Very Different Length Scales
 

In the moment I try to model a "Slot Die" (3D). The first problem I was faced with was the very different length scales. While the Inlet and the cavities have diameters of around 2mm, the "slot" has a width of 0.01mm, and the height of the "slot" is 20mm. I added a screenshot of the geometry. It is the first try and therefore very simple. To reduce the amount of cells I am using symmetrical boundary conditions in the middle of the domain. I am using ICEM CFD to generate the grid. For the reason of the very different length scales ICEM generates a mesh of around 50mio cells which is way too much to be solved. I am working on a machine offering 16 cores and 16GB of memory.
So what can I do? Split the domain? Is it possible to define the output from one calculation as input for another?
The other part of my question is about VOF. In the moment I am just interested in the internal flow within the "Slot Die". But when it comes to the outside I am not pretty sure what the meshing strategy would have to look like. Will I have to generate a cube around the "Slot Die" and mesh everything (internal and external), switch on the multiphase solver and VOF define an inlet and just watch the results? Do I have to define an outlet boundary?

I am very thankful for all your effort

Kind regards

Hi,

it is me again. Now I found out that it is possible to read hexa mesh into FLUENT.
But the problem I am now faced with is the transition zone between the inlet (tube) and the cavity. The cells within the tube are of curved shape. I tried to discretize the "slot" with hexas but by looking at the mesh using the scan plane tool I do see that in the region where the inlet (tube) merges with the "slot", cells in orthonormal direction have been created. This means that the scan plane is no longer plane. I attached some pictures of different scan planes in y-direction. As a result the quality of the grid is very bad and the "slot" is no longer perfectly discretized cause the cells do shrink and wrap.

Is there anyone who knows something that could fix that problem?


Any ideas would be very much appreciated.

Kind regards

Link Edges
 

Hey Philipp,

The problem is the very thin split under the pipe. The one set of edges is associated with the curve, but the edges very near to those is unassociated. Hexa uses interpolation to look after it.

However, I suggest using Link Edges to link the shape of the near edges to the curve associated edges.

This can be found under the blocking tab => Edit Edges => Link Edges.

Attachment 3326

I also added an Ogrid to improve the quality in the pipe. Since there was no need for the Ogrid to pass thru the entire model, I just had it go one block into the first Slot like this...

Attachment 3327

Attachment 3328

From here, you would still need to match edges, adjust edge params, etc for smooth transitions.

Simon

Images...
 

Not sure why the images failed... I will put them here.

Hi Simon,

the linking is clear but how exactly did you create the O-grid. Did you use the same splitting I used? Which blocks and surfaces did you include and how did you modify the O-grid afterwards? I am not familiar with defining O-grids. Including the blocks of the pipe, the block of the slot linked to the pipe, and the corresponding block of the cavity (not the entire cavity) results in an O-grid without any use regarding the improvement of grid quality.

Sincerely

Ogrid.
 

So there were three blocks in the pipe direction, the pipe, the thin sliver after the pipe and the almost wedge block below that.

I split the wedge block to create a 4th region.

Then to create the Ogrid, I selected the first three blocks (the pipe, the thin layer and the top half of the wedge block). I selected the end of the pipe as the only face. That's it.

This gave me an Ogrid that was aligned to the pipe walls, hand a nice inlet at the one end, but then turned around on its self (was self contained) on the wedge side with plenty of room for good mesh angles.

Hi Simon,

did you use some kind of index control? I think I was able to block it the same way you did. There are two more questions:
Do I have to link the edges before or after snapping the associated edges and which feature do I have to enable for displaying it like you did. To project the associated edges I turn on the "Projected Edge Shape" Option but that does not have any effect on the linked one. Does it make sence to move vertices in this case or is this just an issue of how ICEM displays it and in the end the information comes with the linking?
The second question is about bunching. Having two parallel curves; one associated to a single edge and the other to an edge which has been splitted into two edges, how am I possible to control the bunching to get a high quality grid. There should be the same amount of cells on both sides of the surface.

Thank you so much for your time.

