Dealing with inflation layers around sharp corners in Ansys workbench meshing

  • 2.9K Views
  • Last Post 15 October 2018
  • Topic Is Solved
jamesgr posted this 16 July 2018

Hello everyone!

I am trying to create a sufficiently good mesh of a full centrifugal pump with a semi-open impeller design in order to determine performance characteristics such as pump head, efficiency and cavitation characteristics. I have already created the volute, clearance domain, inlet and outlet pipes using ICEM. However the impeller domain will need to fairly automatic as it will be used for design optimisation, and so I thought Ansys meshing workbench might give me a more automatic routine for this portion (also I had trouble in ICEM capturing edges between faces for this geometry using the Octree method).

Using just the automatic method with resolution settings set to fine and a proximity and curvature size function, as well as face sizing at the trailing edges and inflation layers on the impeller walls, gave me the following mesh.

In general, this mesh qualitatively looks to be of sufficient quality, however I am having a number of troubles around the trailing edge inflation layer.

This is quite the trouble area as the inflation layer consistently has a number of skewed faces in this region due to the shape of the corner here.

I have attempted to change a number of inflation parameters in order to create better elements around this corner to not much avail. The most recent iteration of these parameters are as follows:

Due to the sharp corner here, I wonder if my best bet wouldn't be to either use an internal wall or to project the surface mesh of the trailing edge back to the edge of the domain, however I'm not entirely sure how to do this in Ansys meshing workbench. Also both of these methods would require a significant amount of user input, whereas I would like the process to be as automated as possible for a design optimisation routine.

Does anyone have any advice on how I can proceed with this?

James

Order By: Standard | Newest | Votes
peteroznewman posted this 15 October 2018

Hi Catia,

Try slicing on the plane shown by this yellow line that passes through the tip.
That should create similar geometry like what you have on the stinger.

In the future, please create a New Discussion if the old discussion is marked as solved.
You can include a link to the old discussion.

Regards,
Peter

CatiaV5 posted this 15 October 2018

Hi Peter,

I was wondering what advice you could give me for slicing a delta wing with sting attachment as shown in the picture below. Currently I am not able to generate a mesh around it. I have sliced it already at the tip, but I'm still not getting inflation layers around it. I was wondering if you had any advice please?

jamesgr posted this 20 July 2018

Hi Peter,

OK, no problem. Hopefully someone with a little more experience will chime in with some suggestions.

Thank you again for all your help!

Regards,

James

peteroznewman posted this 19 July 2018

Hello James,

I'm really a structural kind of guy, and have only played around with a few CFD models, but I am fairly good at geometry and ANSYS meshing. Never used ICEM or CFX so I hope an expert in those areas can comment as I am out of my depth here.  Good luck!

Cheers,

Peter

P.S. yes, I live in the USA now.

jamesgr posted this 19 July 2018

 Hello again Peter,

I am also having difficulty with the named selections. Namely, they are not showing up in either ICEM or in CFX-Pre, although I have set all of them to send to solver. I am sure I'm just forgetting something, but would you be able to have a look to see if they show up for you?

Thank you again for all of your help, I appreciate it.

Regards,

James

  • Liked by
  • shazimy
jamesgr posted this 19 July 2018

Hey Peter,

I'm no CFD expert either, but my feeling is that considering I am largely interested in performance prediction and not secondary flow features, this small defeaturing should not be a problem. However, that may not be the case for the defeaturing of the sharp blade edge, but I guess I will find out later.

Using the above approach, I think I have managed to get a decent looking mesh, although I had to smooth it a little in ICEM to get decent quality in a small number of the cells. I will say the only seriously negative reports I receive while performing a mesh report in ICEM is the following:

49  problems  were found for delaunay

2240  problems  were found for 3_surface_node_internal_faces

I am not exactly sure what this means, nor if this will make a major effect on my convergence. I have included the archived project file, if you have the time to have a look, I would appreciate it if you could have a quick look at the elements and quality statistics to see if there are some major problems I am missing.

Regards,

James

P.S. Haha I suppose you're located state-side? I am based in the UK in Cambridge.

Attached Files

peteroznewman posted this 18 July 2018

Hello James,

I reckon this is a good approach, since you want to have a parameterized model, but I'm not a CFD expert, so I would be interested to hear any other opinions.  

Regards,

Peter

P.S. I haven't heard the word reckon used much since I left Australia many years ago. Where in the world are you?

jamesgr posted this 18 July 2018

Hello again Peter,

I have been mulling over the problem quite a bit, and I cannot seem to come up with a way to model that sharp TE using a parametrisable surface that splits the body into two.

However, I did manage to get what seems to be a serviceable mesh by rounding that edge such that the inflation layer can wrap around it. This is more of a workaround rather than a real solution, but seeing as I can't seem to make anything else work, it might just have to do.

I used the proximity and curvature sizing function in order to capture this new rounded face, and so in order to more accurately capture a good transition in the boundary layer, I set the sizing to be quite small along the blade. I'm still not completely happy with the boundary layer at that corner, but I think it is improved.

Do you reckon this is a good approach to solve my problem for the time-being?

