CFD Forum

Welcome to Autodesk’s CFD Forums. Share your knowledge, ask questions, and explore popular CFD topics.

Turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

This page has been translated for your convenience with an automatic translation service. This is not an official translation and may contain errors and inaccurate translations. Autodesk does not warrant, either expressly or implied, the accuracy, reliability or completeness of the information translated by the machine translation service and will not be liable for damages or losses caused by the trust placed in the translation service.
Translate

Topic Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

Message 1 of 27

Anonymous

1612 Views, 26 Replies

03-04-2018
05:48 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-04-2018
05:48 PM

Hello,

I'm modelling leakage flows within the turbine stage of a gas turbine engine. Essentially leakage flows can occur through the stator disk. As the leakage flow increases, this would disrupt the conventional rotor-stator flow structure and vortices starts forming as can be seen from Figure 1.

I'm basically trying to model this using CFD. I also have to acquire some values such as the pressure coefficient distribution and swirl ratio as a function of the vertical distance within the wheel space; I have experimental results to compare these values to. I have created a basic geometry to model the fluid in the wheel space between stator and rotor disks. I have attached a pdf drawing to show what it looks like (excuse the lack of professionalism). The left one is the stator disk and the right one is the rotor disk. I'm only modelling an 11.25 degree sector with one leakage flow hole to utilise axisymmetry; I'm using the periodic boundary pair on either side of the wheel space cross-section to do this. I have applied a total of 5 boundary conditions to the problem. I have attached the CFD file along with the support file so it is clear what I have done.

I have a few questions.

1. I have made the inlet (bottom) sufficiently long for the flow to develop, moreover Autodesk didn't let me apply a mass flow rate boundary condition on a non-planar surface which meant that I had to add an extension to the front end of the inlet (the bottom). Is there a way to add the mass flow rate condition on a non-planar surface on Autodesk?

2. Would you recommend doing a rotating region analysis? If so how can I go about doing this as I'm not sure how I would model the rotating region into this. Right now I'm just doing a steady state analysis, applying the boundary condition of rotational velocity to the rotor disk surface. The rotor disk is rotating at a velocity of 2500 rpm.

3. When I run the model, it seems to give similar flow pattern as Figure 1 by looking at the velocity field. However, the values I get is not correct for pressure coefficient for example. I get negative pressure coefficients from the built in pressure coefficient result parameter in Autodesk, which is not what I should be getting. In some cases these values are extremely large, much greater than 1. How does Autodesk calculate this parameter? Figure 2 below shows the formula I need to calculate this result, where b = 0.185 (wheel space radius) and omega = 2500rpm and P is just the normal static pressure at each point. Pbar is the mean static pressure within the wheel space. How can I obtain the mean static pressure from Autodesk?

4. With regards to calculating the swirl ratio (defined as the ratio between tangential velocity of the air to the rotational velocity of the disk), I'm not able to find how to identify the tangential velocity of the air in Autodesk.

5. When I use the xy plot to plot some results, how can I see the origin of the co-ordinate system it is obtaining the x and y co-ordinates from?

6. Also, with regards to meshing, I have tried to set wall layer parameters to essentially decrease the y+ value. This causes the model to be stuck at volume meshing when I run it. How could I resolve this? When I run it with the normal default wall layer parameters, it gives me y+ values of zero when I run the model. I don't know why this is the case.

7. Is there a way to do a structured mesh in Autodesk? If so how?

Just to make things clear, I have attached the CFD files and a pdf drawing (image). I can also attach the inventor CAD file if you require it.

Hope I'm not bombarding you with questions. I will really appreciate any help with any or all of the questions.

Thanks,

Rejoys

Solved! Go to Solution.

Solved by David.Short.. Go to Solution.

Solved by David.Short.. Go to Solution.

26 REPLIES 26

Message 2 of 27

03-05-2018
05:42 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-05-2018
05:42 AM

Hi Rejoys,

Please can you attach a [.cfz] file rather than the [.cfdst]. The [.cfz] file is similar to a zip folder and contains all the relevant files for your simulation setup. The [.cfdst] file is a stand alone file that cannot be used without the rest of the design study folder contents.

I can then have a look at your meshing issues.

