# Transient Blade Row - Time Transformation - Transient Details

 Register Blogs Members List Search Today's Posts Mark Forums Read

 October 14, 2014, 08:30 Transient Blade Row - Time Transformation - Transient Details #1 New Member   Join Date: Oct 2014 Posts: 14 Rep Power: 11 Hello everyone, I have some questions regarding the Transient Details when setting up a Transient Blade Row Simulation with Time Transformation. First of all: I am simulating a two-stage Turbine with different amounts of blades in each blade row. Hence I want to use Transient Blade Row modelling to obtain a better result than using "normal" Transient mode. 1. Do I have to set up a new Time Transformation for every interface? 2. What Domain should be selected in the Time Period section? I was thinking that there must be a connection between the above selected Domain Interface, but as default it gives me a domain not connected to the interface. 3. After reading through CFX-Help I am still not sure how Period and Run are exactly defined and how it connects with the amount of Timesteps that needs to be set. Is the Period equivalent to the Passage? And then the Passing Period is the amount of time it will take the machine to rotate to the next blade? So by setting Timesteps/Period I can specify how many Timesteps should be solved per Passage? And Periods/Run gives the number of how often those Timesteps/Period should be simulated? So the total amount of Timesteps (leaving out the coefficient loops) would be Timesteps/Period times Periods/Run? Thank you a lot for your help, Simon

 October 14, 2014, 09:13 #2 Senior Member   Join Date: Jun 2009 Posts: 1,803 Rep Power: 32 Dear Simon, Have you run the Time Transformation tutorial for the single stage turbine ? Do you understand the purpose of the transformations (Time or Fourier) ? The statement "I want to use Transient Blade Row modelling to obtain a better result than using "normal" Transient mode" hints it is not clear to you what these transformations do. If you model the "proper blade count" on each blade row, the "normal" transient method will produce the best solution for a given mesh and timestep that you can get given the CFX discretization schemes. If you model a "reduced blade count" on each blade row; then, you need some kind of transformation to account for the unequal pitch between blade rows in your model. These transformations will give the closest solution to the normal transient method with considerable savings in computational effort. They will NOT produce a better/more accurate solution (again the keyword is "proper blade count") Also, I advice you to read about the limitations of the Time Transformation for multi-stage machines and how to model such cases. You may need to contact ANSYS CFX support for additional guidelines. On the timestep details, which Domain is selected allows you to think in terms of the period computed using the blade count of that particular blade row. Then, you can decide how many timesteps per passing period of the row of interest you want to base your solution on.

 October 14, 2014, 09:52 #3 New Member   Join Date: Oct 2014 Posts: 14 Rep Power: 11 Dear Opaque, thank you for your reply. Of course I know that it would be best to set up a simulation with the entire blade rows instead of only one passage and that this would give the most accurate solution. But my mesh is pretty large so that I have no other choice than calculating it by one passage per row. And I have ran through the tutorial several times. But I still can not get any answers out of it since it is only one interface that is transformed. I thought that given the circumstance of not retaining the same amount of blades in each row (also both rotating blade rows have different amounts of blades) it would be necessary to set up a Transient Blade Row simulation to improve my solution. I do understand why there needs to be a Transformation. And Time Transformation seems applicable since my pitch ratio is close to 1 and flow is compressible. But is there an actual need to initialize different Time Transformations because of the different amount of blades in each rotating row; Or in other words: do I need one Time Transformation for every Interface between a rotating and a stationary row? Or will CFX automatically adjust the Time Transformation to every Interface that I put into Transient Details-Time Period?

 October 14, 2014, 10:09 #4 Senior Member   Join Date: Jun 2009 Posts: 1,803 Rep Power: 32 Fair. Not sure what is the blade count between your blade rows, but the "proper blade count" model sometimes is not the full wheel though it will still be a large model. From your description and concerns with interfaces selection, I guess you are not familiar with the limitations of the Time Transformation model for multi-stage machines, nor how it works between blade rows. A short description would be " a given time transformation corrects for the unequal pitch at the selected interface between two blade rows". My advice is to contact ANSYS CFX support for further insight into these complex models, and how they may apply to your specific situation. It will save you considerable time in the long run.

 October 14, 2014, 10:44 #5 New Member   Join Date: Oct 2014 Posts: 14 Rep Power: 11 Alright then I will do so. Thank you for your help so far. If anyone else wants to give hints on this problem you are more than welcome.