Regards,

James

 

jamesgr posted this 18 July 2018

Hi Peter,

I am also having a very difficult time considering how this may be parametrically done, especially considering the shape of the blades and hub may significantly change during the parametrisation process. Do you have any other suggestions as to what I can do get better elements at the TE?

As for the manufacturability, in all honesty, I am currently unaware of how this pump has been manufactured. I can say that the impeller geometry I have sent you, although not an exact replica of the original impeller, is a very close fit.

As a reference, the given impeller looks like this:

The original impeller contained some features that were very difficult to capture during meshing, and so what I have done is use my parametrisation method and a shape matching optimisation algorithm to obtain a close approximation to the original impeller, removing the problem features. Supposedly if my fitting was sufficiently accurate, the geometry I gave you would have the same draft angle as the given geometry.

Regards,

James

 

 

peteroznewman posted this 18 July 2018

Hi James,

I used my NX11 CAD system to create a surface, but it is not able to slice the solid. This is some challenging geometry!  I don't think it will be "easily" parameterised in DesignModeler. I can't say it's impossible, but it may require enormous effort.

 

MANUFACTURABILITY
I thought about how the impeller part could be made, as I know many impellers like this come out of a mold. But designing a part for molding has a geometric requirement on all the faces of the part; they must have a positive draft angle so the part can be pulled from the mold. Your impeller geometry has negative draft angles. In other words, there is an undercut surface that prevents the impeller from being pulled out of a mold.

If the part is made by a six-axis milling machine, your shape can be cut from a block, or it could be 3D printed, but if you want it to be molded, then you must use a positive draft angle on all the faces. Positive draft angles can reduce cost as they make it possible to cut the part on a 3-axis milling machine.

Regards,

Peter

jamesgr posted this 17 July 2018

Hi Peter,

Great! Thank you again for taking the time to help me.

As for the bisection surface, I am having a little difficulty developing a method that can parametrically be used for other geometries. This is the closest I've gotten:

However, I suspect this is less than ideal for use in Ansys meshing (particularly due to the sharp corner created at the intersection of the end of the bisection surface and the pressure side of the TE).

Given an input of one of the three previous formats, can the surface be easily parametrised in either Ansys meshing or Design Modeller?

Regards,

James

peteroznewman posted this 17 July 2018

Hi James, I'm sure one of those is fine.

I will reply once I have something.

Regards,

Peter

 

jamesgr posted this 17 July 2018

Hi Peter,

I see what you mean. I can attempt to create the bisection surface in my CAD parametrisation, but I will need some time to think about how to do this in a parametric way such that the same may be done for a number of geometries without loss of generality.

Unfortunately, I am not using a Parasolid based CAD software and it seems I cannot generate an x_t file. I am using FreeCAD which uses the OCE kernel and therefore the native format is BREP, however I can also use STEP or IGES formats. I have included all three of these formats.

If none of these are sufficient, I can also send the Python script I am using to create the geometry, however that needs the FreeCAD library to compile and I'm afraid the code is pretty spaghetti-like at the moment, and so may be difficult to decipher. However, if there is anything else I can do to make it easier for you, please let me know.

Regards,

James

Attached Files

peteroznewman posted this 17 July 2018

Hi James,

You want the bisection surface that begins at the TE to continue to another wall surface so that the solid body that defines the fluid volume can be split into two or more solid bodies.

When multiple solid bodies exist in a single Component (SpaceClaim) or Part (DesignModeler), Shared Topology is used by the mesher to have shared nodes on the coincident face that connects the two bodies back into a single mesh, and this is what allows for better element shapes in the fluid off the TE.

I opened your attachment, but is is a collection of surfaces and no solid bodies. Could you attach a solid model of the fluid volume from the CAD system in a Parasolid file format (put it in a zip archive to attach). 

Regards,

Peter

jamesgr posted this 17 July 2018

Hi Peter,

First of all, thank you for taking the time to help me. It's greatly appreciated. Also thank you for the offer to attempt this on my geometry, however I will need to automate this process for a large number of geometries and so I really need to be fully aware of how to do this myself. However it may help you understand my question if you can see my case study, so I have included it in this post.

I thought it would be significantly easier to do this in the CAD than in the meshing workbench, as I will need this whole process to be as simple as possible for automation. So I went back to the CAD to create an internal wall that bisects the TE at both the hub and tip.

As you can see the blade TE is at an angle so the internal wall is at an angle, hopefully that won't make too much of a difference. Note the impeller sits within a rotating fluid domain, which has a slightly larger radius and depth than the impeller and looks like this.

Do I need to extend this surface all the way back to the fluid domain boundary, or is it possible to use this partially extended surface as an internal wall?

Also, may I ask what you mean by splitting the solid using this surface?

Thank you again for your advice and help!

Regards,

James

 

 

Attached Files

peteroznewman posted this 16 July 2018

Hello James,

My advice is to create a surface that bisects the two faces of the trailing edge and split the solid using that surface. That way, each side of the flow can be meshed in a clean way as it leaves the trailing edge. See this post for an example. I have done this in both 2D and 3D models.

Attach a Workbench Project Archive .wbpz file to your post if you would like me to attempt that on your geometry.

Regards,

Peter

Close