no significant changes to results anymore.



Thanks
Ted

I noticed that model that I've sent you was wrong in terms of mesh size on underbody. I'm uploading correct model now.

Thanks
Ted

Hi Ted
Just a reminder in the end you have all detected volumes meshed.
I think you need to delete the volume of the rear wing support before outputing the mesh.
Also you need to use Volumes>SET PID to change the property of the radiators.

Here are some tips

As I mentioned earlier when you have baffles it is best that you
grow layers from both sides, even if one side is not so important to the flow,
otherwise you have problems, as the layers are not continuous all around the starting model.
Also you need to be very careful of the orientation.
And of course you need to check from which PIDs you grow layers and from which you do not.

In the final model you will notice I have set some PID names to end with baffle
and some with no_prism.

In this way I know which PIDs to put in which batch mesh session or area.

If you work with this file you will be able to make any changes very easily and quickly.

Good luck with your work

Vangelis

Many thanks for your help Vangelis!

Amazing work indeed!

Now I have to learn a bit more about batch meshing and analyse the way you created this model.

Thank you very much!
Ted

Hi Vangelis,
Passed the mesh to CFX and started the run but solver complains about some of the elements (its face) on the symmetry plane not being parallel to the plane and doesn't report its coordinates/location.

Is there a suitable instrument in ASNA which I can use to try and find it so I can try and fix it?

Thanks
Ted

Hi Ted

Maybe quality improvement step moved away a node from the symmetry plane.

Follow these steps

-Isolate on the screen the shell mesh of the symmetry plane
-Open the DBbrowser
-Double click on the Node entry to open the Node LIst window
The window will appear empty because the ANSA file contains many nodes
so do not worry about this
- Select with Box selection all the grids of the symmetry plane
- in the Node LIst window, right-click on the column of Y coordinates
type in it 0 to force 0 y to all nodes and press Enter
- Now all the nodes of the symmetry plane should have y=0

let me know if this works

Thank you Vangelis!

It works - I can see that all the distorted elements are aligned with sym plane now. I will be able to retry it in slover in fiew hours and will report back.

Thanks
Ted