Negative Pressure Observed before outlet

  • Last Post 31 January 2018
bushrar posted this 10 January 2018


My simulation consists of material flowing down a barrel to a contraction to  counterbore and then through a capillary. 

Pressure at the capillary outlet is supposed to zero, since flow is directed downstream, which was even observed with the resulting vectors.  However it dropped to a negative pressure at the outlet (z=1.5mm).

I used adaptive sizing, and set element size to 0.0075 mm.  Using this , I obtained fairly accurate shear rates and velocities.  I was wondering what changes could be made to make sure the pressure drops to 0 at the lowest.

Order By: Standard | Newest | Votes
Raef.Kobeissi posted this 10 January 2018

Hello, Before answering why is has dropped below 0 may I ask you this:

  • How did you collect this pressure data? Is it from a vertical line ?
  • what are your boundary comditions?
  • Did you check the average pressure at the outlet ? Is it 0?
  • is there any backflow ? Any eddies near the line you took?
  • can you attach a pressure and velocity contour ?

Best Regards

Raef Kobeissi

bushrar posted this 11 January 2018

(Part 1)

Mr. Kobeissi, 

I did collect pressure data vertically starting from the top of the barrel to the end of the capillary (Figure 1- shown with a red line).  The points are located at the intersection of the planes of symmetry [(0,0,-1.9) to (0,0,1.6)].

Figure 1: 3-D Pressure contour 

By "average pressure at the outlet", are you referring to various points at the cross section of the outlet (Figure 2)?  

Figure 2: 3-D Pressure contour-outlet cross section



bushrar posted this 11 January 2018

(Part 2):  Velocity

There is no back flow or eddies around the capillary area as indicated by vector and contour (Figures 3 and 4 respectively) 

Figure 3

Figure 4


bushrar posted this 11 January 2018

(Part 3) Boundary Conditions

Inlet: Volumetric Flow rate- Q=2.0837e-9 m3/s

Planes of Symmetry


outlet: fn=fs=0

Raef.Kobeissi posted this 12 January 2018

Hello, At the bottom (Capillary area) and based on the velocity contour there is an area with very high velocity due to the narrowing of the channel. This could be causing. Negative pressure area. In general I would say your average pressure at the outlet is indeed zero but it is gradient due to the narrowing of the channel and high velocities at the edge. Yes when I say average pressure I mean the cross section at the outlet. I believe what you’re seeing is normal. More mesh refinement will probably enhance your result. If you calculate the pressure outlet using the a erage function or average are favet for static pressure you will discover that it will be zero in average.

Raef Kobeissi

bushrar posted this 12 January 2018

For mesh refinement, I started off with sweeping around the capillary as well as creating 20 edge divisions at the outlet.  For global parameters, I used adaptive meshing with an element size of 0.0075 mm.  This is total yielded around 2.5 million elements,  compared to the 2 million elements yielded from using only adaptive meshing.  

However, not much of a difference was observed with the addition of sweeping and edge divisions alone.

Are there any other suggestions as to how I can refine the mesh to yield a zero average pressure? 

bushrar posted this 16 January 2018

Update:  I tried inflation layers on conical convergence and capillary (together and separately), which produced a failed mesh

peteroznewman posted this 16 January 2018

Sometimes if you Generate Mesh, you will get a failed mesh, but if you selectively mesh each body from one end to the other, it might succeed. Start at the end that has the capillary and work you way up.

Raef.Kobeissi posted this 16 January 2018

As long as the averaged outlet face is zero pressure I believe you’re doing the right thing. It is expected to have negative pressure in the narrow area.

Raef Kobeissi

bushrar posted this 18 January 2018

It keeps failing even after selectively meshing the bodies.  In this case I attempted it with half the capillary body 

raul.raghav posted this 18 January 2018

Attached is the workbench file and geometry with the meshing done for your geometry. A few slices in the geometry to make a hexa mesh with sweeping and some edge sizing. Not sure if it would help you solve the issue but you can atleast rule out the mesh as a possible cause. Attached is a screenshot of the mesh:



Attached Files

  • Liked by
  • peteroznewman
  • bushrar
bushrar posted this 24 January 2018

Thank you raul.raghav!


I'll be sure to run it to see if we can rule that out

Raef.Kobeissi posted this 30 January 2018

Any update Bushrar? Cheers

Raef Kobeissi

bushrar posted this 31 January 2018

Raul Raghav,


My apologies for the delay in updates.  I just ran your geometry and mesh through Fluent and the pressure contours showed a clean, uniform cross section .  


Additionally, the outlet pressure was not negative, but still not zero.  However, the outlet pressure is about 1.6% of the pressure at top of the capillary.

As far as the issue with the pressure drop is concerned, your mesh showed more success than mine.  On your space claim file I was wondering where I could find your geometry dimensions and the planes you created to make those slices.

Thank you very much!




raul.raghav posted this 31 January 2018

Bushra, I had to make the geometry from the image you posted. I could have got the dimensions wrong but attached is the spaceclaim geometry that I used to make the mesh. Please verify the dimensions with what you have.

And why has the pressure changed from an order of 10^-3 to 10^-7? Can you comment on that? And you also attach the z_velocity contour?


Attached Files