How to subtract solid from fluid region ICEMCFD
 

Dear Members,

I have a Impeller , rotar and the blades joined together. I would like to substract the solid part of the geometry from the fluid region in ICEMCFD.

I am not sure how to carry out the boolean operation in ICEMCFD.

Thanks in advance
Sesan

Booleans are unnessary...
 

ICEM CFD is not a solids based modeler (it is surface based). Therefore, Booleans are not necessary.

Instead, go to the geometry tab and "create body", then choose the material point option (from 2 points).

Type in "FLUID" as the Material name and then select two locations on the model such that the mid point will be in the fluid...

Similarly, create a second material point named "SOLID", and select its two locations so that the mid point will be in the solid...

Flood fill will take care of the rest for Tetra/Prism...

For Hexa blocking, you select which volume material the blocks are in... but it still helps to have these material points.

If you skip this step and just mesh the model without material points, it will just create them on its own with names like CREATEDMATERIAL1, etc. I usually create them.

Best regards,

Simon

Hi Simon,

Thanks for the reply. Would also like to know if i can do in Icemcfd Unite,subtract operations like in Gambit.

Since i am looking to subtract the solid from the fluid region and then mesh the fluid region. Like flow around the car. Will it be possible in icem.

Thanks
Sesan

Don't need to do that stuff.
 

Again, ICEM CFD is not a solid modeler and does not need to do any of these operations...

For subtract, you put different Material points in each region.

For Unite, you put the same material points in each region.

It doesn't really unite or subtract anything, but the end result will be the same as if you did.

Side note: If you want to maintain surface elements (internal wall) between volume regions in the same material, you must turn on the internal walls check box on that part (under Params by Parts).

ICEM CFD is very different from Gambit... You need to realize these fundamental differences and advantages or you will be frustrated trying to reproduce the same processes as you used in Gambit... However, if you are willing to change your approach, we can give you the mesh you want.

Sorry, mis click.

Hello Simon!

I suppose. I have the same problem. I'm new in ICEM and in fact I have no experience with Gambit. I'm trying to make task with rotation in OpenFOAM using MRFsimpleFoam. I've found small tutorial for GAMBIT (http://openfoamwiki.net/index.php/MRFSimpleFoam) and now trying to make it in ICEM. I'm very thankful for your previous posts the really added much understanding in differences, but I still need some advice.

Going step by step:
1.generate two cylinders (r1=0.5 h1=1; r2=0.25, h2=0.5) and one cube (h3=0.3)
2.subtract cylinder 2 from 1 (maintain cylinder 2)
3.subtract cube 3 from cylinder

Till that moment there is no any problems. As I understand I need just to make 3 parts in ICEM.

4. Connect the faces (inner face of cylinder 1 and outer face of cylinder 2)

To do that I need to make 3 material points one as solid in cube and two in cylinders as fluid.

5. define continuum types (zones): rotor for cylinder 2, and stator for cylinder

As I understand you I need to mark intwall checkbox in part mesh parameters. Am I right?

6.define boundaries (inlet, outlet, cubeWall, cylindricWall, sliderFace).sliderFace is the connected faces mentioned above.
7.define the boundary for sliderFace as INTERIOR

At this two steps I misunderstanding. Inlet,outlet, walls it's not problem I knew how to do that, but everything connected with sliderFace, boundary between two cylinders, is a mystery. I suppose that it needed not to have a small cylinder as part, but to have some additinal boundary. But I don't know how to do that. Can you show the way?

Best regards,
Andrey

Solver forum...
 

Andrey,

You only need to mark parts as internal wall if the volumes on both sides are the same material, but you want to keep the shell elements. By default (if you don't mark as internal wall) it will remove shell elements if the volume material on both sides is the same.

I am not quite clear on what your model looks like, but generally speaking, you could just put the sliding interface surfaces into a Part (perhaps named "SLIDING_INTERFACE") and then set it up in in FLUENT...

Beyond that, I suggest asking this question under the solver forum (I am not a huge Fluent expert), or look up how to do it in a Fluent tutorial...

