[zeophlite]

I have a reservoir with a pipe coming out of it. I'm using Automatic Inflation and Advanced Size Function. The walls of the reservoir and the pipe are set for inflation. The inflation layer along the wall and the pipe are correct, but they do not join correctly at the connection.

This is causing stairsteps, as well as a high skewness.

I've taken a screenshot of the options I have for meshing. What do I need to set for the boundary layers to connect around the bend?

[mjgraf]

in ICEM I would control that with
Min prism quality
Max prism angle
Max height over base

you may want to try setting "Maximum Angle" to 180.

[zeophlite]

Hi mjgraf,

Thank you for your quick reply. Is there a similar option in Ansys Meshing?

[mjgraf]

that's why I suggest
"you may want to try setting "Maximum Angle" to 180."

[zeophlite]

Hi mjgraf,

Cheers, I didn't realize you were talking about Ansys Meshing in your second paragraph - I'm quite new to this product, and most of those settings are just their defaults. I set Maximum Angle set to 180, and in a different area of the geometry that was also stairstep'd, the new mesh now has a correct boundary layer.

However, now the entire reservoir does not have its boundary layer (beforehand it did, just was stairstep'd at the outlet). The pipe and the reservoir are separate bodies in the same part. In the previously shown area, I get the attached mesh and the below errors:

• Inflation created stairstep mesh at some locations.
• Pre-inflation failed possibly because inflation thickness is larger than adjacent face height.

When I right click on the "Pre-inflation..." warning and select "Show Problematic Geometry", it selects just the right hand wall displayed in the attached image.

[mjgraf]

Didn't realize those were two bodies, assuming Ansys Meshing is primarily ICEM in the background.... you can not have that surface interface at that location you created and have the prism inflate off those two walls and into the internal surface interface. I ran into this before in ICEM and needed to move my internal surface or create one continuous domain/body.

searched my email from support back then:

You are extruding prisms from the two walls and also capturing the mesh on internal surfaces. This causes a constraint for the prism mesher. (If you do not have the int-wall, at the corner, prism can wrap around by splitting the angle. Capturing a internal wall there does not allow splitting the angle in that location)

hence the stair stepping.
so merge your two bodies into one or move that interface to the right some to create a nub on the reservoir. Not sure how your model is setup or how Ansys Meshing works. In ICEM, if these were two imported parts, I would just delete the surfaces at the interface and create a single body part, done.

[Kart379]

Please could someone help me, I am new to AM and I am not able to find where to change the maximum angle to 180 degrees. I too am having issues with stairstepping.

Thank You for your time.

[mjgraf]

Check your Ansys Meshing Users Guide.
It should be Global Mesh Controls > Inflation Group > View Advanced Options > Maximum Angle

[Kart379]

Thank you mjgraf for your quick reply.
The stair stepping error has been replaced by the "Pre-inflation failed possibly because inflation thickness is larger than adjacent face height" error as in the previous problem, but, I cannot understand how to apply your solution to my situation. I briefly describe my problem as below:

I am trying to simulate using sliding mesh, a Ducted wind turbine
The geometry consists of a stationary and a rotating fluid domain.
1. The duct is subtracted from the stationary domain whereas the turbine has been subtracted from the rotating domain. Both the tool bodies were not preserved.

2. The rotating domain is subtracted from the stationary domain but the tool body is preserved.

I have inserted contact sizing, face sizing, edge sizing and inflation operations on the turbine in the rotating domain. The inflation layer fails to generate at the radially outermost edges of the blades. Please help me solve this problem.

I deeply thank you for your patience and time

[mjgraf]

i have not seen that error in some time and going on memory here.
something with your sizing parameters is not correct. In ICEM some parameters need to be absolute and others are relative to the global size factor.
try only inflating 3 or 5 layers and then check/measure actual distances to help troubleshoot the situation.
This was a method I used to speed up meshing where I knew the thickness settings, only inflated 3 or 5 layers and then split those layers and redistributed. I rarely waited for 21+ layers to generate in ICEM.

[Kart379]

Thank You for your reply
I have tried making a finer mesh but it hasn't solved the problem. I did not understand this "then check/measure actual distances to help troubleshoot the situation". Please could you guide me to the right source to understand this concept?

