[Jambond]

Hello everyone,

I am new to this forum and to CFD in general so I might be asking dumb questions, but I'm really struggling with Star-CCM+ right now. Thanks in advance for your help.

I'm trying to simulate the intake air/exhaust gas flow through a turbocharger for a project at school. I've got the CAD files and the first step is now to create a volume inside of the turbocharger for the fluid to flow through.

I am using the 'extract volume' tool for this matter. I followed this tutorial: https://www.youtube.com/watch?v=XWWgBc_24LU

But once I completed all the steps, filled the holes and so on, I get this error whilst trying to extract the volume: "Could not find any topological region attached to selected surfaces".
I think the problem might come from the Merge/Imprint part, but I can't come up with a solution...
I neither have found anything on this forum nor elsewhere online concerning this particular error.

I hope you guys can help me. I can review each and every step in detail if needed.
Much appreciated!

Jambond

[fluid23]

Are you using v6 like the video? It sounds to me like the surface wrapper would be a better choice for this if you have a newer version.

[me3840]

I will disagree here wtih MBdonCFD; the surface wrapper is really useful for larger geometries with lots of parts, but turbochargers aren't that big and it's not a huge task to be able to clean them unless the input CAD is garbage. Turbomachinery are very sensitive to mesh quality and I would be concerned with poor surface quality produced by the wrapper.

Can you post some images of your geometry, or the geometry itself? This error related to extract volume likely means either (a) the geometry is not clean, or (b) the geometry is not properly imprinted. Are you making this a CHT problem?

[Jambond]

Morning!

Thanks for your answers.

@MBdonCFD: I am using v9. I later found this other tutorial using the surface wrapper (http://wenku.baidu.com/view/b5f3ead2...886ce6.html###), and managed to generate a more or less proper mesh in the end, but when trying to run a simulation on it it told me about a missing volume mesh. I didn't really look into it though so maybe we'll get to that later.

@me3840: Here are a few ProE views of the geometry. I am currently practicing/testing the meshing methods on the compressor alone:




So right now I'm not sure what to do. Should I carry on with the surface wrapper or stick to the extract volume tool?
Thanks in advance for your answers.

Oh and I'm not sure what you mean with CHT but if it stands for Heat Transfer-something; yes I'm supposed to simulate the heat transfer from the turbine towards the compressor. But I think this stands a few steps ahead Or maybe I'm already tackling the problem wrong?

Jambond

[fluid23]

Surface wrapper will only create a surface mesh. Think of it like blowing a balloon up inside a box. You still need to go through and generate a volume mesh from the surface mesh that comes out of the wrapper.

[Jambond]

Yes I eventually figure that out by myself, but thanks for your reply, that's actually exactly the right explanation

I just managed to obtain an approximative fluid path, that more or less ressembles the one of the air through the compressor:


However, it's not exactly right, the outlet part is missing. I used the 'seed point' mode instead of 'largest internal'. I positioned the seed point somewhere inside the air duct, as shown in an online tutorial. Could the problem stem from there? I mean, could the position of the seed point drastically change my surface (and volume) mesh?


About the other method (without the surface wrapper); I followed the advice given in this thread: http://www.cfd-online.com/Forums/sta...ping-mesh.html
I did fine up to the 'split by surface topology' step... Almost all the parts just disappear.
So I did what willimanili sais in that same thread and attempted to extract the individual volumes and the unite them... Didn't work either. I don't even know what mode I should use: automatic or surface?
- When using the automatic mode, I get this error:

- What surface should I choose in the 'surface' mode? I tried with the inlet surface but the then extracted volume is just the compressor itself, not the air duct... Makes no sense

So my last question would be: should I try and dig further with that method, or rather stick with the surface wrapper?

I think there are quite a few things I still don't understand about all this, but I' really trying hard Thanks for your help.
Jambond

[me3840]

It looks to me like your surface is not closed or properly imprinted. Have you run the surface repair diagnostics on your parts?

Is this geometry sharable? I'm willing to give you some help with it if you are willing to send me the files.

