CFD Pressure Results reasonable at early iterations but not at convergence autostop of iterations

[patrick.droste]

CFD Objective: Pressure Drop prediction of strainer 

Current Results:

Analysis at Iteration 20: reasonable results (pressure closer within limits)

Analysis at Iteration 315: not reasonable results. (pressure at orders of magnitude to high) 

Screen shots attached below along with CFD share file. 

Not sure what is causing the jump in analysis or root cause of issue 

Attached screen shots and CFD share file

Any help would be great

Regards

[karol.suchon]

Hello Patrick,

Around the 20 iterations, the value of the pressure generates a very high pick around the outlet where you apply the pressure BC.

Probably the average pressure value is in the proper range but the picks just give us an improper view.

I will refine the mesh on the outlet and will let you know if that helps to avoid the pick of pressure.

Best regards,
Karol

[karol.suchon]

The pressure pick on the outlet is connected with the forced flow at the outlet, even if we apply the fully developed flow there could be some issues with the pressure at the outlet. I think that you just could ignore them and set the specific range of the pressure field using 0 as a maximum and the average pressure value near the outlet. Just create the plane plot and set it near the outlet and compute the average pressure using a bulk calculator.

There is a different issue which has a much higher influence on the results, you have a very small velocity in the simulation so the Reynolds number will be very low. In that case, I am sure that flow will be laminar, not turbulent in the entire domain. Pure laminar flow generates a few times lesser pressure drop. Do you have some test data from similar projects to get more info which value will be true ?

Best regards,

Karol

[patrick.droste]

Thank you for looking into this, Karol. I don't have any empirical data for this design; but, based on the viscosity for this fluid I ran the model as laminar. I also ran the CFD study with the flow boundry check box "checked" and "unchecked" for fully developed......didn't seem to make a difference. 

I've attached another screen capture with markings to make sure our terminology is matching....in case the CFD share file didn't transfer correctly or something.  

In reference to the attached picture why is there an abrupt change in velocity near the end of the outlet? is there some incorrect setting or geometry I am missing.  

Appreciate the help.

Thanks again,

Patrick 

[karol.suchon]

If we apply the forced flow at the outlet software needs to recalculate the outlet velocity profile( the flow is straightened even if we apply the fully developed flow). IN most cases that do not generate the issue and the pressure picks are rather small but you have a very low velocity with extremely high viscosity, which generates the issue.

In your case, we should exchange the boundary conditions side( inlet volume flow rate on the inlet and the pressure on the outlet) but on the inlet, you also do not have uniform velocity.

We should use the double pressure boundary conditions which you want to get from the simulation or just ignore the pressure picks. I tried a few different meshes but I always get a high negative value near the outlet.

Please use the workflow to assign the minimum and maximum value of the pressure on the scale and look if the results are reasonable.

• Create the plane plot near( +- more than 1 mesh element from the outlet) the measure the pressure value.

• Click on the scale by RMC and click set to part and use the body where are the holes( the pressure will be the highest here.

• At the end edit the scale and set a minimum value equal to the value computed from the plane.

I know that is rather a painful approach but forced flow on the outlet, high viscosity and FEM is an exploding mixture 🙂

You could also get the value from the plane and apply the minus pressure on the outlet. That will be the best way to avoid the picks.

Best regards,

Karol