Q&A...
 

yes, I used index control to keep the splits from going too far, but you don't really need to.

Yes, you must associate the edges with the curves and get that layer how you want it before linking to the next layer in...

Projected Edge shape works great for surface or 2D blocking because it doesn't require a premesh compute every time you make a change... but to see the edge curvature on internal edges, turn that off and turn on the option for "Projected Mesh Shape". This does ask you to update after every change, so you probably won't want to keep it on for long.

You can use the option to link bunching (so that one edge aligns with 2). There is a trick to it, so read the info in the help. Alternativly, you can just extend all your splits thru all the blocks (under Split => Extend Split). I recommend new users always let splits pass thru all the blocks (rather than limiting them with index control)

Hi Simon,

incredible how the grid quality did improve.:)

Thank you very much.

What kind of length ratio would you recommend for the cells throughout the slot. The actual cells are very long but very thin at the same time. The flow is expected to be fully laminar.

Refinement study...
 

You could call you solver support people and ask them about ideal ratios. Alternatively, you may need to do a grid refinement study to figure out your own question...

Basically, you would run a variety of ratios and plot the results. You will find that the solution converges as your aspect ratio is reduced. You can use the chart to pick the right compromise between element count and reduced aspect ratio. Of course, this info would be more valuable if you were planning to do a variety of similar models.

Dear Simon,

I do know about the necessity of a grid independence study but in fact I have not been able to perform one because of the lack of an appropriate o-grid which lead to an decrease of quality by refining the mesh. I am just asking because I read something about a tolerable ratio for laminar case of 100 and just wanted you to confirm. As you say it is solver dependent I will perform an independence study.

In a next step I want to model the environement, too. So that I can follow the fluid after leaving the slot by VOF.
What is the best way to proceed?
I am not sure how to mesh the environement and still separate it from the inside of the die.
Do I now have to model a wall thickness, re-block everything, and define three domains? Inside (fluid), die (solid), and environement (mixture fluid_1 and fluid_2)?
Or is it possible to use the existing blocking and just define a cube around it and build up a new mesh which does neglect the inside of the die, or is it finally much more clever to just model a cube with an inlet of the same shape and size as the previous outlet at the top, perform two separate calculations and transfer the data from one calculation to the other? Although I am not sure wether or not FLUENT (the solver I use at the moment) is able to do that. I mean to define one output as input for another calculation.

Hope you can help.

Thank you

But you can do a non-conformal interface with FLuent, or you could merge two blockings together... Or you could do the environemnt with Tetra and do a tetra/hexa merge.

I am not sure what shape your "environment" is or how it relates to the die. A picture would help me recommend the best approach.

Simon

Dear Simon,

I am not familiar with the method of non conformal interfaces. From what I have read it enables me to define several domains which must not necessarely have contact and FLUENT will eitherway transfer data, but it just remains the same calculation. I thought of a possibility to transfer the output of a calculation as input for a second calculation. But that way seems possible.
To clarify the problem did I add two scetches (Detail and Domain).
The environment I want to define is very simple. I just want to position the die close to a moving wall so that I can track the resulting filmthickness (see figure Simon_Domain). The die should be surrounded by ambient pressure. I am not sure how to realize that one. Is it superior to define far field conditions and all the other bocos within ICEM or should I do that within FLUENT? How far away from the die would you define the bocos and what kind of bocos are needed (e.g. pressure outlet?)?
In all my naivety I would build a cube structure around the entire die, but I also thought of the possibility to just mesh the lower part of the cube (to reduce total amount of cells) which could be possible because of the much higher density of the fluid which leaves the die compared to the surrounding fluid.

I hope I was able to explain. Please excuse any kind of confusion.

Just block it again...
 

Looking at your model, I think the easiest way to get a mesh would be to simply start over and block it again with your far field. The simple box far field doesn't really add much complexity to the blocking (but it will take a little more time), so it is worth it to gain the accuracy of conformal hexa mesh.

In ICEM CFD, you can put certain blocks (such as your solid portions) into Vorfn (deleted) or you could put them into a solid material if you were planning any calculations in those regions. It is pretty easy.

