February 22, 2018 at 1:43 pmSiva Pavan JosyulaSubscriber
I am facing problem when meshing my model in ANSYS workbech mechanical.
I was not able to obtain smooth transition of mesh even after assigning line division to obtain smooth mesh.
Here I have defined the line spacing and also as mappable face.
But the mesh which I obtained looks like this. with no smooth mesh transition in shell meshing.
in below picture we can easily depict the no transtion of mesh.
Can anyone help me with this problem?
February 22, 2018 at 1:54 pmpeteroznewmanSubscriber
If you create an Archive of your project, you can attach it to your post above using the Attach button if the file is < 120 MB.
Where did the geometry come from? It looks like it is in a multibody part, but some CAD interfaces (like NX) do not create shared topology like DesignModeler does.
February 22, 2018 at 1:59 pmraul.raghavSubscriber
Pavan, instead of defining the line spacing, can you try defining the number of divisions on the edges. Try to keep it consistent (same) for all the edges and see if that fixes the issue.
February 22, 2018 at 2:25 pmpeteroznewmanSubscriber
I see two vertex points in the image. One belongs to the grey surface and the other vertex belongs to the brown surface. In DesignModeler, you can split an edge. If you split the edge of the grey surface at the vertex on the brown surface, and split the edge of the brown surface at the vertex on the grey surface, you will have two matched edges (one long and one very short) and setting the number of divisions as Raul suggested on those two edges should force a congruent mesh.
February 22, 2018 at 2:43 pmSiva Pavan JosyulaSubscriber
I have imported from NX and its not a multibody part. my model is 3D wind turbine rotor blade.
In 3rd picture of my Post they are not vertices, but they are nodes and we can clearly see dissimilar mesh between two surfaces in same part. I would like have a amooth transition with the mesh sharing same nodes between two surfaces.
Is this due to bad geometry cleanup from ANSYS workbench
February 22, 2018 at 2:50 pmSiva Pavan JosyulaSubscriber
Hi Rahul, Line spacing and edge division is same and I have maintained line spacing consistantly.
My question is not how to mesh, rather if you see 3rd picture in my 1st post, I have highlighted the nodes where you can see dissimilar mesh which is very unsual having dissimilar mesh when two surfaces are sharing common line to a part.
My basic question is why I am getting different nummber of nodes common line shared between two surfaces to form a geometry?
February 22, 2018 at 2:56 pmpeteroznewmanSubscriber
I have a best practice for bringing geometry in from NX. After import, I immediately open the geometry in DesignModeler, then pick the part at the top of the tree and right click to Explode Part. There will be 10 Parts and 10 Bodies. Then pick the 10 Parts and Form New Part. There will be 1 Part and 10 Bodies. Now Refresh in Workbench to update the geometry in Meshing. The Shared Topology should now work as designed and create congruent meshes.
I do this Explode Part / Form New Part routine at the start of the model building phase since it will break the scoping after BCs have been applied to those bodies.
February 22, 2018 at 3:12 pmSiva Pavan JosyulaSubscriber
I followed the same process of forming a single part in Designmodeller after importing from NX for the case of geometry cleanup later I have created datums to slice bigger component to form smaller bodies for better meshing.
Please let me know, if you have any alternative Ideas on this problem.
February 22, 2018 at 3:21 pmpeteroznewmanSubscriber
Add one more slice through the center of the tube slicing all bodies in order to create matching vertex points on the circumference on adjacent edges.
February 22, 2018 at 11:22 pmraul.raghavSubscriber
Could you possibly upload the geometry file or the workbench archive file? It would be interesting to know why the shared topology is not working in your case.
February 23, 2018 at 12:02 ampeteroznewmanSubscriber
Recently, I added mesh controls and shared topology didn't work. If I deleted all mesh controls, then shared topology worked.
Do you get a congruent mesh if you delete all mesh controls?
I'm also interested to see the geometry. You can attach a zip file or a project archive .wbpz file if it is < 120 MB.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- ANSYS Workbench Measuring within Design
- How to resolve Mesh Failure
- check element type
- The mesh file exporter could not resolve cyclic dependencies in overlapping contact regions error
- Meshing Error
- Error in meshing
- Conformal vs Non-Conformal Mesh
- Ansys 19.0 – will not create mesh
- Dealing with inflation layers around sharp corners in Ansys workbench meshing
- execution error inside the mesher. The process suffered an unhandled exception or ran out of memory
© 2022 Copyright ANSYS, Inc. All rights reserved.