Learning Forum

[Sam Ho]

Hi, I am trying to create a mesh of this model, however, it does not mesh and tells me that: "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." Hence, I went into Spaceclaim and fixed the geometrical errors, however it still won't mesh as shown in the figure below.

Hence, I split the body up and slowly combined them and seeing if they mesh. They meshed, and eventually, I reached a plane where I could no longer combine and generate a successful mesh. The picture below shows as far as I can go without an error.

I considered this being an error between the faces and I split the body at a different area, but it still meshes.

Therefore, basically, my model won't mesh as a full body, but it will mesh as separate bodies and it is not caused by the interface between the faces. Does anyone know why?

[Rahul Kumbhar]

If you right click on the mesh error and select option 'Show problematic geometry', does it highlight any face. Please check the geometry for any thin features which may be defeatured during meshing.

[Sam Ho]

Hi, Thank you for your reply.

How do I go to the show problematic geometry page? If I right click on Mesh, nothing like that appears. If I right click on the message, there isn't that option either. I can only get it to show the object, which is that entire body since I am trying to merge it into one body. Also, I've already used spaceclaim to check geometry and it told me no geometrical error.

[Sam Ho]

Also, can you explain the differences between bonded contact, shared topology and merging them into one body? I have been trying out these different set ups and they all yielded different deformation and stress results. In my case, my geometry is one big piece of structural steel welded together (50+ layers of weld) and can hence be assumed as one body/part, which one out of the above should I be using?

[Rahul Kumbhar]

Also in Spaceclaim, use check geometry to find any geometric issue.

[Rahul Kumbhar]

In Share topology, the common faces betweent wo bodies are merged into one. The bodies are separate but its face is shared. So when you generate the emsh, the nodes on the common face are shared between elements on two bodies.

The bonded contact, a contact is defined on two surafces of these two bodies. The nodes are not common. Additionally there are contact elements on both faces. Ideally you should get similar result using Shared topology and bonded contact.

Merrging bodies does not keep any common interface and thus it is continuous single volume with same material properties.

[Sam Ho]

Hi, thank you for your reply. Does that mean in order for the deformation and stresses to correctly pass through the geometry, I need to merge parts into one body? Also, what about a fixed connection? Would that allow stress and deformation to be passed through correctly?

[Rahul Kumbhar]

Both Share topology and bonded contact do very accurate load transfer through the interface. so the result should be same as single body.

[Rahul Kumbhar]

Do you have any thin faces or thin geoemtry section in thsi model? You may try changing the defeaturing tolerance under the details of Mesh. 

[Sam Ho]

Yes, there are thin faces and geometry but the interesting thing is that the frame at the front that doesn't allow me to mesh as one body anymore has identical geometry as the ones in the middle. Therefore, it's weird why it can mesh individually but won't mesh as a whole. Is there a limit to the size of a body or number of elements Ansys allows on a singular body? (Nothing regarding exceeding number of elements popped up though.) I have already tried turning defeaturing off and it still doesn't work.

[Rahul Kumbhar]

There is no limit. As indicated by the error, the faces may be intersecting in the thin region causing meshing error. If you are able to mesh by splitting then additionally use share topology or bonded contact. The result should be same as single body.

[Sam Ho]

I've lowered the mesh defeaturing tolerance and it works now. So apparently I have to lower it and not turn it off.

Do you mind if I ask why this is the case? (Is it because if the defeaturing is set to zero, then my model is too complex to mesh and if set to default, the tolerance is too large hence resulting in errors?)

All in all, Thank you very much for answering my questions! You were very helpful and I hope you have a great day.

[Rahul Kumbhar]

If you turn off defeature, then there could be very small features(not important for FEA) which mesher will try to mesh and may fail as the minimum size is larger than those features.

Also there can be situation where defeature tolerance is large such that it is defeaturing important features from mesh, which may also cause meshing issue.