CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > ANSYS Meshing & Geometry

[ANSYS Meshing] ANSYS Meshing Issue - How To Mesh Complicated Geometry (~80,000 Faces)?

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   October 9, 2019, 06:12
Default ANSYS Meshing Issue - How To Mesh Complicated Geometry (~80,000 Faces)?
  #1
New Member
 
Sam Marshall
Join Date: Oct 2019
Posts: 4
Rep Power: 2
Sam Marshall is on a distinguished road
I am attempting to mesh a complicated design (~80,000 faces) for a microchannel heat sink, as pictured, and I would appreciate some advice. I have tried a range of different mesh controls (especially face sizing and body sizing), mesh settings and element sizes, and all have failed to produce a working mesh. The most common errors are shown in the attached picture, in particular the one regarding "The following surfaces cannot be meshed with acceptable quality. Try using a different element size or virtual topology." However, I have already reduced the element size to 2x10^-6 m, which takes two days to resolve before failure.


Unfortunately I cannot alter the geometry significantly, as it is imported from generation in SolidWORKS as either a STEP or an x.t file. As such, any advice for how I can successfully mesh the geometry for CFD analysis in FLUENT would be greatly appreciated.


I can provide more details or the geometry file itself if required.


Thanks in advance.
Attached Images
File Type: jpg Meshing Attempt.jpg (76.0 KB, 28 views)
Sam Marshall is offline   Reply With Quote

Old   October 9, 2019, 07:48
Default
  #2
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 350
Rep Power: 15
Gweher will become famous soon enough
Hi Sam,

It's a bit difficult to get a sens of the geometry, but I would use Spaceclaim to edit the .step file. As it's a direct modeller you can directly edit geometries without the need to reverse engineer them.

So I would start with cleaning-up unnecessary geometrical details, and also run through some of the repair tools in Spaceclaim (gaps, duplicated edges, etc...).

Then I would play around with the mesh parameters.

Have fun
Gweher is offline   Reply With Quote

Old   October 9, 2019, 22:50
Default
  #3
New Member
 
Sam Marshall
Join Date: Oct 2019
Posts: 4
Rep Power: 2
Sam Marshall is on a distinguished road
Quote:
Originally Posted by Gweher View Post

It's a bit difficult to get a sens of the geometry, but I would use Spaceclaim to edit the .step file. As it's a direct modeller you can directly edit geometries without the need to reverse engineer them.
Thank you for your response. Please find attached some images that might better visualise the geometry. The design is a 15mm long microchannel with two large "hills" or "rolls" that make up the major features. The shape was defined via topology optimisation in COMSOL, then a solid body was generated in SolidWORKS. I am hoping to use FLUENT to simulate a fluid passing over this geometry.

Quote:
Originally Posted by Gweher View Post

So I would start with cleaning-up unnecessary geometrical details, and also run through some of the repair tools in Spaceclaim (gaps, duplicated edges, etc...).
I have attempted to use the Repair tools (especially Repair Faces) in Design Modeller, as well as the Merge function, and they have either not solved the meshing issue or failed outright. I will try to repeat the process in SpaceClaim, though I am less familiar with that program. I'll let you know if it works or not.

Best regards.
Attached Images
File Type: png Model Geometry.PNG (176.1 KB, 19 views)
File Type: png Front, Top and Side Views.PNG (134.9 KB, 16 views)
Sam Marshall is offline   Reply With Quote

Old   October 11, 2019, 05:57
Default
  #4
New Member
 
Sam Marshall
Join Date: Oct 2019
Posts: 4
Rep Power: 2
Sam Marshall is on a distinguished road
Quote:
Originally Posted by Sam Marshall View Post
I will try to repeat the process in SpaceClaim, though I am less familiar with that program. I'll let you know if it works or not.
Unfortunately, I have now attempted to use SpaceClaim to simplify the geometry, without success. In particular, when I try to use options such as Small Faces, the program crashes.

Do you have any other advice on how to simplify the model without significantly altering the design?

Thanks again.
Sam Marshall is offline   Reply With Quote

Old   October 14, 2019, 08:53
Default
  #5
Senior Member
 
Gweher's Avatar
 
Gwenael H.
Join Date: Mar 2011
Location: Switzerland
Posts: 350
Rep Power: 15
Gweher will become famous soon enough
Hi Sam,

In design modeller it will be way more complicated than in SpaceClaim. I'm thinking of two approaches. First you can play around with the repair tools. In your case as it appears that you have a lot of small faces you could also imprint different "regions" of your model and use the split face first and then regroup several faces using merge tool / repair tools. If your model is too large for your hardware resources it could be that the small faces repair tool crashes. If I remember correctly you can limit the number of faces to correct at once to help SpaceClaim to progressively repair / smooth your model.


Second option which I think would be more straight forward is to directly import the .stl file from the Comsol optimization and use the facette smooth tab in Spaceclaim. This will avoid initial processing in Solidworks before sending the geometry to SpaceClaim. Once you're happy with the smoothing you can then transform the facetted geometry to solid > rbm on the geometry > convert to solid > merge faces.

Have fun
Gweher is offline   Reply With Quote

Old   November 11, 2019, 03:14
Default
  #6
New Member
 
Sam Marshall
Join Date: Oct 2019
Posts: 4
Rep Power: 2
Sam Marshall is on a distinguished road
Quote:
Originally Posted by Gweher View Post
Second option which I think would be more straight forward is to directly import the .stl file from the Comsol optimization and use the facette smooth tab in Spaceclaim. This will avoid initial processing in Solidworks before sending the geometry to SpaceClaim. Once you're happy with the smoothing you can then transform the facetted geometry to solid > rbm on the geometry > convert to solid > merge faces.
Thank you for your suggestions - this ended up being the solution. I eventually solved the issue by importing the original mesh generated by COMSOL into SpaceClaim, then employing both the "Smooth" and "Reduce Faces" tools in tandem to simplify the geometry, before finally using SolidWORKS to turn the smoothed mesh into a solid body. This body retained many of the same features as the original, but was much less complex, having two orders of magnitude fewer faces. In turn, this permitted both meshing and heat transfer analysis in FLUENT.

Thanks again for your assistance,
Sam
Sam Marshall is offline   Reply With Quote

Reply

Tags
cfd, fluent, heat sink., meshing

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

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 Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[snappyHexMesh] Error snappyhexmesh - Multiple outside loops avinashjagdale OpenFOAM Meshing & Mesh Conversion 53 March 8, 2019 10:42
GenerateVolumeMesh Error - Surface Wrapper Self Interacting (?) AndreP STAR-CCM+ 10 August 2, 2018 08:48
snappyhexmesh remove blockmesh geometry philipp1 OpenFOAM Running, Solving & CFD 2 December 12, 2014 11:58
Moving mesh Niklas Wikstrom (Wikstrom) OpenFOAM Running, Solving & CFD 122 June 15, 2014 07:20
[Commercial meshers] fluentMeshToFoam multidomain mesh conversion problem Attesz OpenFOAM Meshing & Mesh Conversion 12 May 2, 2013 11:52


All times are GMT -4. The time now is 15:58.