I am helping out one of your class mates (Chris) in another thread so maybe its best if you keep an eye on that one. I am suggesting using a 2d axisymmetric model rather than modelling a small segment, this avoids the need for periodic BCs. I am still unsure if we can use the rotating velocity BC on a section of a rotor but we shall see!

Regarding your questions I will do my best:

1. Modelling the inlet with an extension is good practice so stick to that.

2. As the rotor is not the prime driver of flow a rotating velocity BC should work well as both you and Chris seem to have figured. Using a RR would likely just add complexity without improving the simulation.

3. I am fairly sure the pressure coefficient is simply the standard as described on wiki. As for finding mean static pressure maybe try using the custom results quantity editor.

4. Could you not just use Vx, Vy or Vz velocity result quantities?

5. Not sure I understand the question. When you do an XY plot you must create a plane on which to plot thus you must know the coordinate system of the plot.

6. Specifically which wall layer settings are making the sim crash? I would recommend using 8 layers with factor 0.60 and gradation 1.30 as a starting point provided that you are using the SST k-omega turbulence model.

7. As we only have tetrahedral elements we can't really do structured meshes as such but if you want some more regularity you could either apply uniform meshing or use a manual mesh.

Hope that helps,

David

David Short

Technical Support Specialist, Simulation

Message 3 of 27

03-05-2018
07:36 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-05-2018
07:36 AM

I am helping out one of your class mates (Chris) in another thread so maybe its best if you keep an eye on that one.

I am still unsure if we can use the rotating velocity BC on a section of a rotor but we shall see!I am suggesting using a 2d axisymmetric model rather than modelling a small segment, this avoids the need for periodic BCs.

I don't understand what you mean by a 2D axisymmetric model? Do you mean an extremely small sector, if so I'm restricted by the leakage flow hole.

3. I am fairly sure the pressure coefficient is simply the standard as described on wiki. As for finding mean static pressure maybe try using the custom results quantity editor.

The only way I could think of finding the mean static pressure is by exporting the data as an excel sheet and finding the mean from that. I wasn't able to find a way to get the mean from the custom results quantity. Maybe I am missing something?

5. Not sure I understand the question. When you do an XY plot you must create a plane on which to plot thus you must know the coordinate system of the plot.

So what I have done is created a plane in Z and viewing the results from an xy plane, it gives me co-ordinates in x, y and z (z being the same for all ofc). However, where are the co-ordinates from? Is it reasonable to assume that they are from the centre of the sector, which is the origin when I modelled it on Inventor.

6. Specifically which wall layer settings are making the sim crash? I would recommend using 8 layers with factor 0.60 and gradation 1.30 as a starting point provided that you are using the SST k-omega turbulence model.

For the wall layers, I was using 10 layers, with a factor of 0.60 and gradation of 1.50. I was still using ADV scheme 5 but not sure if this would be the issue?

Lastly, I had a small admin issue just recently,

Somehow, I managed to stop the server manager. I tried both the start and uninstall button but both gives me errors saying unable like the one above.

I have attached both the cfz files for model I had and a new model I'm working on, using the information I gathered from Chris' thread. The initial one I had I didn't feel the need to model the aluminium solid parts so I only modelled the fluid inside the wheel space. The second one, I added a 0.001m thick layer of solid surrounding the fluid, where necessary. However, I'm finding it difficult to get a solution for the latter with solid layers. Would you be able to give some feedback as to which is a better way to model this problem?

Thanks, I really appreciate your help as u answered all my other questions.

Rejoys

Message 4 of 27

Anonymous

in reply to:
Anonymous

03-05-2018
07:51 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-05-2018
07:51 AM

It doesn't let me attach the cfz files for some reason so I attached them to an A360 drive.

https://a360.autodesk.com/drive/app/

Let me know if you can access these if not I can give u the username and password.

Message 5 of 27

Anonymous

in reply to:
Anonymous

03-06-2018
08:29 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-06-2018
08:29 AM

Hello,

Just managed to figure out how to send the cfz files.

So the first one where I'm only modelling the fluid: http://autode.sk/2FjrH01 -> I feel as though this is a more important model. It would be good if you can check this out.

Second one where I'm modelling the fluid with solid layers: http://autode.sk/2D4tQuL

Message 6 of 27

03-07-2018
02:03 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-07-2018
02:03 AM

Hi Rejoys,

Your model without solids modeled looks great, particularly the BCs and solver settings. I am however concerned about how much mesh you are using. The approx element count is 74 million. Do you have the RAM to do this (you will need roughly 150 GB)?