[Jambond]

I just re-ran it, here is what the diagnosis looks like:


There seem to be a lot of pierced faces in the wheel/axis area... I'm not sure what to do with this though
I'm currently checking with my advisor to see if I can send you the files, it would sure be easier.

One more question, rather out of curiosity: I've seen different tutorials where people are either importing the CAD part (Parasolid file) through the 3D-CAD Module, and then creating geometry parts and assigning regions to parts; or importing a surface mesh (using the same Parasolid file) and checking 'create new region'.
I don't really see the point of the second method, in that it doesn't let you run a surface repair on your parts because well there aren't any... Or am I seeing this wrong?

[me3840]

The lack of errors in the last 3 category and presence of them in the first indicates that you have a model composed of valid solid bodies but they are not imprinted properly or at all. I would run the CAD-based imprinter (operations>new>boolean>imprint, and switch the imprint mode to CAD). This should figure out which surfaces of the bodies are touching other surfaces and split them appropriately.

On your curiosity question:
The second mode you stated (create new region) is a legacy feature from older versions of the code; the 'parts' folder didn't used to exist. You can still run surface repair on the then-created 'initial surface' representation if you wish. But doing things this way eliminates a lot of good features of the parts tree, so I don't recommend it.

[Jambond]

Hi me3840,
First of all, here is how far I've got right now. I simply refined the mesh and it gave me a proper extracted volume for my TC:

It fairly looks like the path the air is taking in the TC.

Now I tried to run the imprinting operation anyway. And well... I'm not really happy with the result

I ran the imprinting by right-clicking on Operation, then New>Imprint, and chose the CAD mode.
It basically deleted almost all parts and left me with this geometry:

As you can see it looks nothing like a turbocharger of any kind...

I also tried to imprint the parts by selecting them all in the tree, and then Create Mesh Operation > Boolean > Imprint Parts, but got an error.

So on one hand I managed to get a proper result using the surface wrapper; but on the other hand there clearly is a problem with my CAD as the imprinting shows...
Are you familiar with this issue?
Thanks in advance!
Jambond


PS/Edit: Thanks for your answer on the two import modes. I understand that importing the CAD via the CAD modeler is better, however I've come across a strange problem doing so; one of the faces of the housing is missing, plain and simple:

It makes no sense to me. The CAD is fine, I've probably imported this exact same Parasolid file 20 times without any issue and now this... Then I used the second method out of despair and it worked fine, so I'm really tempted to go on with it...
I know we're drifting a bit from the original topic here but it's really weird... ever seen that before?
Thx!

[me3840]

Do you mean you refined the tessellation? Did that extract volume operation give you correct contacts between the solid and the fluid?

If you are using the imprint operation, be sure to get rid of any contacts you have before the operation. I'm not sure what the difference between the first and second imprints you did are..

Note that for the extract volume method with CHT meshing, the workflow should be:
1. Import solid CAD
2. Repair anything to create closed solid volumes
3. Imprint the solid volumes together
4. Use extract volume to get the fluid volume
5. Mesh

Importing directly to 3D-CAD is identical to importing to the parts tree. In fact, any CAD part you import to the parts tree can be moved to 3D-CAD. The parts tree just contains the tessellated surface as well as the associated CAD information, whereas 3D-CAD only deals with the later.

The fact that a face is missing in 3D-CAD is not entirely surprising, often this indicates the CAD file is invalid or contains some issues. You can right click the part and select 'check validity' to verify. If you are in 10.04 you can open CAD repair to actually see what parts are damaged where and why by just right-clicking the part and selecting CAD repair.

Did you get anywhere on sending the geometry? CHT is not always the easiest setup from the CAD perspective.

[Jambond]

By refined I simply meant diminished the base size of the mesh.

What do you mean by get rid of the contacts?
I tried to imprint following either the online tutorials or your advice, and every time it ended up deleting most of my parts and leaving me with just a couple parts that don't even have anything to do with the air flow.
I know I'm doing something wrong but I don't know what

By "repair anything to create closed solid volumes" you mean for example recreate that missing surface after the import? Because I've tried this but didn't succeed... I used the repair mode and the "fill holes" tool but the shape is apparently to complex.