As for the size of the "environment", it could be a complete box, but I think it would also work well as just the bottom half or bottom third of the box (which would reduce your mesh size and blocking hassle a little bit).

I am pretty confident that you can get this mesh beautiful (and I will help as needed). But I have never actually run a problem like this before. Perhaps you could leave the meshing details out and just ask the physics question (bocos and other setup) on the solver forum.

Dear Simon,

thank you very much for your advice. I gonna try to re-block the entire structure. I think this will be more difficult because I will have to model a defined wall thickness. I will give it a try. But due to the guidance you gave me, the resulting grid should become as good as the former one.
In case I just want to model the lower part of the environment, do I have to build faces just of that size? Do I need faces to create a far field, or would I define a block much bigger than the die (not sure how to, just used the blocking function to create a block which does include the die), start splitting from there, and do not associate and snap the most outer edges?

Regarding the questions dealing with the solver I hope I will find another advisor who will guide me with the same patience and competence.


Sincerely

Not a problem.
 

It won't be a problem... Just get a new geometry or use the ICEM CFD tools to create a box around the lower portion of your previous geometry. The splitting works the same way, but you create a few extra splits for the inside and outside of the solid portions.

Association works the same way also, except that you have more edges to associate to more curves.

The key difference is just that you have to delete those blocks within the solid (or put them in a SOLID part)...

Simon

Thank you.
In case of conjugate heat transfer calculation I would mesh the solid part too, right?

Right.
 

Right, you block it the same way, but instead of deleting blocks for the solid region, you just put them into a solid material. You will get a conformal mesh with all the solid and fluid regions...

I think I will keep the blocking for the internal region. Is it possible to coarse the mesh throughout the far field? I do know that I can cause a coarsening with increasing distance, but the number of cells I define at the edges of the die will cause a high nuber of cells throughout the domain. Would you recommend to combine hexa and tetra mesh. Is it possible to combine tetra and hexa in a way to get hexa also around the outlet and tetra for the far field where I won't expect any great gradients?

Hi Simon,

I now want to block the environment too. I want to do it seperately. I want to use the outlet condition as inlet. Therefore I would prefer to use exactly the same grid for the inlet (former outlet). But due to the blocking it is not that simple. You told me I may match vertices. But this time I do have two different projects. Would you recommend, or is it even possible to start the old project and block the environment there. and then use the match edges feature and finally delete the old geometry? I used that match edges feature to determine the bunching at the splitted edge so that it will show the same bunching as the respective none splitted edge but despite that the bunchings are not exactly identical (regarding the spacings and stretch factors). I could also use non conformal calculation but is it that exact? The solver will have to interpolate.

Thank you in advance.

Sincerely

Options...
 

Sorry, I missed your post from May 25th. Certainly it is possible to combine Hexa and tetra mesh... There is a tutorial about it (HVAC tutorial), and there are several more slides about it in the Tips and tricks presentation (I have posted the link on CFD Online a number of times, but don't recall it right now).

If you now want to hexa mesh the Far field, you can block it separately and then load both blockings at once (with all the geometry so the blocking has something to associate with). Then you can merge the two blocking files into one file (using the topology branch of the blocking tree), and then you can merge verts at the interface to sew the blocking together. Since you must merge vert with vert, you need a 1 to 1 correspondence that demands the same topology on both sides, at least for the interface. I think I covered this in the tips and tricks also, but if not, let me know and I can post some slides about it.

The downside to merging is that your index control gets really mixed up. It is workable, but awkward.

As I said before, for this model, it really wouldn't be difficult to just block the inside and outside all at once, but you have options.

Dear Simon,

I think blocking all at once will be possible but in the end I do not want to have the complete geometry within the same case file because this will result in too many cells. I would like to seperate both problems. The flow within the die and the flow at the outside of the die. Therefore I am now trying to setup a grid for the outside but I need exactly the same meshing at the face which do combine both parts because I think FLUENT does store the information at the center of the cell. Now I do have a split which passes through the entire domain because of the inlet. I could try to reblock the die and use index control to not let the split pass until the outlet and then use the match edges feature. But in that case I would have to mesh anything a second time and also the solver has to re-calculate. Therefore I am asking wether it is possible to add geometrical parts match blocking and then delete the old blocking. As I tried I was ask to merge and that resulted in a loss of the bunching information. Would you recommend to remesh the die so that I get a non splitted outlet block?
Or do you know that FLUENT is able to transfer that data neglecting the blocking?

