Assigning pressure to closed fluid domains
 

Hi All,

I have what is basically a torque converter, and would like to explore the effect of charge pressure on performance. Basically the fluid is filled into the cavity of the geometry at 500kPa before it starts running. I have tried 2 things mainly to simulate this. One is to assign 500kPa to the reference pressure in the domain settings, and the other is to assign it to the initialization. Neither seem to have the effect my fluid dynamics judgement would suggest they have.
When I do this i get the warning at the start of a run:
Domain Group:rotor

Pressure has not been set at any boundary conditions.
The pressure will be set to 0.00000E+00 at the following location:
Domain: Rotor
Node: 1 (equation 1)
Coordinates:.......

This leads me to strongly believe I am certainly not simulating the 500 kPa charge pressure.

Is the simulation incompressible or compressible?

Incompressible

So that means the absolute pressure level makes no difference, and the flow field is just offset from the reference pressure.

To model the effect of pressure on the model, you need to include some physics which depend on pressure. Maybe the flow cavitates? Or is slightly compressible? Or some other physics dependant on pressure?

Until you find some physics which depends on pressure nothing will change as you change the reference pressure level.

I see what you're saying. That is definitely what it does, just offsets from the pressure of reference. I suppose the only thing I can do is model in the inlet to that initially charges the domains, but since it is not periodic all the way around the device I would likely have to model the entire device instead of just one period.

I do not understand your comment. If the flow is perioidic then you should be able to use a periodic boundary, regardless of pressure level.

But again, what physics is dependant on pressure? If you have no physics dependant on pressure then nothing will happen in this model either.

Yea, I see how it was confusing.
The periodic issue was having to do with modelling just one blade passage of the rotor and stator. The fluid is pumped in from ports that are not fully around the item so you could not employ any sort of geometric symmetry or periodicity if you would want to model in this the ports with their boundary condition pressure condition.

OK, so the flow is not periodic. But as it now seems you have inlets and outlets then is it not a trivial matter to assign it any pressure you like?

Why are you getting an unassigned pressure warning? Surely you have a pressure boundary in your model.

Did you find a solution
 

Hi, I am also modeling torque converter and I received the same pressure warning message. Did you find a solution to assign charge pressure?

Thanks in advance for help.

Aladdin,

I hope what I have learned helps as the problem was quite easy to resolve once I understood the torque converter, not just the fluid physics....
In the torque converter the fluid is incompressible, unlike a retarder for example, since there is no cavitation. What this means is that the determinant of torque is not the pressure everywhere in the domain, but is simply the ratio of pressure of on the blade pressure vs. suction side. So having flow thru the torque converter, or trying to get pressure up inside does not change the torque number. This can be demonstrated by looking at performance curves for the converter and noticing that once enough pressure is applied to fill the domain, additional pressure does not increase performance.
This is also verified by several published papers I found from Chrysler, Komatsu, GM, and Mercedes. It is working well for my applications as well which has built confidence.
Basically you can ignore that warning, and only worry about initial or input pressure to the domain if things like cavitation are going to be significant.

A small but important point - No, not the ratio but the pressure difference over the blade.

Thanks
 

Thank you for your reply.

I have a study paper titled "COMPUTATIONAL FLUID DYNAMICS ON TORQUE CONVERTERS – VALIDATION AND APPLICATION" that shows a figure of pressure distribution along torque converter parts at charge pressure 40 psi and different pump speeds . How can I simulate this pressure? and how can I check the charge pressure value for my simulation?

If the flow is incompressible in a closed domain the reference pressure is irrelevant. You can add any amount you like to it to get the reference pressure you want.

Thanks Glenn Horrocks . Does this mean in CFX simulation of torque converter I define the value of reference pressure equal to the value of charge pressure?

I am not an expert in torque converter design so do not know what charge pressure is - but if that is the base pressure of the device then yes, that would be a good reference pressure.

Charge pressure is a tricky thing in torque converters. It is going to be dependent on how and where it is measured, and its only real use is to ensure the cavity is filled. When at 40 kPa the entire domain may not be filled due to cooler flow path, but at 180 kPa it is, and as you increase pressure you do not change performance.
Charge pressure may be measured at a wall on the pump hub, or sometimes even at the stator shroud. So one company's charge pressure is not relatable to another necessarily. The charge pressure is really only modulated by one control, and that is mass flow the cooler pump sends in. Beyond that, the factors of cooler pressure drop, RPM, none of those are variables used to control this charge pressure.

Thank you all for your reply.

Torque Converter charge pressure again
 

Hi all. I changed reference pressure in modelling a torque converter in CFX, the output torque on all elements did not change. Do you have any suggestions to order to model charge pressure?

