Pointwise Mesh to Fluent Multiblock Issue

NeroBlade · January 26, 2016, 10:39

Hey folks,

I've stumbled upon an issue that I've been experiencing lately when I've started using the Pointwise meshing software and exporting the mesh onto Fluent.

I setup the structured meshing parameters for each edge to suit my needs for a simple cube case and then I select all the blocks generated and export a new case file. The cube and floor is wall, sides and top are symmetric and an inlet and outlet is included.

Everything seems fine until I run the simulation with the same physics as before but the converged result seems to have some interface problems between each block as shown on the below image.

The exported mesh contains two interior blocks one being the blocks themselves and the second being the interface in between.

Any suggestions of idea why does this occur and would anyone know how to resolve this?

Cheers,
Lee

cnsidero · January 28, 2016, 23:33

In Pointwise create a Volume Condition, assign both blocks to it and change the type to Fluid. Then when you export the mesh to Fluent there will be one zone and the interior interface between them will disappear.

NeroBlade · January 29, 2016, 08:01

Thank you cnsidero, I gave that a shot and exported it but I still have the two interior zones.

I selected all the outer blocks around the cube and assigned the volume condition as fluid and the cube itself I assigned it as solid and exported.

Below is the screenshot of the issue.

cnsidero · January 29, 2016, 09:34

This likely means some blocks are not point matched. Go to Set CAE Boundary Conditions. If any internal domains are selectable then your blocks are not point matched (e.g. mismatching connectors).

NeroBlade · January 29, 2016, 10:08

Okay, because what I've done was I've created the connectors for one side and then copied the connectors and pasted them in a translated position via z axis. Then afterwards used connectors to connect the two sets of connectors together. Is this the correct procedure?

I checked via boundary conditions and no internal domains are selectable, which is a good sign.

cnsidero · January 29, 2016, 10:19

It's tough for me to tell what the issue is. Are you able to attach the .pw file (or provide it some other means)?

NeroBlade · January 29, 2016, 16:19

Sure okay, here's the .pw file.

https://www.dropbox.com/s/8qvm442l2y...ube_0h.pw?dl=0

RcktMan77 · February 1, 2016, 12:07

I believe the interior boundary condition within FLUENT is just its way of identifying the interior faces between blocks. It uses this interior boundary condition to interpolate solution information at these faces.

After looking at the initial picture of your solution that you posted and then your mesh, I think the issue you're having is more due to the large jumps in spacing the you have. For example there's a 40x jump between the mesh spacing on the face of your block and the initial spacing used to resolve the viscous region surrounding the cube. A similar jump exists between the blocks aligned in the same y-plane as your cube and the farfield mesh adjacent to it. You want to avoid jumps like this and have a smooth transition between cells where the growth rate between cells is no larger than 1.2.

As information is interpolated along these interior faces, you don't want to have large jumps in your mesh in these regions, which is likely the phenomena you're observing in the image of your solution that you posted.

Similar Threads
Thread	Thread Starter	Forum	Replies	Last Post
sliding mesh problem in CFX	Saima	CFX	46	September 11, 2021 08:38
Importing 2D separated Hybrid mesh from PointWise to Ansys Fluent	Masoud.A1	Pointwise & Gridgen	6	July 8, 2017 10:23
Interesting problem: Parallel Processor VOF Fluent + Dynamic Mesh + System Coupling	spaceprop	FLUENT	5	September 2, 2014 10:43
FLUENT Not Recognizing That Mesh Has Been Updated	tantin	FLUENT	0	January 7, 2013 20:01
Moving Mesh Velocity Issue: Mesh velocity does not equal displacement	Doginal	CFX	2	September 8, 2011 13:02

January 28, 2016, 23:33		#2
cnsidero Senior Member Chris Sideroff Join Date: Mar 2009 Location: Ottawa, ON, CAN Posts: 434 Rep Power: 22	In Pointwise create a Volume Condition, assign both blocks to it and change the type to Fluid. Then when you export the mesh to Fluent there will be one zone and the interior interface between them will disappear.

January 29, 2016, 09:34		#4
cnsidero Senior Member Chris Sideroff Join Date: Mar 2009 Location: Ottawa, ON, CAN Posts: 434 Rep Power: 22	This likely means some blocks are not point matched. Go to Set CAE Boundary Conditions. If any internal domains are selectable then your blocks are not point matched (e.g. mismatching connectors).

January 29, 2016, 10:08		#5
NeroBlade New Member Join Date: Jun 2014 Posts: 10 Rep Power: 12	Okay, because what I've done was I've created the connectors for one side and then copied the connectors and pasted them in a translated position via z axis. Then afterwards used connectors to connect the two sets of connectors together. Is this the correct procedure? I checked via boundary conditions and no internal domains are selectable, which is a good sign.

January 29, 2016, 10:19		#6
cnsidero Senior Member Chris Sideroff Join Date: Mar 2009 Location: Ottawa, ON, CAN Posts: 434 Rep Power: 22	It's tough for me to tell what the issue is. Are you able to attach the .pw file (or provide it some other means)?

January 29, 2016, 16:19		#7
NeroBlade New Member Join Date: Jun 2014 Posts: 10 Rep Power: 12	Sure okay, here's the .pw file. https://www.dropbox.com/s/8qvm442l2y...ube_0h.pw?dl=0

February 1, 2016, 12:07		#8
RcktMan77 Senior Member Zach Davis Join Date: Jan 2010 Location: Los Angeles, CA Posts: 101 Rep Power: 16	I believe the interior boundary condition within FLUENT is just its way of identifying the interior faces between blocks. It uses this interior boundary condition to interpolate solution information at these faces. After looking at the initial picture of your solution that you posted and then your mesh, I think the issue you're having is more due to the large jumps in spacing the you have. For example there's a 40x jump between the mesh spacing on the face of your block and the initial spacing used to resolve the viscous region surrounding the cube. A similar jump exists between the blocks aligned in the same y-plane as your cube and the farfield mesh adjacent to it. You want to avoid jumps like this and have a smooth transition between cells where the growth rate between cells is no larger than 1.2. As information is interpolated along these interior faces, you don't want to have large jumps in your mesh in these regions, which is likely the phenomena you're observing in the image of your solution that you posted.