I really don't understand what the problem is with the import, it used to work fine

I'll try the workflow you suggested in the morning, but it really ressembles what I've been doing up till now, and it always gets messy at the imprinting step... I've read and watched all available tutorials on this and I'm getting nowhere, I feel like I'm missing the whole point.
For example I've used the surface repair tool, Merge/Imprint mode, then Multi Part Imprint, checked for close parts and then ran 'Imprint all'... Should work shouldn't it? Well it doesn't
And using the Operations node, I get a different but just as unacceptable result, as shown above.

It feels like my CAD is rubbish, or like there's something I didn't understand about all this; or both.

Thanks for your help so far, I'm sure it will work out in the end!

PS: I've asked my university about sending you the CAD but it's a no for the moment; I'll try to talk them into it.

[Jambond]

(Sorry about the double post but I think it's clearer this way)

Forget about my question on the contacts, it became clear once I had the software in front of me...
So I went on and:
- imported the CAD
- created new geometry parts from it (at that point the missing face reappeared)
- ran a validity check on those parts: a good dozen of them is labeled non valid, including the most meaningful ones (housings mostly)
- deleted the existing contacts
- selected all parts and launched the Multi Part Imprint mode with a tolerance of 1mm. It found nearly 300 pairs and took about 2 hours imprinting them all. Here's what the result looks like:


As a reminder here is what the TC should look like...


So it seems my CAD really is garbage doesn't it?
What does the "non validity" exactly mean?
I didn't design the CAD myself but I highly doubt it was done that badly, it actually looks just fine in ProE. Could this be a compatibility issue between Star CCM and ProE? A wrong file format?
Thanks in advance, have a nice day!

[me3840]

I know complex geometries like this can be frustrating especially if you're not too sure on what all the switches do.

Did you take a look at your CAD in CAD repair? This will show you what all the invalidities are. Perhaps that can fix some of them too, but there aren't many options for it, just 'fix'. STAR's pro/e CAD translators, are, in my experience, kind of awful. You might try exporting it as a parasolid. When you import the CAD, uncheck 'create contacts from coincident faces' too.

I would stick with the imprinter in the parts operation tree because its actions are reversable. I don't like doing things that can't be changed later, so I try to avoid using the surface repair imprinter.

It found nearly 300 pairs though? It didn't look like you had anywhere near all of those parts in the simulation; where are the rest? I only see perhaps 10 or so.

The problems you're having look like they lie entirely in the imprinter. You import closed valid solid bodies it looks like. Try imprinting just 2 or 3 of the important parts and see what it makes.

Getting help with these kinds of cases is relatively difficult without seeing the geometry, but hopefully we can manage either way.

[Jambond]

So here is what I just did (I prefer to go ahead and detail all the steps every time, in case there is a tiny thing I did/didn't do that messes everything up):

- Started a new simulation
- Imported my geometry as a Parasolid file (which I created by saving my file with a new .x_t extension in ProE) using the CAD module
- Created new parts from this geometry; unchecked "Create new contacts" etc
- Right click on just the compressor housing I know to be faulty > Repair surface
- Ran a diagnosis, here's the result:

- Clicked on the bottom right button shown above: "Auto repair surface errors". Output:


If the software went ahead and simply deleted all the faulty faces (cause it's what it looks like), well... there's a lot of them

So there seems to be quite a problem with this part's surfaces already, and it's just the tip of the iceberg; I have another dozen faulty parts that should show just the same issues.

I'll now try and imprint just 2 or 3 parts together as you suggested and get back to you.
I also found it very odd that nearly 300 pairs where found, that's why I pointed it out... Seems to me as if the software were treating my parts as a cluster of smaller parts and thus trying to create contacts between non existing parts/faces where there is no point even trying to do so, and of course failing.

[Jambond]

(I had to double post because of the many images)

So I've tried a few other things and I'm just lost. I'll detail it all again so you can try to understand the problem because I don't.

