3d wing from 2d airfoil-volume sweep
Hi all,
I am trying to create a 3D wing in GAMBIT. I am using a 2D airfoil in a Cgrid. When i use Form Volume -Sweep Face, with path vector. I get an error : ACIS error 95034 :Attempt to sweep a non-manifold face. Sweeping or revolving face circl1 failed. The two rectangle faces are made to 3D but the circle face with the airfoil fails. Could anyone guide me how to resolve this please. Could it be due to the two airfoil edges ending at the same point (trailing edge ending at one point)? Thanks in advance. |
you can try a workaround: copy your face with the desired vector, and then create (wireframe) the lateral surfaces.
And finally create (wireframe) the volume |
Thanks Max for that , I am trying it out.
The semi-circle face with the airfoil , I have copied it with the required vector. when you say create wireframe the lateral surfaces. Do I create the edges first to join the two semi-circle faces together then make them into a new surface? |
yes you need to "close" the lateral surfaces by joining your 2 semi-circles.
|
Hi Max,
I managed to create the 3D volume of the semi-circle. Many thanks! I have meshed both sides of the 3D cgrid and have created the volume mesh for the two cubiod parts. When I try to create a volume mesh for the semi-circle I am getting the below error: "volume circle3d cannot be meshed because two sets of source faces which form natural starts for the projections could not be found" I am trying to do a hex mesh type Cooper and giving the two semi-circles as the sources. Do you know what is causing this and what I can do to fix this? |
a picture may help to understand... :)
you can try to split the volume into 2 simpliest volumes |
sorry about that Max :D, I did think of adding my Gambit files , but it was 17Mb. Is there a place I can upload it. Or would a tiff image or even generate mesh do.
I will not be able to do send it untill later on this evening. |
just a picture of the volume giving you trouble
|
1 Attachment(s)
Attached is the image. The semi-circle volume part is what is giving me a problem.
|
ok.
I suppose you have an airfoil or something like this at the center of semi-circles. I would split the volume along the airfoil geometry, like this : Attachment 3013 (see http://www.cfd-online.com/Forums/flu...e-meshing.html) |
Yes in the centre is the airfoil. I will give it ago and let you know how I get on.
I just relised that the wing I am modeling does not have the same chord lenght accross the wing and has rounded tips. I will create a CAD drawing then import into Gambit and start again. Thanks Max for all your help! |
Hello ibzyuk,
I've generated mesh for 3D wing in GAMBIT. The first time I also got the same error with yours. Then I solved it by let the gap between two surfaces of the foil at the trailing edge (I used NACA 0012). Now the mesh works well! Good luck! |
Hi Nvtrieu,
Thanks for that. I did initially try this leaving a gap at the trailing edge, but ran into a few problems. The airfoil I am using is the FX63-137 which is not symmetrical on the x-axis. I took 0.001 of each of the airfoil edge , but when trying to set the surfaces they did not line up. I was following this tutorial: http://web.missouri.edu/~solbrekkeng/TherMMEC/pubs/thesis_logsdon.pdf Do you have any ideas how I can overcome the airfoil not being symmetrical? |
Hi ibrahim,
I also followed that thesis. First step, I create two curves that will be used to make the upper and lower surface later, then use a straight like to connect them at the trailing edge. Then save it in iges file. Second, import the iges file into GAMBIT. After create the faces, the volume is created by using Sweep face function. So in the first step, if we donnt let the gap at the trailing edge, we cannot create the volume for the semi-circle face! Okay, I haven't meshed on non-symmetric foil. However, I think they should be meshed in the same process. So, I just suggest you try to do it one more time then we'll see what happen. Good luck! Trieu. |
Hi guys,
I have a same problem about sweeping the ellipse edge, when I use sweep edge to create the surface, I receive the following error: the edge being swept has moved from its original location. Try changing the default GEOMETRY.VOLUME.SWEEP_PATH_ALIGNMENT to 1 or try aligning the path(edge/vector) to start from edge being swept. ERROR: sweeping or revolving edge edge.3 failed I would really appreciated if you let me know what the problem is?! Thanks |
Hello,
I have the same error ACIS 95034-attempt to sweep a non-manifold. I am trying to sweep a face in Gambit to create a volume.The face contains two blades of a turbine with rectangle surrounding it.I want to create separate volumes for the turbine and the rectangle.Can anyone help me please..? |
post pictures
|
1 Attachment(s)
Hello, I have attached the photo.I tried using split face option and split faced the rectangle and turbine. I also want to mesh the face before sweeping it. PLease can you help me
|
please help me as soon as possible.
Thank You in advance |
sweep the blades for getting volume
sweep (or create your outer box as volume) substract blades volume from outer box |
Hello,
I tried doing as you said. N it did created volumes.but my total mesh is in 100 KB. which should not be the case.I want mesh in 100 MB's and more. Also once when I tried to import that mesh in Fluent I couldn't see the rectangle.Only turbine was imported.This means my geometry wasn't good. |
That means your volume has not been imported.
