How can I identify pressure behavior across a manifold

[Meriem_Boukhaima]

Dear experts.

I am designing a manifold in which a given the flow rate at 1 bar pressure at inlet would create vaccum due to high turbulence on the small outlet inside the manifold (see attached). if no vacuum is created in the region in circle. then I will have to modify the angle of the small outlet so it creates a vacuum. I need help on how I can use CFD to get to the right design. 

Thanks in advance!

[marwan_azzam]

I would assign either flow rate or pressure at inlet.  Zero pressure at outlet, then look at the pressure profile.

A cut plane would probably give you a better view of the pressure inside.  Maybe also an iso-volume of pressure.

Marwan

[Meriem_Boukhaima]

Hi Marwan,

Thanks for your quick reply!

I did a test. so if I set -0.5 bar pressure at the small oultet. I get a 53 bar inlet pressure. does that mean if I apply 53 bar of pressure at inlet I will get vacuum at the small outlet?
I hope you can read my attachment

Thanks for your support!

[bob.schlosser]

In addition to what Marwan mentioned, you will also need a boundary condition on the inlet portion of your vacuum tube.  I modeled up a similar part and used the 'unknown' boundary condition and it seemed to work.  I'd be interested if there is a better way to do this.  

This setup will likely be highly mesh dependent.  I would use a couple mesh refinement zones around the 'vacuum tube' and increase the wall layers to 10.

[marwan_azzam]

Bob is right.

You need to boundary conditions on both inlet and outlet.  It does seem that it would be an unknown at the outlet unless it goes out far enough that we know it's Pressure = 0.

There is no model attached to any post.

If you want to send a cfz file you need to zip it first and post the zip file.

Marwan

[bob.schlosser]

Attached my set up.  I just threw this together to see if the set up was giving flow in the correct directions.  

[bob.schlosser]

You could replace the flow boundary condition on the inlet with a pressure if you want.

[marwan_azzam]

Bob, your model would have positive pressure at the unknown surface and it behaves as an outlet.

It would be interesting to see the OPs model.

Marwan

[Meriem_Boukhaima]

Thanks a lot guys!

I will set the small outlet boundary condition as unknown. same as Bob's. just to give you an idea of what I am doing. see attached. appreciate your guidance!

Flow at inlet: 40-100lpm

Flow at small outlet : 0.1-2 lpm

Pressure at inlet: 0.1 – 2 bar

[bob.schlosser]

Remove the 'unknown' boundary condition from your inlet.  

Is the small tube closed off on the outside surface or is fluid allowed to flow across that boundary surface?  If fluid can not flow through that surface do not put a boundary condition on it.  I'm assuming the oil in your model is meant to be pulled through the small tube from some other reservoir?  If it is closed off like a sensor plugging the hole their is no need for a boundary condition.  Both conditions yield results of approx 3.3 (open tube) and 3.15 (Closed tube) bar near the outside surface.

[Meriem_Boukhaima]

Hello Bob,

The small tube would be connected to a tank. my target is that the oil flows from the inlet to outlet while creating a vacuum in the little outlet so there would no fluid back to the tank connected to the small outlet. I would like to validate the design with different tube angles and which one is optimal. now the problem is, whenever I set the big and small outlets to 0 bar pressure. the result I get converges to 0 so if I apply 2 bar pressure at inlet, the outlet pressure would be around 0 which is a misleading. I need some support on how I can set the boundary conditions on this software. appreciate your help!

[Meriem_Boukhaima]

another thing I have noticed. How can ISO VG 68 oil have a viscosity of 5 cp at 10C? could the database be wrong?

[bob.schlosser · Accepted solution]

Start with what you know to be true about the system. For a moment, think of this as a straight pipe without the angled inlet. Pressure difference from one end of the pipe to the other drives the fluid to flow from high pressure to low pressure. The software will solve for either the flow rate of the fluid if you know the pressure difference or the pressure difference if you know the flow rate. If you specify both it it creates a contradiction. Similar to A+B = 10. If A is 3 then B can be solved to be 7. If you specify A =3 and B =6 it doesn't work. All this is to point out that your latest model is over constrained.

If you know the flow, place a flow boundary condition on your inlet. The outlet opposite would have your P=2. The small angled surface that you want to check if it is an inlet would be the 'unknown' boundary condition. This is all you need for flow.

A couple of side comments. The material data for the oil is showing poise, not centipoise. Always verify any material data. You can create custom materials if needed. Second, is set the material to variable or it won't use the table to change viscosity by temperature. Either enable 'heat transfer' in the solver or change the overall environmental conditions in the same window that you change to variable material.

[Meriem_Boukhaima]

Thanks Bob! you're champ!  it finally works!

[Meriem_Boukhaima]

Hi Bob,

I'm not sure if I am doing things right.

see below cross section:

so first I set up the below boundary conditions:

Fluid ISO VG 68

1: pressure 1 bar gage - temp: 70C

2: unknown

3: 100lpm  direction out

results:

negative pressure at the angled tube -0.34 bar (which is great news for me and that's what I want to achieve)

0.24 pressure drop

Now I have switched the boundary conditions from 3 to 1 as per below:

same fluid

1: flow: 100lpm

2: unknown

3: pressure 0.76 bar

result: 

pressure at zone 1 was around 1 bar which is ok but pressure at zone 2 was 0.5 bar positive. I am not sure what happened here. which method is right?

Thanks again for guiding me!

[bob.schlosser]

Something doesn't look right in the graph.  Velocity or pressure shouldn't have a large step change across the pipe like it shows in your picture.

[Meriem_Boukhaima]

Hi Bob,

The colors refer to the change in static pressure.  I have attached a copy of my simulation. I calculated 3 points:

point 1: inlet

point 2: small tube

point 3: outlet.

As you can see the inlet and outlet pressures are similar however, the two configurations have resulted in two different pressures inside the tube. I want to understand why?

Please steer me in the right direction.