# what to do w/ highly skewed elements? (GAMBIT)

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

 May 13, 2007, 23:33 what to do w/ highly skewed elements? (GAMBIT) #1 mike Guest   Posts: n/a hi folks, i'm trying to model a 3d rotating car tire. i've kept everything very simple with the geometry: it is simply a cylinder within a rectangular brick (far field). the cylinder interfaces with the brick with an infinately small contact patch. i use boolean subtracts of the volumes, create a size function around the tire, then try to mesh the volume. even with an extremely small initial mesh size on the tire of 0.25, the mesh will not generate due to too many highly skewed elements. the highly skewed elements originate at the contact patch, and then procede outward. the next thing i tried was to create a small face around the contact patch, and include that in the size function. this did not improve the situation. finally, i have tried to mesh the small face and the tire faces independantly, then mesh the volume. this allowed for a mesh to be generated, but there are more than 1500 highly skewed elements (again, originating from the contact patch). any ideas would be greatly appreciated.

 May 14, 2007, 01:44 Re: what to do w/ highly skewed elements? (GAMBIT) #2 H.A.S Guest   Posts: n/a hello , Try to use the edit panel in Gambit and to change the value of the skewed number that was initially to more than 0.97 . Most probabely it will works . Edit - Defaults ... OR Try to mesh it with a smalller interval size , in ur interested region then make the interval size larger whenever u r far from it .

 May 19, 2007, 20:47 Re: what to do w/ highly skewed elements? (GAMBIT) #3 HAYATI ERKAN TASYUREK Guest   Posts: n/a First, Change the``Meshed S.F. on B.L. CAP`` Number from volume mesh , meshing interface.It is originally 1.2 but try 1.5 or 1.6 or something more than 1.2, probably it will solve your problem. Or you may mesh the model from another FEM software like Unigraphics, Ansys or solidworks etc. then you may export the mesh to Fluent or Gambit if your problem continues. Good Luck...

 May 21, 2007, 07:41 Re: what to do w/ highly skewed elements? (GAMBIT) #4 E Eklund Guest   Posts: n/a Hi, The reason for the high-skewed cells are a simply due to the very acute angle between the cylinder and the wall. This is a common problem in automotive industry, and there is essentially only one solution to ensure good quality. A very small fillet has to be created around the contact patch. This can be done in GAMBIT by copying the floor plane a small distance above the floor, use this plane to cut the cylinder again. Now Sweep the edge created on the cylinder down through the floor and split that face with the floor. Good Luck !

 May 23, 2007, 22:59 Re: what to do w/ highly skewed elements? (GAMBIT) #5 mike Guest   Posts: n/a thanks everyone for the responses. i'm afraid that i wasn't able to quite understand the response from 'HAYATI ERKAN TASYUREK'. i understood the bit about changing the ratio from 1.2 to 1.6, but i didn't understand the first bit that you mentioned. 'E Eklund', i tried your suggestion, and also bumped into an article on the FLUENT website: http://www.fluent.com/solutions/auto...bile_wheel.pdf it helped me understand the concept of how the moving walls work a bit better. i also put a small fillet between the wheel and the ground (i did this in CATIA, as it is a one step operation). this helped the meshing problem. i've managed to get a solution out of FLUENT using this mesh, but will continue to tinker with it. thanks very much for your help.

 June 2, 2007, 22:10 Mesh Export #6 HAYATI ERKAN TASYUREK Guest   Posts: n/a Mike, Meshing process in Gambit is really a nightmare, if your problem is still continue, you can make your mesh by another software ( Annsys, Unigraphics or Solidworks) then you can import that mesh file by GAMBIT... Sometimes, meshing with Gambit takes forever thats why mesh export is very common in CFD. Take it easy bro, HAYATI ERKAN TASYUREK Claire Yu likes this.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post rk2011 Main CFD Forum 1 January 26, 2011 19:24 Sanjay Jain FLUENT 1 April 8, 2008 15:57 xiaofish FLUENT 3 September 18, 2007 09:51 Hengky FLUENT 2 August 11, 2005 12:17 Chie Min CFX 5 July 12, 2001 23:19

All times are GMT -4. The time now is 06:35.