I am having a similar problem and also having trouble following Simon's explanation. For simplicity, I'm trying to model the 2D heat transfer through a square aluminum block with a circular hole in the center. I'm having trouble creating a mesh because I don't know how to exclude the circular region from the rectangular aluminum domain in ICEM. All geometry (points and edges) were created in ICEM.

Thanks for your help.

Normal Vector... Hexa or Tetra? Assuming Hexa and assuming you have blocked the plate and it has thickenss, you just need to place the blocks into the correct part. Do this by right clicking on the volume part => Add to Part => Add Blocking Material.

If it is a zero thickness baffle, then all you need to do in hexa is work with the associations => Face to Surface. Assign the face to the surface and the shells (internal wall) will be created.

If this doesn't help, please include an image so I can understand the issue.

I've attached what I'm working with. I'm trying to mesh the grey part using a 2D, zero-thickness tetra mesh to use in FLUENT. In Gambit I would just create the rectangular and circular surfaces and then use the boolean subtract to leave the rectangular surface with a circular hole cut out of the center. As you've said, ICEM is completely different from Gambit and I'd like to transfer that procedure into ICEM but I've had no luck. Does my problem require blocking?

Thanks for your time.

Simple surface based paradigm.
 

So it is just a surface with a hole in it... You just want a 2D triangle mesh?

No problem.

If the grey part is a surface, just mesh it. If there is a surface for the circle in the middle, just delete it (or don't select it to be meshed). It is a surface based mesher, there is no need for booleans.

ICEM CFD has several meshers that could get it done for you.

If you use patch dependent surface meshing, then you will need to make sure that you run Geometry => Repair => Build Diagnostic Topology. This tool makes sure that each surface is bounded by "attached" curves. You will need to set the sizes on these curves (or the overall parts). The Patch dependent mesher starts from "loops" that get their sizes from these curves and then pave across the surfaces using a recursive loop algorithm. If you want prism, do a search for instructions regarding BLAYER2D.

If you are going to use Patch Independent surface mesh, you just set up sizes on surfaces and curves and hit mesh. It is not as picky about attachment or gaps or anything like that. You can look up more about this algorithm in the help.

Either way should be pretty easy.

ICEM CFD Hexa would also be nice and not hard to block either. But you should probably try a tutorial or two first.

Best regards,

Simon

Yeah that's basically it, I'm not working with too complicated geometry. Perhaps I should have mentioned that I'm creating this geometry inside of ICEM from points, curves and then surfaces. My problem is getting a surface in the shape of the grey region. When I choose to create a surface from the four outer square edges and the circle, ICEM disregards the circle and just creates a square surface with no hole in the middle.

Meshing makes more sense now... so an edge mesh is necessary?

Oh, so you don't yet have what you showed me. Instead, you have a square surface with a circle drawn on it...

There are several ways to cut the square with the circle.

The most obvious is "Create/modify surface => Segement surface => by curve". Then delete the surface inside the circle.

But most users just run build topology. It will automatically sort out issues like this and segment the surfaces while it builds up the connectivity. Then you just come back and delete the circle if you don't want it.

Simon

Thank you, that worked perfectly. While I still have you here, I have another question. I saw on another one of your posts about mesh growth control that you mentioned using the mesh params by parts tab. Will I use that for my 2D case? I want to recreate something like the attached; small elements at the wall and larger elements in the center. I want to do an edge mesh size of, let's say, 0.08 on the surrounding edges and I want it to grow to a size of 0.5 at the interior with a growth ratio of 1.2. Is that growth controlled by "mesh params by parts"?

Hi Simon. As you mentioned to created materia points, I just want to know how does ICEM determine which part belong to the body you set? Let's you create a CAR solid from two points around a car, and the car is divided into many parts ,then which zone belongs to the CAR solid?

I also had a question about material points. Should it be created before or after the mesh? Also how does ICEM know what to take as one body... is it determined on a surface basis?