 October 15, 2014, 04:09 #6 Senior Member   Thomas MADELEINE Join Date: Oct 2014 Posts: 126 Rep Power: 11 Hi all, If I understood all clearly you want to make a stator/rotor TBR- Time Transformation. So you want to simulate a two stage turbine. so each blade see a periodic disturbation in the effect of the other stator/rotor. For that the Time Transformation collect the data between the two stages. Then it expand this interface ( with periodic condition ) and reintegrate inside the model. So while you have only one blade of each stage, the pitch ratio don't really bother you ( try to keep it between 0.6 and 1.3 but i'm not sure ) that's for how it works. if it is a simple single rotor stator case just copy the ccl from the tutorial. time transformation rotor stator define the rotor domain define the stator domain define the interface between the two domain ( only with ggi ) etc 1) Use Time Transformation only on the interface between the stator and rotor (it will ask for other thing). only 1 Time Transformation between 2 domain 2 Time Transformation between 3 domain etc... (if someone from ansys can confirm for further stages, i am not sure) So for me a 2 stages turbine (2 rotor and 2 stator) should have 3 Time Transfomation 2) how many Domain do you have ? Normally Time Transformation will ask for the stator domain and the rotor domain only. 3) So the period depend on the rotation speed of your rotor and the amount of blades of the rotor and stator It is the time for one rotor blade to go through the entire domain of one stator blade ( not sure to be clear here ) so you will technically have 3 different Period Time ... I don't know which one use to define your time calculation I expect something like the smallest multiple of them (like for 3s , 4s and 6s => 12s) see the expression in help at : ANSYS Help/CFX/Modeling Guide/6.Transient Blade Row Modeling/6.8.Use Cases/6.8.2. Case 2: Flow Bounndary Disturbance (At the end you have the DeltaT expression) Hope it is clear and correct I didn't really try this one.

 October 16, 2014, 04:53 #7 New Member   Véronique Penin Join Date: Mar 2014 Location: Lyon, France Posts: 21 Rep Power: 12 Thanks Thomas Madeleine for your explanation. A small precision : in tutorial #35 (of CFX 15.0), "For the Time Transformation method, you should always maintain an ensemble pitch ratio within a range of 0.75 to 1.4.", which is a little different that Thomas Madeleine said.

 October 16, 2014, 07:52 #8 Senior Member   Join Date: Jun 2009 Posts: 1,803 Rep Power: 32 The use of more than one Time Transformation is a beta feature (Enable beta features in CFX-Pre and see the message once you activate more than 1). It is a beta feature for a reason that must be discussed with ANSYS CFX support to confirm your case is suitable before attempting such calculations. Certainly, you can activate as many transformations as you please as long as you are aware of the consequences of doing so. Keep in mind that transient simulations are computationally expensive and time consuming. You do not want to run a calculation for days to realize the setup was incorrect for some subtle details. My 2 cents.

 April 28, 2015, 04:01 #9 New Member   Albert Join Date: Apr 2015 Posts: 3 Rep Power: 11 Hey, I'm simulating a multistage axial turbine. To safe calculation time and effort I want so reduce the transient problem to one blade per row. However I did the tutorial and read all depending pages from the provided ansy help viewer. I understand how this interface model works and can setup several setup for a singe stage. My problem is that as soon as I use the beta features for the multistage modeling the ANSYS Solver adds a sixth imbalance. I'm wondering if someone knows how to deal with the 'Streamwise Scale Imbalance (%)'. As soon it is a constant value with no change over time I would suggest that it is only a simple scale factor? Thanks for your help Alex

 April 28, 2015, 04:50 #10 Senior Member   Thomas MADELEINE Join Date: Oct 2014 Posts: 126 Rep Power: 11 I am not sure of what I will say but as far as i understood the theory, CFX will save the interface data over a period in order to reinject this on the different interfaces at the right time (the T-deltaT thing in the help). So for me the streamwise scale imbalance should be connected with that like how much data are lost in the process or do we recover all our flow at the end. If you want to be sure I can only suggest to mail that question to ANSYS directly to know what really this is. aVe78 likes this.

 April 28, 2015, 08:19 #11 Senior Member   Join Date: Jun 2009 Posts: 1,803 Rep Power: 32 For clarification, the term "Streamwise Scale" is a variable used to compute the Streamwise coordinate (how far within the machine). That is, 0 at the inlet, and 1 at the outlet. This coordinate may be used for multiple purposes. For example, CFD-Post creates a similar variable when doing turbo-processing. Hope the above helps, aVe78 likes this.