Your turbine should appear as surface and not as a volume. Did you receive any warning while exporting mesh from Gambit (like warn unmeshed entity are not exported) |
No. It did not gave me any warning. N when u say that turbine should be surface and not volume, what exactly do u mean ? Because when I sweep the face of turbine it creates volume.And i do want volume for both turbine and rectangle.
Do Split -Face option help? My friend suggested to split-face turbine from rectangle, then mesh and sweep it. But that is not helping me either. |
You have 2 volumes: your outer domain and the impeller.
If you subtract the outer domain with the impeller, then you get the outer domain with impeller as hollow. That means your impeller is only represented by its outside surfaces. And the volume represents the fluid domain around the impeller. |
Hii, thanks for the advice.. I got my geometry done. But now i have to restrict the motion of turbine in all directions i.e. translational and rotational except for rotation in x-direction. How do i do that..? Do i use the 'specify continuum types' in zones option in Gambit ? Do i define turbine as fluid or solid type for that?
Please help me |
do you want moving mesh, Single or Multiple Reference..?
check here: http://aerojet.engr.ucdavis.edu/flue...ug/node412.htm http://aerojet.engr.ucdavis.edu/flue...ug/node436.htm |
Moving mesh...
|
then you have to disconnect rotor zone to stator zone.
Doing this, you will able to set interfaces between both zones (one interface for rotor, and one for stator). Then fluent will be able to move rotor zone, and data will be interpolated on interfaces (which you have to define "again" in fluent /define/grid-interfaces) |
How to disconnect rotor from the rectangle ?
|
do a split to distinguish rotor from stator.
If the split is well done, then both domains are connected, which is not wanted. So copy rotor zone with any translations-vector. Delete original rotor zone. Now you can see your stator with an hollow. Define the interface face (stator side) Define the interface face (copy of rotor side) Move back the rotor zone. That's it (Now both interfaces are stacked) |
Hello,
What do you exactly mean by copy rotor zone with any translations-vector ? I did not understand that where should I copy and what rotor zone are you talking about.. What should I do before deleting the rotor? |
if you copy your volume, it will be localised at it original place, and you won't see it
If you give a translation's vector, it will be copied and translated, so that you will be able to delete the original volume http://aerojet.engr.ucdavis.edu/gamb..._volm_movecopy |
Hii, You said to define the interface on rotor and stator.. Is that in Gambit or in Fluent ? and how do you define it? Also you said that - move back the rotor zone.. I did not get it. I will translate the rotor volume- delete original. Then I did not get the interface defining part and again moving back the rotor zone part...
|
5 Attachment(s)
You have to do that in gambit.
I give you an example: -you have a square 100x100 -in the middle you create a rotor zone with radius 10 (just create a circle R10) Attachment 22437 So you split your square (surface) with the circle. It gives you 2 connected zones: the rotor surface (disk R10) and the rest (stator). Attachment 22438 If you mesh both surfaces, they are connected and you don't have any chance to move the rotor zone. For sliding mesh, you need to disconnect both zones and the data interpolation will be done through interfaces. In this case the interfaces will be circles (you need an interface for the stator, and one for the rotor). Now both surfaces are still connected. Copy and translate the disk anywhere and delete the original. Doing that you disconnect both zones and you can assign interfaces easily. Attachment 22439 Attachment 22440 Just move back the copy of rotor. Attachment 22441 That's over: you have stator and rotor disconnected with interfaces Then in fluent grid/interfaces... |
Hii, I tried as you said.. N that was really well explained. Thank you for that. I have a doubt... When i copied the rotor and deleted the original, it did not got deleted in real coz I had used split option between outer box and rotor. So even when i deleted it,I could see the rotor as a whole volume with the box. Is that a problem ?
And after the interfaces are separated, how do i restrict the motion of rotor in all directions except in only one direction..? is that done in gambit itself or I have to use fluent? |
Quote:
Quote:
|
1 Attachment(s)
Good evening to everybody.
Im new to the cfd world so my questions may seem a bit newbish but i really cant help it...so here it goes!First of all id like to say that i am studying the airflow over a wing,namely a s809 3d airfoil,and my goal is to compare the results of this analysis with the experimental ones for various angles of attack as well as various turbulence models (SA,k-e realizable,k-w sst),as far as cl,cd,cm are concerned.Im modelling the wing in gambit and processing with fluent 6.3.My problem came up in 2nd order k-e realizable where i either get the error "turbulent viscosity ratio limited" or i do not get convergence.That is for most of the AoA anyway since ive come across some convergence in some others.My first question then is about the mesh itself.The worst element is in a critical region of the flow and i cant seem to get rid of it.Secondly id like some insight on how to mesh the flowfield next to the wing,meaning from where the wing ends till the boundary.I would be glad if some1 gave me some piece of information! |
All times are GMT -4. The time now is 00:06. |