1) I tried to work on just 2-3 parts, i.e. the compressor side.
- New simulation
- New CAD Model > Import CAD (Parasolid file)
- New geometry part > Uncheck "create part contacts" > OK
- Select all parts > Repair surface > Diagnosis:

- Auto repair surface tool; output:


(so this time the output geometry looks fine... hum)
- Close Surface repair tool
- Operations > New > Imprint (Select all parts, tolerance: 1mm)
- Output geometry looks fine (basically just like the one shown above, apparently no deleted parts), output message:
Warning: unable to match patch 8253 to a source-side part surface.
Warning: unable to match patch 8277 to a source-side part surface.
Imprint operation created 10 new contact(s).

So now all my parts are imprinted, I'm going to try and extract the volume. I know two methods, so here we go.
First of all, fill holes:
- Right click on the housing part > Repair surface > Check "Edges" > Select inlet and outlet edges (circles) > "Fill holes" tool (H)
- Close Repair surface mode
So the inlet and outlet holes are properly filled. Now:

First method
- Select all parts > Right click > Create mesh operation > Extract volume > Mode = automatic; no error, result:

So clearly not what I wanted... Next method

Second method
- Split by patch > Select inlet and outlet faces (from Fill holes) in order to rename them; I noticed a problem with the inlet surface:

As you can see the selected surface (pink) isn't just the inlet plane as it should be, but as an additional conical face to it. Really weird as I used to same method for both outlet and inlet and this mistake doesn't show up at the outlet. Anyway...

- Continua > New mesh continuum > Select Meshing models > Surface wrapper + Polyhedral mesher
- Select all Parts > Assign Parts to region:

- Change Volume of interest methode to Seed point, create a seed point somewhere in the air duct near the inlet face
- Delete the feature curves
- Generate surface mesh; error:
"Boundaries: "..." and "..." share patch=xxxx but are not internal interfaces"
(I've got like 30 lines of this... what does this mean???)

So I wasn't even able to mesh the model in the end.


2) I then tried something else, on the whole turbocharger this time.
- New simulation etc... Long story short: I imported the whole TC and created parts from the geometry.
- Repair surface on all parts; output:

Here is where the pierced are looking to be located:

- Auto repair; output:

So fewer pierced faces but a LOT more face quality and proximity defaults... Anyway here is a close up of the output geometry:

It's awful! The wheel is gone... No point even trying to imprint this


So I might be set for the longest post ever award right now...
I hope you can help me, I'm really starting to lose hope here
Thanks in advance!
Jambond

[me3840]

I wouldn't loose hope, I think you're learning, but there are a few mistakes in your procedure:

1. When you are looking at a geometry representation of your model, you can ignore face quality, proximity, and even some pierced faces. In general the presence of these errors does not indicate a problem with your geometry. If those errors appear on the remeshed surface, that is an issue, but we're not at that stage.

2. The surface repair auto-repair feature is not really intended to 'fix' dirty geometry at all. It's far better suited at repairing small errors in the remeshed surface automatically. Never, ever, ever run auto-repair on anything other than a remeshed surface (or an imported delaunay surface). The output will be garbage, as you have seen!

3. Your imprint produced some errors, you need to find out why and correct them. Never just assume it'll be okay and continue on. Take a look at what the imprints actually look like; are the faces matched? Did your imprint produce any pierced faces? Pierced faces are bad news for the output of an imprint operation.

4. Your inlet surface is joined with the side of another CAD patch because you did not put the inlet surface into a new part surface in surface repair. Split by patch is unable to break up patches built in surface repair because those patches are not CAD based. You need to go into surface repair and put the faces of that inlet into a new surface.

5. The automatic extraction rarely figures things out right, use the surface selection method and select your inlet.

6. You're trying to extract the volume, I'm not sure why the surface wrapper gets used; I would avoid it for something like this.

You may be able to get by in this simulation by using non-conformal interfaces, although it will hurt your accuracy. It's pretty easy to mesh with them; just select per-part meshing, mesh all your parts, and make interfaces between the boundaries. That will work, but it's not ideal from an accuracy standpoint.

[me3840]

To be a little more descriptive, I think you should:

1. Import just a few of your parts.
2. Check that they have zero non-manifold edges, vertices, and free edges. Ignore any other metric at this stage.
3. Imprint those parts.