 April 28, 2015, 09:49 #12 New Member   Albert Join Date: Apr 2015 Posts: 3 Rep Power: 11 First of all thank you very much for your reply. I think I can use your information to do some more progress and contact the support afterward. I can only tell you that if you use the mesh from the tutorial 35 and simply copy the first stage and use it as the second stage you will get the imbalance from -4% (S1), +0.2% (R1), +0.5% (S2) up to +6% (R2). The imbalance is not increasing continually and I don't think thats it is only depending on the axial position as the different from S1 to R1 is not the same like S2 to R2. I will try some more test and if I'm getting some more news I will come back here. A.

 April 28, 2015, 09:55 #13 Senior Member   Thomas MADELEINE Join Date: Oct 2014 Posts: 126 Rep Power: 11 Since you do some test can you please have a look at the massFlow in each passage ? I would expect it differs depending of the passage size (the global massFlow is constant only on the entire model). Thanks a lot: I hope it is connected with this value. And if you have any answer of what this imbalance means, please fell free to post your explanation here I am sure some people (at least me ^^) want to know it. Again thanks again for your work

 May 4, 2015, 17:29 #14 New Member   Albert Join Date: Apr 2015 Posts: 3 Rep Power: 11 Hi again, I took a look in the massFlow. You are right that the massflow vary from blade to balde and row to row. But it is like I expected, the chance from blade to blade in one row is really small, the change from row to row is only depending on the different blade count. Did I match your question? I also had a talk to the ANSYS support...he even didn't hear about the "Streamwise Scale Imbalance"

 May 5, 2015, 03:46 #15 Senior Member   Thomas MADELEINE Join Date: Oct 2014 Posts: 126 Rep Power: 11 thanks for the details it was exactly my question. so for me the streamwise scale imbalance is bound to this (if it keeps things between the TBR interface). To have precise details about this method you should ask to the developers. If it is the same team than for the TBR-FT it should be based in Canada, maybe you can send them a mail.

 May 8, 2016, 02:50 #16 Member   misagh Join Date: Apr 2012 Posts: 64 Rep Power: 14 Hi Time transformation and Fourier Transformation methods can be used for single stage machines. for multi stage machine, you can use profile transformation method. Regards

 August 6, 2016, 09:40 #17 Member   Join Date: Jul 2016 Posts: 33 Rep Power: 9 Dear misagh, Ansys allows for multiple time transformation methods. Here, documentation of Ansys 17 exaplains how to model a multistage problem but I somehow cannot even see the "single-sided TT interface" option in my current academic Ansys 17.0 version...: https://www.sharcnet.ca/Software/Ans...07949160230086 I have read the documentation, tutorials and many posts on this forum but I cannot find why my multistage problem does not work. The pitch is acceptable, but the CFX-Pre says: "only certain combinations of disturbances and interfaces are supported." I can't find why my combination does not work if the pitch is between 0.79-1.3.

September 8, 2022, 05:23
#18
New Member

JiandongYan
Join Date: Mar 2021
Location: Beijing
Posts: 9
Rep Power: 5
Quote:
 Originally Posted by Sasquatch Dear misagh, Ansys allows for multiple time transformation methods. Here, documentation of Ansys 17 exaplains how to model a multistage problem but I somehow cannot even see the "single-sided TT interface" option in my current academic Ansys 17.0 version...: https://www.sharcnet.ca/Software/Ans...07949160230086 I have read the documentation, tutorials and many posts on this forum but I cannot find why my multistage problem does not work. The pitch is acceptable, but the CFX-Pre says: "only certain combinations of disturbances and interfaces are supported." I can't find why my combination does not work if the pitch is between 0.79-1.3.
Dear Sasquatch,

I have checked the document you cited, where the CFX-Solver Modeling Guide only illustrate the 'Modeling a multistage turbomachine with Time Transformation TRS and single-sided Time Transformation interfaces (STT-TRS)'. In this case, the Sigle side time transformation was used. As a result, the disturbance between different rows can only propagate in one direction, which is not the initial intention of utilising the TT method. however, I read some references showing that they have succeeded to apply the TT interface in a 6-stage axial compressor, which means there were at most 11 different TT interfaces used. Unfortunately, they did not show clear procedures.
__________________
Jiandong Yan