Thank you for your time and effort

[n0t_sm0L]

I'm having the same issue as well. I'd like to inflate the bottom wall, as well as the wall of the cylinder, to accurately capture boundary layer effects. In the images I've uploaded, you can see that I can only either inflate the bottom wall or the cylinder wall, but not both. I' not using automatic inflation, as I've given a local inflation for each face, but when i try to run the whole thing, I get stair stepping, and it doesn't inflate the cylinder. I have to suppress one to inflate the other.
Please help me.
Thanks so much in advance

[kjetil]

Do you have a separate inflation for each face? I would combine most of them in as few inflation entities as possible, even though it shouldn't matter much.
Also, small general sizings on edges or faces can influence the inflation layers.

[n0t_sm0L]

Hi kjetil,

Thanks so much for your reply. I had 2 separate inflation instances, once for the bottom face, and one for the cylinder wall. The reason for this was so I can inflate the cylinder walls more. Turns out, I had forgotten to inflate the top surface of the cylinder, and had only included the curved surface. The issue was resolved for the single cylinder case. The first picture shows the cross section of 30 layers around the cylinder and 12 on the bottom face, for a single cylinder.

I wanted to replicate this for an array of cylinders placed side by side. Also, is 30 layers of inflation at a growth rate of 1.2 too many? I tried 15 layers of inflation on both this time, for the multiple cylinders case (2nd picture attached). Is this too few?

Thanks and regards

[kjetil]

This would depend on the purpose - the cells you show in the two images would have quite high aspect ratio, as they are very thin compared to height. And this is not generally a good thing. High boundary layer resolution might be necessary for some purposes, as with heat transfer or high resolution turbulence, but if this is not of concern then you might be happy with using wall functions and far fewer cells. This would lead to better aspect ratios as well.


Personally I seldom use more than 15 cells, even for heat transfer applications. 5-8 is perhaps a good starting point, and you would be able to inspect this in postprocessing if the absolute thickness is appropriate. As always you will find good recommendations here: https://www.cfd-online.com/Wiki/Ansys_FAQ

[n0t_sm0L]

Understood. My application is turbulence related. I'd like to capture vortex shedding. My end goal is to use cylindrical vortex generators on an Ahmed body (canonical body for an automobile), to see of the vortices energise the boundary layer to keep the flow attached to it, preventing delayed flow separation and possibly reducing pressure drag.
Regarding the aspect ratio, what would you recommend I do? Should I slice the geometry around the cylinders and provide a fine sizing only there?
Thanks, I will check out the link you sent.

[kjetil]

To lower the aspect ratio I would set a finer surface sizing on the object itself, reduce the global expansion factor, and lower the number of inflation layers from 30 to max 20. Finer surface resolution would also add spatial resolution, which you seem to be after. No need for additional slicing.

[kjetil]

If you want to study the drag, you might consider adding a Body of influence to have a finer volume region there in the wake of the body you study.

[n0t_sm0L]

Thanks so much for your prompt replies.
Okay, I will try this. I don't want to add an unnecessarily fine mesh in areas where nothing is going on. Hence, I made the domain smaller as well, and added symmetry boundary conditions at the walls along the length and at the top of the domain (for this analysis). But I guess, the refinement is unavoidable in places where I want to capture flow physics accurately.
What would you recommend as the best way to reduce the total number of cells I'm using? I understand that I'll have to do a grid independence to figure that out, but I meant more in terms of a mesh technique?
Right now, I'm using the patch conforming method, as you've seen. This is so that I can convert the mesh to polyhedra in fluent. This reduces the number of cells by a fair amount, is that correct?

[kjetil]

Well, if you are running this in Fluent, I would do the whole meshing in the watertight workflow there. But I wouldn't make this move only for the sake of getting "efficient polys". I think you would be better off with flow-aligned cells, which the poly-hexcore can get you (in Fluent), or some clever sweep meshing in Ansys meshing (but then you would have to do some nice cutting and shared topology, which I believe at this point would add too much complexity). But if you're interested, have a look at https://www.computationalfluiddynami...hing-in-ansys/


To have flow-aligned sweep-like cells in Ansys meshing, you might give Multizone a try, though I rarely use it. I rather make some body intersections and sweep those myself (apart from the innermost part in this case, which would not be suited for sweeping).


Bottom line: you could try multizone with hexcore in Ansys meshing, Fluent polys are not necessarily the way out (you get fewer cells, but many nodes -> need more memory in my experience). But Fluent poly-hexcore adds a flow-aligned structured mesh far from unstructured surfaces, which probably would be the best mesh in this case, though maybe a Body of influce also would be needed here.