You may also want to consider extending the inlet and outlet to improve accuracy and avoid recirculation. Also apply a plane surface on these extensions. This article may help.

Regarding mean pressure I agree that the best way is likely exporting to something like excel (i would use Matlab as it is much easier to work with large data sets).

Coordinates on a plane will be based on the bounding coordinate axis system. Turn this on under 'view'. I imagine this is the same as the base coordinate system in inventor but you might have to check.

Let me know which other questions are still pressing!

All the best,

David

David Short

Technical Support Specialist, Simulation

Message 7 of 27

03-07-2018
08:24 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-07-2018
08:24 AM

Hello David,

What approximate size mesh would you recommend to not exceed as a maximum? I only have 4GB ram which explains why it was taking too long to solve.

You may also want to consider extending the inlet and outlet to improve accuracy and avoid recirculation.

Also apply a plane surface on these extensions.This article may help.

Yes thanks I'll extend these further. However, I don't understand what you mean by applying a plane surface on the extensions?

I have questions about convergence and turbulence modelling.

With regards to convergence, is there any guide or rule of thump as to what is a good "tight" convergence setting. Or if there are approximate values for each of the individual parameters to edit individually? Like the instantaneous convergence curve slope for example.

With regards to turbulence model, I'm using an SST k-omega at present but would you recommend doing an RNG k-epsilon model for my flow analysis?

Lastly, what about advection schemes, for my application would ADV 5 be the best?

Once again, I really appreciate your help. It is definitely a good learning experience.

Thank you

Rejoys

Message 8 of 27

03-08-2018
12:22 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-08-2018
12:22 AM

Hi Rejoys,

As a general rule of thumb you will require 2 GB of RAM for every 1 million finite elements. I have given it an initial run with 1.1 million elements and the results are starting to look tasty!

However there is definitely recirculation at the outlet as shown below.

So either extend the whole outlet or get rid of the slanted lip. Removing the slanted lip should be sufficient as the flow looks pretty good in the straight section.

SST k-omega is probably the best first choice, you can have a play with others once you have results! Stick with ADV5, it is default for a reason and has been extensively tested!

I would stay with the default automatic convergence assessment first then if you are not satisfied with the results start thinking about tightening convergence.

I have attached a .cfz with the settings that I used.

Hope that helps,

David

David Short

Technical Support Specialist, Simulation

Message 9 of 27

03-08-2018
06:45 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-08-2018
06:45 PM

Hello,

Thanks again for your help.

I have increased the outlet length now. Here is my updated model: http://autode.sk/2twOXGC

When I run simulations on it, I get some lines on it when I look at the results from the centre plane. The lines are from the mesh but I can't seem to figure out why they are there. I took a screen shot of it below.

Also, I'm hoping to do a scalar mixing analysis with air and carbon dioxide through both the inlets. So instead of putting air into one inlet and carbon dioxide into the other inlet, is there a way to add concentrations of both into one inlet while only having air in the other inlet and see how well the carbon dioxide is mixing into the wheel space?

Lastly, when doing a manual mesh sensitivity study, would you recommend using either the pressure or velocity magnitude at one specific location within the wheel space as the varying parameter?

Thanks

Rejoys

Message 10 of 27

03-08-2018
11:43 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-08-2018
11:43 PM

Hi Rejoys,

You can remove the red outlines by expanding the planes ribbon and unchecking 'show outlines'.

Scalar mixing should be possible with a modified air/CO2 material with density varying with scalar (assign scalar 1 to the density of CO2 and scalar 0 to have density of air). Check out the help docs on scalar mixing. Then use scalar values between 0 and 1 at the inlets to represent mixtures.

You can use either value or both (they are intrinsically linked anyway) just use the same point.

All the best,

David

David Short

Technical Support Specialist, Simulation

Message 11 of 27

03-09-2018
04:11 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-09-2018
04:11 AM

Hello,

Thanks again for the reply.

I have some questions about convergence which I wanted to ask you. How would I determine from the convergence plot of the various parameters (velocities, pressure, TKE and TED) to show how accurate the solution is? I had read the following on the Autodesk website. However, although it talks about the residuals in and out, I'm not sure which parameters to look at for residuals in and out. Also, there is an initial and final value for residual in and residual out so which one from these would I be looking at; I assume it is the final one?

