[kimie]

hye everyone . i am currently a cfx simulation to study the effect of the bypass pipe toward the turbine efficiency. before i run my case, i have run a turbine model which has no modification at all (no waste-gate pipe) to validate my model and the model give a good result.


After that, i have change the connecting duct of the turbine with the modified version which i add a new opening called wastegate_outlet. the opening should be to the open air so the boundary that i set at the opening is.

opening pressure: 1 atm
opening temperature: 298k



This boundary is the same boundary that i use at the turbine main outlet which is also to the open air.

the theory is when i adding a new opening bypass before the air entering the turbine, i can expect that the turbine efficiency will decrease with the opening area.

My problem is i cant get a good result when i run the cfx with my new modified model . my result is not reliable because i get too much torque at the blade when using my new model and this should not be right because adding the bypass will make my turbine to run at a lower efficiency. the fact, my result


for the input massflowrate :0.3kg

original model efficiency : 0.7
new model efficiency :4.9


this is obviously something is not right with my new model as soon as i add new bypass pipe. my first opinion is i think that my boundary for the pipe outlet is not too right but i have no more idea because i have set the ambient pressure and temperature correctly.


i hope there is someone who can view my problem because i have been through the almost same problem with me at the cfd online forum but still i cant figure out where is my mistake.


i have attach the picture of my original turbine model and my modified modal.

original model
https://www.cfd-online.com/Forums/at...1&d=1495120870


wastegate-added model

https://www.cfd-online.com/Forums/at...1&d=1495120918


thanks

[ghorrocks]

You probably should have the waste gate at 0 pressure and use a reference pressure of 1 atmosphere. Are you sure you have set the reference pressure correctly?

I would have a look at the streamlines and flow vectors in your results. Are they behaving as you expect?

Also check your calculation of the efficiency. There could be an error there.

[kimie]

hye ghorrocks! i am so happy to see your respond.

currently i have set the reference pressure as 0atm for the whole system .

at the turbine outlet i have set 1atm pressure at 298k opening temperature.

at the wastegate outlet also i have set the same thing as turbine outlet because both of them should expose to the ambient.

or you have suggest me to change the reference pressure :1(turbine whole volute) and opening pressure :0(wastegate opening) or change the reference pressure for the whole system?

for the streamline and flow vector, it did look as i expected.


so here i am attach my boundary setup, streamline,flow vector of my model.


thank you so much for the respond ghorrock.


reference pressure:

https://www.cfd-online.com/Forums/at...1&d=1495152054

waste-gate boundary

https://www.cfd-online.com/Forums/at...1&d=1495152089

rotor pressure

https://www.cfd-online.com/Forums/at...1&d=1495152106


streamline

https://www.cfd-online.com/Forums/at...1&d=1495152114


vertex at wastegate outlet

https://www.cfd-online.com/Forums/at...1&d=1495152131

[kimie]

continue from my previous reply with attachment of my setup, also ,I'm pretty sure my calculation is correct because this is the calculation I used to validate my previous unmodified model.

Thanks again.

[ghorrocks]

You should use a reference pressure set to a pressure somewhere between the biggest and smallest pressure you are going to see in your model. If your device is connected to atmosphere somewhere then it makes sense to use a reference pressure of 1 [atm] and then all pressures are gauge pressures from there.

Why? This reduces round off errors and makes you simulation more numerically stable. You comments suggest your model is running OK without it, but you never know when a change you are doing will require additional numerical stability and will not converge. It is a simple way of making your model more numerically stable, so why not do it?

Your images did not get attached properly. Have a look at the FAQ on attaching images: https://www.cfd-online.com/Wiki/Ansy...n_the_forum.3F

Your posts are going to moderation because they have lots of links in them and lots of links triggers the spam detector. I have approved all your posts, but you should post such that it does not go to moderation. If you attach the images as directed in the FAQ it should not trigger the spam threshold.

[kimie]

Originally Posted by ghorrocks

You should use a reference pressure set to a pressure somewhere between the biggest and smallest pressure you are going to see in your model. If your device is connected to atmosphere somewhere then it makes sense to use a reference pressure of 1 [atm] and then all pressures are gauge pressures from there.

Why? This reduces round off errors and makes you simulation more numerically stable. You comments suggest your model is running OK without it, but you never know when a change you are doing will require additional numerical stability and will not converge. It is a simple way of making your model more numerically stable, so why not do it?

Your images did not get attached properly. Have a look at the FAQ on attaching images: https://www.cfd-online.com/Wiki/Ansy...n_the_forum.3F

Your posts are going to moderation because they have lots of links in them and lots of links triggers the spam detector. I have approved all your posts, but you should post such that it does not go to moderation. If you attach the images as directed in the FAQ it should not trigger the spam threshold.

hye ghorrocks thanks again for your response. my previous setup of reference is 0atm and my opening pressure is 1atm.