Sincerely

Lots of options.
 

You have lots of options... I am pretty sure you can map the output from the first case as an input to the second via interpolation that doesn't require the same mesh... Fluent is really good at that actually. Look up load mapping or ask on the Fluent Users Forum.

You could also block the entire model at once, but put the two halves in different volumes and output the volumes separately to Fluent.

You could merge the two blockings to make sure the faces matched, but then only output one of the volumes at a time...

If you know your topology at the interface (Ogrid or what ever), you could create some curves and points and associate each side separately to those geometry entities (like construction geometry)... Then make sure you have the same mesh distributions, etc. and you don't ever need to load both blockings to ensure that things will match... For example, if you created points where all the verts were on blocking A, then you could just copy those same interface points to Geometry B and associate blocking B with them... (to copy geometry between tetin files, Just turn off the other parts and File => Save Geometry => Only Visible. Then load the Geometry B tetin file (replace Geometry A) and then load/merge this Visible portion of Geometry A.)

Dear Simon,

these are really lots of options. I think I will first try to use FLUENT to interpolate. I will report the experience I gonna make.

Thank you very much.

Hi everyone, Hi Simon,

I do have another problem..

Did change the configuration of the geometry. Now I have the problem that at a certain point two curves meet tangentially. There I do have just one edge but two curves. I tried to associate both curves with the single edge but that did not work out very well. I attached a picture of the situation. Do I have to change the model? But it can't be possible to adabt the geometry on ICEM. Is there a possibility to block that thing shown in the picture?

I am happy for any advice

Wedges?
 

How do you feel about wedges?

I would block that with an Ogrid thru the cylinder and thru the block, then add wedges for the corners of the blocks. You would get prisms (Penta-6) elements in the cusp areas.

You would probably find that quality improves a little if your mesh jumps off the circle as it nears the wall, at least for the last element or so... You don't need to change the geometry, but maybe plan your geometry so that the opposite wedges (on either side of the cusp) don't actually meet, but rather have a couple extra splits thru the cylinder to keep them on either side of the theoretical meeting point.

I would block it out for you, but I am really swamped this week.

Simon

Thank you so much Simon..

Think wedges would be great but I am not sure how to apply. So far I just cut orthogonal to existing edges. I do start with a cube surrounding the entire model (3D bounding Box). Is it possible to just cut a wedge from an existing cube? If so, how would I allow ICEM to allow prisms?
To apply the O-Grid you have in mind, would I just need to create a 3D bounding box, block and from there choose the blocks and faces? Or would I first have to cut the wedges? Would you cut the main block where the cylinder and the cube meet? What is with the possible edges that will be created by that action. Would you associate those to the curves of the cylinder or to the curves of the cube?
How would I allow the mesh to jump near the wall?

Thank you so much in advance..

What do I have to do in case penetrating elements do appear where everything looks fine to me? May I neglect?

And a problem I do have with the settings. ICEM is running on several Computers. Every installation except of mine does allow by associating vertices and edges to neglect the apply button. What is wrong with my settings. I really enjoy that the association is accepted by chosing the respective point. Hope you understand.. Just want to chose vertice and point and go on with the next point without the need to apply..

Sincerely..

hi everybody
 

I really need ur advice on this
I am try to model scour under pipelines lying on a seabed using FLUENT
I intend to use eulerian multiphase model which requires me to create two zones(water and soil).
I have used projection to split a surface into two under Design modeller to create the two faces.
The issue i have is that when i try to mesh the surrounding of the cylinder, the mesher; the mesh under the pipe is scattered because of the projection line that is there.
I have attached the picture of the mesh i got
pls i will appreciate any contribution