Hi everyone

I have created a turbine which sits on a structure made up of cylinders, spheres and cuboids. I have tried to mesh the 3D structure but am having big problems with Skewness. When i attempt to mesh it tells me the skewness on some faces is too high, i then change the mesh on these faces and it effects the skewness on other faces and so the cycle continues...

I think the problem is with the way I have constructed my geometry. Can i just confirm something (I have never taken any training in GAMBIT)?

Is there particular methodology you must stick to when joining up solids? I have literally just let my shapes over lap (but not stick out) and joined them together.

Cheers

dave

take care of edges wich produce very small angle. Typically a circle on a surface. if the circle is tangential to one of the extremity of the surface, wou'll have skewness problem

I have 2 cylinders intersecting with the end face of the smaller one sitting inside the shaft of the other...what are the implifications of having that face inside the other solid?

how did you connect the 2 cylinders? if you united them, then you shouldn't have any surface inside any cylinder. you can put your dbs file on one server, I will take a look at it

mAx

I have wrapped a box around the structure which will be used to define my boundary conditions. The actual structure itself can be played around with in terms of being moved/rotated a little bit here and there if that helps with getting rid of the acute angles.

Thanks for this, let me know what you think

http://www.megaupload.com/?d=WQQICVDY

Dave

ok, I checked your geometry. Your problem isn't a technical problem, but an understanding one. You are using Fluent for computing impact of wind on your impeller. So you have to take care on the fluid domain which is between your impeller and the outside domain. Thus you have created a box which surround your impeller. This is ok. But you have to substract this box with your impeller for having the right fluid domain. And before that you must unifify all the volumes which define your impeller. (you are just interested by the outside design of your impeller). So in Gambit, do this: Geometry/Volume/unify .... volume unite volumes "volume.3" "volume.6" "volume.7" "volume.8" "volume.9" \ "volume.12" "volume.13" "volume.14" "volume.15" "volume.16" "volume.20" \ "volume.21" "volume.22" "volume.24" "volume.25" "volume.26" "volume.27" then your impeller will be defined by volume 3 you still have volume 23 which is your box. Fluid domain will be the domain between the box (23) and the impeller (3) So Geometry/Volume/substract volume subtract "volume.23" volumes "volume.3" Finally you still have just one volume (23), which is your fluid domain (the right one) you can now try to mesh it, but you will have problem on face 25,102,103. So go and merge them: face merge "face.24" "face.25" "face.103" "face.102" mergelower after that you can mesh your geometry.

mAx

Thankyou for that. I would never have though to merge those faces together and it seems to have got rid of most of my problem - I had originally did the same thing as you suggested, i.e. create one volume.

A problem has arose now which appears to be simply solved but that is not proving to be the case. For some reason I cannot mesh the faces of the 2 cylinders at an angle to the X-plane (faces 52 and 54). It says the triangular surface mesh failed for both. I have tried to mesh these using every possible element and type but I cannot get them to mesh - do you have any idea why this may be happening?

It always seems like sorting out one mesh in GAMBIT leads to a you mucking up another one! Makes me sick i tell you...

Dave

I also have the same message if I mesh them with size 1 (tri). Size 1 is too coarse. If I switch to size 0.1 I don't have any problem. Take care for having a fine mesh on your impeller, else you will have problem with the convergence.

Cheers for your help...I have finally meshed it and imported it into FLUENT where it iterating at the pace of an asthmatic ant.

Dave