Floodfill explained (briefly)
 

Material assignment is done by a concept called "Flood fill". You should place the material point before mesh generation because Flood fill is part of the octree process, but you can also place a material point later and run flood fill manually from the "Edit Mesh => Repair" DEZ.

I am sure I have described this in detail before, so just do a search for "Material Point" or "FloodFill" for that.

The short version is that it locates the material point and then finds the cell (element) that the material point is in. It logically assumes that you want that cell to be in that volume. Then it assumes that you also want all the volume cells attached to that cell. Then it assumes you also want the volume elements attached to those cells and so on. It stops in any particular direction when it reaches surface elements (shells) that were formed earilier when the mesh was being cut into the geometry. However, in other directions, it keeps adding where ever it finds a volume element next to a marked volume element. Eventually, it runs out of elements to add and then start with the next material point and does the same thing.

If during the process the flood fill encounters another material point, it will say that you have leakage because there were no shells between the material points.

As I said, more detail is in the help and on CFD Online...

Does ICEM's material point determination work with just surface meshes? I'm working in 2D and thus have no volume.

No, material points are for marking the volume. Surface meshes or 2D meshes will inherit the part of the surface geometry they follow.

Simon

Alright, no material points for me. I saw another post of yours about conjugate heat transfer and the wall/wall shadow not showing up in FLUENT when meshed in workbench. You mentioned making a multi body part and the original poster said the problem was worked out but never said how. I'm not using workbench, is a multiple body part the route I need to take as well? The wall shadow isn't showing up for me in FLUENT either.

Again, I appreciate all this help. I'm making the switch to ICEM and haven't gotten my hands on any tutorials yet.

NormalVector... If you are working in 2D, then you are just working with shells and I don't think you end up with shadows, but I guess there is the side1 and side2 equivalent...

If you mesh them now, I guess it is meshing each "part" separately and then giving you "walls" around the perimeter of each part.

What you want is for it to mesh conformally between parts so that Fluent knows that the lines between the parts are interfaces?

You just need to create a multi-body part. Here are the steps

In DM, Create your named selections for each zone... Click on edges to create named selections for things like the interface, inlet and outlet. CLick on surfaces to create the 2D fluid or solid zones. Then left click (with the ctrl held down) to select all the parts you want in the multi-body part. Then right click and you will see an option that is something like "Form New Part" (sorry, the wording may be a bit different, I am writing this from memory). This will create a new multi-body part. Then save and proceed to ANSYS meshing.

In ANSYS meshing just mesh and it will automatically create a conformal mesh. Make sure you see your named selections... If you don't then maybe you need to check an option so they are passed from DM... Or you could just create them in ANSYS Meshing if you want (actually, I think ANSYS Meshing has easier tools for creating Named Selections).

Then send the mesh Fluent and your "INTERFACE" named selection will turn into "INTERFACE-side1" and "INTERFACE-side2". (They don't really call it a shadow wall for 2D).

Have fun.;)

Have

Thank you ,Simon.

Hi all,

Can Someone help me?

I am new user for ICEM CFD.
I have a real image from CT scan data in STL file format.
I have imported it into ICEM.
Can smoothing the image be done in ICEM?
When I checked the image in ICEM is in a surface body. Can ICEM create a solid body from this surface body?

Thank you so much is someone can provide me with information.

Regards,
Naima

There is a tutorial for bio-medical scan data... Check the customer portal and find the Aorta tutorial.

ICEM CFD is a surface based modeler. You don't need a solid. Just make sure the surface is "closed"; there are lots of STL repair tools to help you do this. Then put a material point inside and mesh...

ICEM CFD is not intended to smooth the image... It is design to mesh the model, not make it look "artificially" good. Programs like 3DExploration from XDimension Software do a good job of smoothing STL images...

Best regards,

Simon

If you're looking for a program to smooth and manipulate STLs, my research lab uses a program called 3-matic to do all of the prep work on geometry originating from CT scans. I don't have much experience with it but I think it works pretty well.