It is a good thing the charge pressure did not change the performance, that is physically real. The only scenario where your performance should change with changing pressure is if you have cavitation or significant air entrainment. Neither of these is significant in a fully functioning torque converter.

If you do have an odd situation that has compressible flow issues or works with a partially filled TC you will need to simulate the inlet/outlet conditions. Most TC's are periodic, so you can keep one blade passage, and you will need mass flow rate in and pressure out. This will likely be very difficult to obtain.

Thank you for your quick reply.
I think I'll go with modeling partially filled torque converter. I am doing a PhD research and my supervisor thinks that one of the unknown problems in torque converters is partially filled torque converter performance.

Ahh, makes alot more sense now why that would be of interest. That does have an impact on performance since the centrifugal force means fluid is only going to act on a smaller percentage on the blade (near the hub). Also, it might not be a bad idea to turn on bouyancy in that case as gravity may or may not have a significant impact at certain RPM's.
Generally the inlet/outlet is near the shaft for the turbine, with the inlet being generally on the pump side between stator and pump passage, and outlet being between turbine and stator passage. Periodic, so that helps alot, and you could use a "reasonable" set of boundary conditions to generate something like a matrix of solutions. 70-80 liters/min is a reasonable volume flow thru the TC, outlet pressure, hmmm, not 100% certain of that, but I guess you can take reasonable numbers like 50-90 psi and see what happens when paired with different inlet conditions.

In your opening, Do I make pump inlet as an Inlet boundary condition with mass flow rate and stator exit as Outlet boundary condition with pressure or what do you think?

The entrance and exit of the TC occurs at the hub (outer portion of the torus), but not towards the core/shell. Placing an inlet domain just on the hub in a small slit between stator/pump and outlet just on the hub between turbine/stator will work. This will be roughly perpendicular to the flow path within the TC.

Your suggestion is a slit between the pump and stator as an inlet and an outlet on turbine hub. Why on hub? and how this is will be created in mesh?

This image may help:
http://www.google.com/imgres?hl=en&s...,r:6,s:0,i:160

The fluid enters between transmission case and the pump (near where they meet). Fluid exits down from turbine/stator intersection between the transmission input shaft and transmission case. The basic device is called a ground sleeve. This allows fluid to come in and out at via the same central area, but in different channels. This is important for cooling.

As for meshing. If you are using bladegen/blade editor and turbogrid you can create inlet and outlet blocks by moving the pyramid shaped delimiters.
If you are not using turbogrid with bladegen/blade editor I HIGHLY reccomend using it. But if you aren't, then I assume you have an extracted fluid domain from a cad program. This will work fine, although not as efficiently. You will have to slice off a bit of a chunk at the stator to pump and turbine interfaces, make sure they are periodic and rotating with their respective turbine/stator/pump domain, but make the hub side of these blocks and inlet and then outlet condition as appropriate. How you do this depends on the CAD program, i.e. using perhaps planes or a sketch/extrude like in NX. You will have to play with this. Unfortunatly, getting good at manipulating CAD seems to be an important part of being a CFD analyst.

I am actually using bladegen and turbogrid. Do blocks can be created in bladegen? I have no experience with doing this. I think I'll go with creating a CAD part and insert it between torque converter parts.

It's actually fairly easy in turbogrid. I'll do my best to explain how to create these blocks so that you can have faces to apply inlet/outlet without disrupting the flow. If I fail to clarify anything there are a few turbogrid experts at CFX who can help you.

Basically once you export your points to turbogrid and open it up you will see at the inlet/outlet boundaries (really the interfaces between the TC components) that there are white pyramid shaped objects. If you drag these they will follow the hub/shroud lines and make a cut in the domain. These will be your inlet/outlet blocks.

These will need to be meshed, so when you go into your mesh definition control panel (or whatever its called) you will have to click on inlet/outlet domain. The last tab on that menu box will allow you to change the mesh conditions in these domains if you so wish.

I think I got it. I'll try it and keep you updated. thanks for your comments. They are very helpful.

This might be late reply. Can you please post the image of torque converter modeling with inlet and outlet. I am using bladegen and turbogrid and I cannot make inlet/outlet in turbogrid.

Closed domain compressible flow simulation
 

What if the closed domain consists of air at reduced pressure initially say 0.4 bar and I am charging it with air at 21 bar ? In that case how do I fill the closed domain with air at the specified pressure (do i just patch the values of pressure and temperature in that domain and that does the job?)

Over that pressure range I do not think you will be using the incompressible fluid assumption. So my comments from the previous post do not apply.

You would have to have to explain what you are trying to do before I can answer your question on how to model it. But please start a new thread to ask this question, it is a different question to this thread.