Actually i have been running the simulation with the new reference pressure :1atm as soon as i read your response and i have setup my opening


turbine opening:0atm
wastegate_opening:0atm



again, here is an attach image with the correct ways of my streamline and vertex velocity at the wastegate opening.
streamline.png

vertex.png

thanks again ghorrocks. i have lost my motivation before this until i see your respond toward my post. i hope this will be my new solution. i will keep update my progress in this thread as soon as my simulation is done.

[ghorrocks]

Are you still getting unrealistic efficiency?

The turbine speed probably changes when you turn on the waste gate. Have you taken that into account? Has the results you are comparing against taken that into account?

[kimie]

normally my simulation will run for 6hours or more to converge.so i cannot find the efficiency yet. i see your point about the rotation speed of rotor as i open my wastegate the rotation should decrease. But what i has done is i am running at fix 30,000 rpm speed and i trying to find the efficiency at that fix rpm. is it still reliable case?or my case has turn into false case.

[ghorrocks]

Most systems like this are set up with a turbine (with a performance curve) connected to a load (with a performance curve). Where those two performance curves intersect is the steady state operating speed of the system. If you change the turbine performance curve by putting a waste gate in then the intersection of the two curves will more to another speed.

If you have used the same speed for both simulations it means at least one of the simulations could be off the correct speed. Then the turbine will be generating too much torque (and the system will respond by speeding up to reduce the torque); or too little torque (and the system will respond by slowing down to increase the torque). But whether this effect is significant depends on how the details of the performance curves of the system.

[kimie]

actually what i am trying to do is i want to make a comparison of different wastegate area toward the turbine efficiency at fix rpm.

so i have 3 case which is from the smallest area to the biggest area.

the idea is, as the pressure inside the turbine is decrease, the torq that spin the blade should be decrease then i should have a good efficiency which the torq change.


but my previous run that has problem has give me unreliable efficiency so i guess there is something wrong because that is my first line of run.

so what i am trying to do now is i run with new reference pressure and opening pressure at 30k rpm.


what i should do next?

i should figure out to run the simulation with less rotor rpm as the wastegate is open but is it still reliable if i just put the rpm because i have no idea about the rpm value when open the wastegate.


thanks again ghorrocks

[kimie]

for now i am not comparing the result yet because my first few run has give me unreliable efficiency but i can see your suggestion which is.

for opening 1 -30k rpm

opening 2(smaller)-35k rpm

opening 3(smallest) -40k rpm

which is the rpm will decrease as my opening increase. but for now im still trying to run the fully open condition with 30k rpm.


am i still on the right path?

[kimie]

hye ghorrock. finally my first run is converge, this is my setup

input massflow rate:0.3kg
reference pressure:1atm
wastegate outlet pressure:0atm
turbine outlet:0atm
rotor speed:30,000 rpm

seems like i obtain same torque wih my previous run and my calculated efficiency also still unrealistic. i am lost now..

hoping for your response

thanks

[kimie]

now i understand what are you saying ghorrock. i assume when my wastegate is open, the pressure inside my turbine has no strengh to rotate the rotor for 30k rpm but still i set the rpm to 30k rpm. that is why the efficiency become huge because it is really too efficient to rotate the blade to this rpm point with the super lower pressure.

[kimie]

still i cant figure out how to find the best rotation speed for my case ghorrocks..

[ghorrocks]

To find the rotation speed:

Do a series of runs at different rotation speeds. This will give you a torque versus speed curve. You should have the torque versus speed curve for your load. Where the two curves intersect, that is your operating speed and load. This is the point where the turbine torque generated equals the load torque absorbed.

You will need to repeat this at each different waste gate opening.

[kimie]

Thanks you so much ghorrocks! I will try it now.you awesome!

[kimie]

Originally Posted by ghorrocks

To find the rotation speed:

Do a series of runs at different rotation speeds. This will give you a torque versus speed curve. You should have the torque versus speed curve for your load. Where the two curves intersect, that is your operating speed and load. This is the point where the turbine torque generated equals the load torque absorbed.

You will need to repeat this at each different waste gate opening.

hye ghorrocks. i have done plotting my torq vs speed for my load. the detail is down there:


i have run 2 massflowrate which is my min massflow and max massflow parameter which is 0.2kg/s and 0.8kg/s

for the massflow i have split the speed into 3 which is 6k,10k,20k rpm.


Then i realize that my graph has no intersection. this is an attach graph.

torq vs speed.png


thanks ghorrocks.

[ghorrocks]

I do not understand your graph. Please label the axes and label the curves. Is it the load or the turbine?

The load curve should increase with speed and the turbine curve should decrease with speed.

[kimie]

Originally Posted by ghorrocks

I do not understand your graph. Please label the axes and label the curves. Is it the load or the turbine?

The load curve should increase with speed and the turbine curve should decrease with speed.

hye ghorrocks.

this is the graph of torq vs rpm for variable massflow rate. i though mass flow rate is the load that you mean.


this is an attachment of the picture with the define axis.

torq vs speed for differ massflow.png



thank you soo much ghorrocks.

[kimie]

now i realize that i have misunderstand what you mean. i shold have torq curve and speed curve not torq vs speed axes. i will try again.thanks