Hi Simon,

"There is a tutorial for bio-medical scan data... Check the customer portal and find the Aorta tutorial"

I have try this tutorial but always stuck with the function to create a part.
Why when I select the part, it will select the whole geometry?

" there are lots of STL repair tools to help you do this. Then put a material point inside and mesh"

May I know, what is STL repair tools?


Thank you.

Regards,
Naimah

As for the tools, instead of Mimics, how about Slicer3D?

Could you let us know how you got on, this would be interesting-:)

@wanna88, you should probably run Geometry => Repair => Build Diagnostic topology to segment your model by angle before selecting surfaces to add to a part...

Under the geometry tab, there is an icon for repairing faceted geometry. Once you see the names of the commands, you can check the help for more info...

Hi guys,

Thansk for your helpful information in this regard.

I just have a question. I have a box includes a fluid and couple of solid objects. I have already drawn the geometry in ICEM and created the "Body" as fluid. But after meshing, I dont know why the mesh consists of the solid parts!

Any idea is apprecaited!
Thanks
Amir

Pictures are welcome

may be there are holes in your geometry... show us some pictures !

Thank you guys for your prompt responses.
I have read the book Ali posted online. It was very helpful. I m trying to correct the geometry a little bit since there are some unattached cells and will be sharing the final result with you.

I have somehow the same problem. I have a closed surface in ICEM (empty inner part) and would like to fill it to have an full solid body, How can I do that?
I appreciate any help.
Thanks.

Hi Ali Sarami,

Make sure you have done the following steps :

1. Your surfaces cretaed properly and named in the part section
2. The "internal wall" section has been turned on in the part mesh set-up for all the internal solid parts

Good Luck,
Amir

I have a Cylinder and i want to create a outlet on that cylinder but when
 

I have a Cylinder and i want to create a outlet on that cylinder but when i create a part the cylindrical part and the surface created are showing and the cylindrical part is not murging
please can anybody help me or suggest me whats the problem

Doubt on Material Point.
 

In ICEM CFD, What is material point? What is the difference between meshing a 3D model with material point and without material point?

Material point is point which directs the icem cfd to create mesh in specified region if it is closed from all sides.

You dont need the material point usually for 2d or 3d case.

you need material point when you have more than one cell zones in your domain. For example solid and fluid. Air and water etc

Few more doubts in ICEM.
 

Thanks for clarification. I have few more doubts.

I have only one fluid domain.

When I import geometry in ICEM-CFD using IGES/STEP format, in the left window, I can see a some new options, " 1. Bodies " and " 2. Fluid_1_1_MATPOINT ". [Fig 1]

When I share geometry dierctly from Design Modular, these two options will not apper on the window. Why so? What is the difference of these two procedures?



Also, In Fig 2, While blocking, What is that "PART" option. Which option I have to choose to create blocking of my fluid domain.?

Please explain.

It is material point, also known as body.

Neither. Use your own name e.g. fluid.

Or I would delete these bodies and create my own.

@ Sumanth Bhat
In the tree you see a list of different types of geometries: points, lines, surfaces and bodies. Here, bodies are material points. Nothing more, nothing less. You can visualise each type of geometry by ticking them on or off.

If you have a geometry that contains two different volumes, you have to define two body points (material points) within each volume. To help ICEM in detecting the separate volumes during the meshing process.

Then in part you see objects with a specific name. These names will end up in your mesh. The part can contain surfaces & points & lines on which you can define different boundary conditions in Fluent or CFX. It can also contain a body like a fluid or a solid, which end up in fluent or CFX.
Do not create parts that contain surfaces and bodies together. Make unique parts for each body!

When you import an igs-geometry, ICEM creates a single part and normally puts all geometry in there (in your case: Fluid_1_1_MATPOINT). This is a little weird. Like Far explaines, you have to create you own parts. You should put all geometrical objects (points, lines, surfaces and bodies) in different parts that make up boundaries and volumes. If you have assigned every geometrical object to a part, the part that ICEM initially created will be almost empty. It will contain a solid, to my best knowlegde. Then you can delete this part safely.