Learning Forum

[19251758]

Without fillet as in the high stress edges in defected pipeline above, the accuracy of the simulation is low. On adding fillet to mitigate the high stress edges/ sigularuty effect I struggle to get a hexahedral mesh, please I need the steps to achieve that.

Kind regards

Martin

[peteroznewman]

In SpaceClaim, split the body into solids that are easily hex meshed and a solid that has the fillet.  On the Workbench tab, use the Share button to keep the mesh connected across the bodies by sharing nodes on the split faces.  In Mechanical, right click on the bodies to be hex meshed and mesh those first.  Mesh the fillet body last with tet elements.

[19251758]

Thank you kindly Peter for the modeling suggestion. With the 5mm fillet, I have 1/4 defected pipe divided into sweepable parts. I do not know why I am still having error messages in trying to hexa mesh this. Please I still need your help.

 

Kind regards

Martin

 

[peteroznewman]

Upload your .scdoc file to a file sharing site and reply with the link.  If using Google Drive, make sure to Share so that Anyone with the Link can download it and not leave it at the default Restricted share setting which means no one with the Link can download it without first getting permission from you.

[19251758]

https://drive.google.com/file/d/1o8RwyJa7Ill1Da0T_qcmtkUjlELuxa27/view?usp=sharing

[19251758]

Good morning Peter,

Please find the link to the quarter pipe in Ansys spaceclaim above.

Kind regards

Martin

[peteroznewman]

I don’t have access to 2024 R1, so I have meshed this in 2025 R1.  Notice how I have used parallel planes 5 mm on either side of the fillet.

A finer mesh can be put on the fillet, by using twice as many elements through the thickness of the rest of the body.

To put a finer mesh on the fillet add face sizing to the fillet. Selective order of meshing can sometimes create more hex elements on the extruded shape.

Adding a Hex Dominant Method to the fillet block.

[19251758]

Good morning Peter,

Thank you kindly for solving this problem that has been a challenge, I will carefully follow the steps you explained and try to achieve the same result. But please could you save the file in a lower version (2024 R1) and share the link.

Kind regards

Martin

 

[19251758]

Otherwise I can download the student version of 2025 R1.

Kind regards

[19251758]

Good afternoon Peter,

I have done some meshing but still trying to improve the accuracy, please see below. When I applied refinment at the fillet, the removes the entire hex mesh.

Kind regards

[peteroznewman]

Hello Martin,

Ansys can’t save projects as older versions of the program. Here is a link to the Ansys 2025 R1 archive. https://jumpshare.com/v/CoTzIWqIgxwkPIYAr4Mx

You will see that I use Edge Sizing mesh controls to force the mesh to stay aligned by choosing the Hard option and selecting all the edges that I want to stay aligned. 

Though more hex elements are created at the surface using the Hex Dominant method on the fillet corner solid, there are some skinny elements below the surface that allow hex elements at the surface.

Regards,
Peter

[19251758]

Good afternoon Sir,

Please I have been working on this particular model to improve the mesh element quality yet it appears the meshing has not improved whenever I check in the mesh metric, please I need some help.

 

[19251758]

Good afternoon Sir,

After splitting the interacting defected pipeline, most of the solid parts were sweepable apart from 2 parts.

I do not understand why I am getting poor quality mesh. Please find the pipe attached here-in. 

https://drive.google.com/file/d/148jbore67vbSY1mCLOLdwUfgiDDe7I7Y/view?usp=sharing

https://drive.google.com/file/d/148jbore67vbSY1mCLOLdwUfgiDDe7I7Y/view?usp=sharing

Kind regards

Martin

[peteroznewman]

Hello Martin,

You should show where the poor quality elements are using the Mesh Metric function.

A plane used to split the solid created sliver faces which can lead to poor element quality.

Some mitigation can be done in Mechanical by inserting Virtual Topology to merge those faces, however, VT caused the gray body that was originally sweepable to become not sweepable.

I recommend you go back to SpaceClaim and more carefully create planes to split the solid such that no sliver faces are created. After I Combined some solids into one body and used a more precise horizontal split plane, when I tried to reuse a vertical split plane, new inaccurate faces were created as can be seen in the image below.

My suggestion is that you locate the split plane a short distance away from a blend edge. Don’t locate a split plane coincident with a blend edge.

[19251758]

Good afternoon Sir,

Thank you kindly for all your response, I am grateful. I have placed the split plane away from the blend edges as adviced, please find the link attached here in.13 sweepable bodies out of 15 solid parts were confirmed. At the Ansys mechanical, after setting the symmetric region, I right clicked on mesh, pressed the mesh start record button and started generating hex mesh for all the sweepable parts, element size for areas away from the defect were made coarse. At the defect area, I made use of edge sizing to achieve the needed element size.

I am still having issues with my meshing, please can I get your advise on the steps to complete the meshing with good element quality. The meshing I did, the element quality was poor, mostly less than 0.2.

Kind regards

Martin                                                       

https://drive.google.com/file/d/1G6-FhNpD8qZCoEZHOQe7FBfvU_aau0gt/view?usp=sharing

 

[19251758]

I received the following warning;

Some of the elements on the problematic bodies can't meet the specified target metrics. Please check the elements and try changing the mesh size settings to achieve the needed mesh quality.

The surface mesh is intersecting or close to intersecting, making it difficult to create a volume mesh. Please adjust the mesh size or adjust the geometry to fix the problem.

Kind regards

Martin

[peteroznewman]

Hello Martin,

I am using Ansys 2025 R2 so you may or may not see exactly the same in Ansys 2024 R1.  Below is what I see in Mechanical when I open the Aug-04-2025.scdoc file.

Notice that the Show Vertices and Close Vertices are turned on in the Display ribbon.

The close vertices are highlighted in yellow.  This is feedback to you that the geometry is not clean.  You should not have any close vertices. However, the mesher is often clever enough to ignore them.

In Ansys 2025 R2, there is a Mesh Quality Worksheet. I wouldn’t pay attention to the red bar with the Minimum Element Edge Length.  That is not the cause of any poor element quality.
The warning limit for Max Skewness is 0.9 and this mesh has a Max value of 0.99892.  Elements over 0.9 are highlighted here:

Zooming in you can see that the tet elements in the corner are the problem.

You have a 5 mm setback from the blend to the plane to slice out the sweepable part.  If you increase that to 15 mm, you might leave sufficient space to allow the elements to mesh with better quality.

A good approach here would be to use just 2 planes to cut the slot out for Tet meshing with an element size of 4.5 mm on that solid, while the other three hex meshed solids have a Body sizing of 9 mm. These values ensure that 2 quadratic elements are across every section of the model, which is the minimum recommended number.  Bonded contact keeps the two cut faces on the slot solid bonded to the other two solids.

In SpaceClaim, hide the slot solid and use the Share button to keep the mesh connected on the three bodies with the Hex mesh so you don't need Bonded contact on those faces.