[ANSYS Meshing] Problem with sweep Method

MrNavierStokes · November 3, 2016, 09:01

Hello CFD community,

I have different pipe sections at the inlet and outlet section of a radial turbine. The first outlet pipe section represents the connection to the rotor domain and is being meshed using tetras. The following sections of the outlet pipe are being swept (see second picture) and I tried to use the same method for the inlet section of the volute. The main part is meshed using tetras but the sweeping method does not work for the inlet pipe (first picture). I receive the following error messages:

A body cannot be swept because the source and target faces are adjacent.

Sweeping failed because there is an existing mesh on one or both of these faces. The existing mesh is most likely due to inflation or selective meshing. To resolve: 1. Specify a different source or target; 2. Clear some body meshes or remesh the entire part; 3. Remove 2D inflation controls.

One or more bodies cannot be swept with the specified source and/or target face because a mesh already exists. The existing mesh is most likely due to inflation or selective meshing.

I checked all of the recommendations and the input is correct. The workflow is the same as for the outlet section: I choose the body and the corresponding source/target face. But it just doesn't work.

Does anybody know a solution for this problem?

Thanks very much!

Regards, Alex.

Gweher · November 4, 2016, 08:52

Hi Alex,

Well apparently the inputs for the manual source and target aren’t correct. In order to avoid overlaps you can use the hide body option to select the proper source and target faces.
Based on the pictures you’ve provided, there shouldn’t be any issue to use a sweep method for this geometry.

MrNavierStokes · November 7, 2016, 03:21

Hello Gweher,

first of all thanks for your answer. I did it exactly the way you described using body hiding and checked a dozen of times for the correct faces, but the problem remains.

I have no clue what could be wrong. Maybe there are some issues concerning the CAD data?

Regards, Alex.

MrNavierStokes · November 7, 2016, 05:33

Dear Gweher,

I was able to fix the issue. I noticed a strongly skewed tri element on the surface of the main part at the edge where the inlet section begins. The edge was divided into a few smaller parts, with one of them being extremely short. This lead to the above mentioned bad tri element ergo a sweep would've resulted in bad mesh quality. Merging those smaller edge sections using virtual topology eradicated the problem.

Thank you for your time!

Regards, Alex.

Gweher · November 7, 2016, 15:08

Thanks for the update Alex. As mentioned, in your case the sweep method shouldn’t encounter any issue, so if you still had a problem even by selecting the proper source and target faces it came from the initial geometry.
De way you create your geometry can affect the downstream meshing. Here you have different options, you can either:

- clean the geometry in the initial CAD modeler
- change the import settings in DM (under cleaning and healing options)
- merge the edges / faces in DM
- use virtual topology in Meshing application
- use a larger defeaturing option under the mesh settings in Ansys Meshing

Best

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
Problem with implementing unsteady Kutta condition-Hess and Smith Panel method	samarthgk.nitk	Main CFD Forum	0	June 25, 2012 03:36
FSI Problem - Utilizing ALE method to map solutions	natern	OpenFOAM	1	November 7, 2011 18:00
a problem about pressure correction method	tommewang	Main CFD Forum	2	May 15, 2003 22:18
what is time marching problem and method	F. Zhen	Main CFD Forum	0	May 9, 2003 15:51
finite difference method for navier-stokes problem	dallybird	Main CFD Forum	5	February 17, 2003 23:00

November 4, 2016, 08:52		#2
Gweher Senior Member Gwenael H. Join Date: Mar 2011 Location: Switzerland Posts: 392 Rep Power: 20	Hi Alex, Well apparently the inputs for the manual source and target aren’t correct. In order to avoid overlaps you can use the hide body option to select the proper source and target faces. Based on the pictures you’ve provided, there shouldn’t be any issue to use a sweep method for this geometry.

November 7, 2016, 03:21		#3
MrNavierStokes New Member Alex Join Date: Jun 2015 Posts: 22 Rep Power: 0	Hello Gweher, first of all thanks for your answer. I did it exactly the way you described using body hiding and checked a dozen of times for the correct faces, but the problem remains. I have no clue what could be wrong. Maybe there are some issues concerning the CAD data? Regards, Alex.

November 7, 2016, 05:33		#4
MrNavierStokes New Member Alex Join Date: Jun 2015 Posts: 22 Rep Power: 0	Dear Gweher, I was able to fix the issue. I noticed a strongly skewed tri element on the surface of the main part at the edge where the inlet section begins. The edge was divided into a few smaller parts, with one of them being extremely short. This lead to the above mentioned bad tri element ergo a sweep would've resulted in bad mesh quality. Merging those smaller edge sections using virtual topology eradicated the problem. Thank you for your time! Regards, Alex.

November 7, 2016, 15:08		#5
Gweher Senior Member Gwenael H. Join Date: Mar 2011 Location: Switzerland Posts: 392 Rep Power: 20	Thanks for the update Alex. As mentioned, in your case the sweep method shouldn’t encounter any issue, so if you still had a problem even by selecting the proper source and target faces it came from the initial geometry. De way you create your geometry can affect the downstream meshing. Here you have different options, you can either: - clean the geometry in the initial CAD modeler - change the import settings in DM (under cleaning and healing options) - merge the edges / faces in DM - use virtual topology in Meshing application - use a larger defeaturing option under the mesh settings in Ansys Meshing Best