**"We generally want to see at least 3-4 orders of magnitude reduction from Resid In to Out (i.e Out lower than In). The higher this order the better. However, this just tells us the solution is moving forwards smoothly, not that the set up is correct. Bear in mind though that just because we are converged, this does not necessarily mean that we have an accurate solution, just that the solve is complete. It still depends on the set up and the mesh quality. To assess convergence, it is better to look at the average value curve to see if the average values (in the dominant directions/press/temp) have appropriately flattened. Something in the region of 5% change in the last 20% of iterations is usually suitable. You can of course customise the convergence assessment too, so that the solution will continue until the change from one iteration to the next is even smaller than before. Typically it is best to leave CFD to assess the convergence."**

Lastly, what are the units of the y axis for each of the plots. Is it the same units as the parameters.. i.e. for pressure are all the plots such as min, mix, Dphi/phi it's is Pascals?

Message 12 of 27

03-09-2018
05:01 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-09-2018
05:01 AM

Hi Rejoys,

The convergence plot alone can't tell you much about accuracy of the results. It is simply identifying whether the simulation was stable and whether or not more iterations would produce a different result. Using the mathematical residuals is one way that automatic convergence assessment will determine whether the solution has converged to a prescribed tolerance. Rather than worrying about the residuals themselves I tend to simply reduce the tolerance of the convergence assessment to ensure tight convergence.

To determine accuracy of the results you need to establish whether the solution is mesh independent i.e. will refining the mesh further produce a different result? With a mesh independent solution you can then test accuracy / validate by comparing with experimental of theoretical results.

**Lastly, what are the units of the y axis for each of the plots. Is it the same units as the parameters.**

The y values are the average values over the whole domain for each solution parameter. Units relate to the units set under geometry in the design study bar. i.e. if global units are in [m}] the average values will be in [m2/s, Pa etc.]. You can check which units by going to results and seeing which units the legends are in.

Hope that helps.

If you think that I have answered your question / solved your problem please can you mark the relevant post as an accepted solution, alternatively you can allow me to mark it as such. This will help others to benefit from the discussion and easily find the solution if they have a similar issue.

All the best,

David

David Short

Technical Support Specialist, Simulation

Message 13 of 27

03-19-2018
02:09 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-19-2018
02:09 PM

Hello,

I still am not getting the right results with a 3D sector. I tried doing a 2D axisymmetric model after suggestions from my colleague, Chris, who is doing a similar project, but without leakage flows, and it produces decent results. However, for the purposes of my project, this is not sufficient as I need to model the effect of the leakage flow through the stator disk and how that affects the flow structure. The leakage flow hole cant be approximated as a 2D axisymmetric model as there are 32 holes around 360 degrees (so 11.25 degree sector with 1 leakage flow hole). So if I can produce the same results with the 3D model as my 2D axisymmetric model then I can trust the model and explore the effect of leakage flows. I have tried refining the mesh and even ran to extremely tight convergence with well over 1000 iterations and still seeing no change in the results. I feel as though there maybe a problem with the periodic boundary condition or the sector model. I wanted to try a 360 degree model but I do not have that much ram for an accurate 360 degree model. In the model, I have extended the outlet to include the atmosphere from my previous versions to reduce possible recirculation.

I have attached the cfz file and the data points file for the centre z plane. The Vz with parametric distance **across the wheel space** should flatten much higher velocity than what it does in the model. Also, the pressure **down the wheel space** on the edge of stator disk should curve smoothly and the values should vary quite significantly, which it doesn't in my model. Let me know and I can show you details on what the graphs are meant to look like.

It would be good if you have any suggestions.

Data point file across wheel space: http://autode.sk/2FN1xHA

Data point file down wheel space on stator: http://autode.sk/2FO6lMU

cfz file: http://autode.sk/2ppIzvz

Thanks

Rejoys

Message 14 of 27

03-20-2018
05:39 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-20-2018
05:39 AM

Hi Rejoys,

Sadly I can't see the graphs. Maybe screenshots would be easier.

So have you tried comparing the 2D axisymmetric model **without a leakage channel** (Chris's setup) with a 3D section **without a leakage channel**. As you point out this would be a good way to validate the periodic boundary approach. If so please share a comparison of results.