And see if that works out for you. Ignore meshing the fluid volume for now and focus on the solids. The fluid is easier to get once the solids are done.

[Jambond]

Morning!

So first of all, thanks for your detailed reply. It really helps, especially right now as I'm quite stranded
Those 6 mistakes you pointed out were really helpful, I think I understand the whole thing a bit better now.

Now, I went on and tried to imprint just a few parts. Just for you to picture the whole thing, I imported the following parts on the compressor side (only):
- housing
- cap (the part that closes the housing on the opposite side of the inlet)
- wheel
- a few bearings/seals in the wheel area; I didn't want to remove them in order to preserve a watertight body

I ran a surface repair diagnosis; it found quite some pierced faces and proximity/quality defaults but no non manifold edges/vertices and no free edges.
I then imprinted the parts with a tolerance of 0.1mm, it created 9 contacts. I verified each one of them with my CAD (i.e. is this part really supposed to be in contact with this one as found by Star CCM?) and aside from the wheel/cap contact it was ok. The wheel isn't supposed to touch the cap for obvious reasons; but I figured I'd leave it alone for now.

My parts are now imprinted but I don't see any geometrical differences with the non imprinted version. Is this normal? I'm referring to your question: "are the faces matched?". Should I be able to observe a difference on the geometry? Or is there another way to do so?

I ran a new diagnosis and it was the exact same one as before. So no pierced faces were created by the imprint.

So it's good news right?
What do you think should be the next step?

What I think I'm going to do now:
1) Try and extract the volume on this same model and see how it works out.
2) Gradually add parts to the model and try to imprint them, then see if a problem shows up.
I'll get back to you after that
Jambond


Edit: So, short update. I tried to extract the volume using the "surface" mode and selecting the inlet. I got the same error as at the very beginning: "Could not find any topological region attached to selected surfaces".
But I had the feeling that this had to do with the wheel area, where several complex parts clog the air duct (mostly the wheel).
So I simply deleted them all and only kept the housing and the cap; so it couldn't be simpler now.
I completed all the previous steps all over again and then extracted the volume: it works.
It then seems that the problem is coming from the wheel area. But I don't really understand it though; why is the software making this a topological problem? At most it should extract the volume between the inlet and the wheel and stop there, since everything is properly imprinted and the contacts are OK... Why doesn't it?

Edit 2: I repeated the operation on the whole turbocharger minus the wheels, and here's what it looks like:

Pretty good right?
There are still a few mistakes but they have to do with the CAD, I'll deal with them.

I also tried to extract the volume on the compressor alone with the wheel, with a refined imprint (tolerance 0.01 mm), and this time it worked.
So maybe the problem was rather coming from the other parts in the wheel area...
Maybe we can do without them for now and get back to it later.

What should be the next step? Mesh?
Have I forgotten something?
Thanks again!

[me3840]

Well, I haven't seen the wheels in detail, but are they both a single part? i.e. is the compressor and turbine and shaft all a single piece? If so, they are probably cutting through the housing and need to be boolean subtracted or something of that nature. You can also go the cheap route and just delete the shaft so the two wheels are just 'floating' in the housing. This is the easiest method and it has nearly no impact on the solution.

Once you get the wheels floating, you need to put some kind of control volume around them. That control volume will be included in the extract volume operation, but that control volume cannot touch any parts - it will also be 'floating' and will become your interface between the rotating and non-rotating portions. Then the extract volume will include all of your parts minus the gas outside of both wheels, but inside their control volumes. Then you can either use another extract volume to get both of those rotating volumes, or a subtract, whatever floats your boat.

On imprinting: When you imprint something, you physically take the outline of a face on one part and project it to another opposing part. This now means the two parts 'share' a face or set of faces. It should cause a noticeable change in the surface mesh of both parts. This face will later become an interface allowing heat or mass transfer. Where things get tricky is when two surfaces are not quite on top of each other, or are not exactly the same size. This is where that tolerance factor comes into play; it's used to figure out how far a surfaces faces or edges can be moved to match another surface.