Thanks,

David

David Short

Technical Support Specialist, Simulation

Message 15 of 27

03-20-2018
12:10 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-20-2018
12:10 PM

Hello,

Thanks for the reply.

The 2D axisymmetric model was done with the same geometry as the 3D 11.25 degree sector. However they give me different results when they should give same results. The results for the 2D model is much closer to theory than the 3D one and this is what makes me believe there is a problem with the periodic boundary condition. Also note that these results were obtained with no leakage flow and a bore flow of 0.0138kg/s for 2D model and 0.00043125kg/s (0.0138/32 since 11.25 = 360/32) for the 3D 11.25 degree sector model.

I have attached images of both 2D and 2D graphs for the following parameters:

1. Vz (tangential velocity) across the wheel space at a radius of 0.17m from the co-ordinate origin.

2. Static pressure distribution down the wheel space at very close to the surface of the stator disk.

__So for 1. here are the 2D and 3D graphs respectively.__

__For 2. here are the 2D and 3D graphs__

As you can see the graphs looks quite different for both 2D and the equivalent 3D model and they should be the same as I have used the same boundary conditions.

I have also attached the cfz files for both and the csv file for 2D and 3D models for both across wheel space at 0.17m and down wheel space at stator surface.

cfz of 2D: http://autode.sk/2DHCaRi

cfz of 3D: http://autode.sk/2DIhd8S

Lastly you might notice I stopped the iterations for the 3D one at 1463 instead of 1500, but it won't affect the results much as the convergence plot had basically levelled off.

Thanks

Rejoys

Message 16 of 27

Anonymous

in reply to:
Anonymous

03-20-2018
12:18 PM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-20-2018
12:18 PM

Sorry last csv data as I was limited by how many files I could attach to the previous post.

Message 17 of 27

03-21-2018
02:26 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-21-2018
02:26 AM

Hi Rejoys,

You have included the leakage path in both models meaning that they cannot be fairly compared because (as you have already acknowledged) in the 2D model the leakage path will be revolved 360 degrees with the model. This may have a big effect on the flow.

Please remove the leakage pathway (the extrusion out of the side of the model) from both models and then compare using similar mesh distribution for both.

Also it is likely not great to have such a large P=0 outlet boundary. I would just use a narrow extrusion (rather than the wide volume) to help avoid re circulation.

Thanks,

David

David Short

Technical Support Specialist, Simulation

Message 18 of 27

03-22-2018
10:46 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-22-2018
10:46 AM

Hello,

I have run the models without the leakage flow paths and still seeing the same sort of results as I was seeing with leakage flow paths (I hadn't have applied any boundary condition here so it makes sense that it doesn't affect the results in the wheel space much). Both 2D and 3D models should theoretically produce the same results or similar results at least but this is not the case.

I could make the outlet narrower or stop it at the end of the narrow section as I had previously. I had found that the recirculation wasn't enough to affect the results in the wheel space by comparing an extended outlet model and one that wasn't extended.

It would be very helpful if you have some further suggestions.

Thanks

Rejoys

Message 19 of 27

03-26-2018
04:43 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-26-2018
04:43 AM

Hi Rejoys,

Thanks for your reply. This seems to point towards there being an issue with periodic BCs. Please can you send me both the 2D and 3D models (without leakage paths) and we will discuss it internally.

Thanks a lot,

David

David Short

Technical Support Specialist, Simulation

Message 20 of 27

03-26-2018
06:33 AM

- Mark as New
- Bookmark
- Subscribe
- Mute
- Subscribe to RSS Feed
- Permalink
- Report

03-26-2018
06:33 AM

Hello,

Great. Here they are:

Also, could I ask if there is any way to view a more coarse velocity field on the axisymmetric plane for a 2D axisymmetric model? Right now when I view say, the x-y projection of the velocity vectors (x being the axisymmetric axis), they are so close together that it is hard to see the vectors even when I drag the bar to the very left. For a 3D model I can create a plane and this gives more options for viewing the vectors which makes it convenient but the same can't be achieved for a 2D model. I suspect that it may be because my mesh is very refined as I am aware that the velocity vectors are calculated at the nodes.

I would appreciate it if you have any suggestions for this.

Thanks,

Rejoys

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page