# In CFX and Fluent, is "mass flow" set under normal or operating conditions?

 Register Blogs Members List Search Today's Posts Mark Forums Read

 September 28, 2020, 09:37 In CFX and Fluent, is "mass flow" set under normal or operating conditions? #1 New Member   Ilya Join Date: Oct 2019 Posts: 5 Rep Power: 4 Hello. Please tell me in CFX and Fluent "mass flow" (kg / s) on the input boundary conditions tab is asked under normal or operating conditions? For a liquid, this is not usually important. It is very important for gas.

 September 28, 2020, 09:42 #2 Senior Member   Join Date: Jun 2009 Posts: 1,471 Rep Power: 27 Not clear what you are asking. You can select several options at inlet boundaries. It is your decision. The first option is just a default, not a requirement. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 September 28, 2020, 09:43 #3 Senior Member   Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,388 Rep Power: 21 Mass is the amount of kilograms per second. In either normal or operating conditions. Since the software cannot read your mind, it is you to tell what the conditions are, by setting the reference pressure and inlet temperature.

 September 29, 2020, 02:50 #4 New Member   Ilya Join Date: Oct 2019 Posts: 5 Rep Power: 4 Thanks. I understood like this: Given: Volumetric gas flow rate under standard conditions (temperature 25 °C, pressure 1 atm). Task 1: Determine the mass flow rate at a temperature of 50 °C and a pressure of 10 atm in the apparatus. Task 2: Enter the obtained mass flow rate into the ansis. Solution step by step: Step 1. Recalculate the volumetric flow rate (m3/s) in Excel under operating conditions (temperature 50 °C, pressure 10 atm). Step 2 Recalculate in Excel the mass flow rate (kg/s) according to the obtained volumetric flow rate under operating conditions in the previous step. Step 3: Enter the obtained mass flow rate into the ansis. Let it be useful to someone.

 September 29, 2020, 04:29 #5 Senior Member   Gert-Jan Join Date: Oct 2012 Location: Europe Posts: 1,388 Rep Power: 21 I can't follow your thoughts. I'm blinded by 25 years of CFD experience. In CFD, you either set massflow and temperature (or velocity) on inlet and zero pressure on the outlet. Absolute pressure is determined by the sum of pressure in your domain and reference pressure. Using these settings, you get the pressure on the inlet required to get the massflow through you geometry. Alternatively you set an inlet pressure (and temperature) and CFD will give you the massflow in line with the pressure difference you set. So, if you have standard conditions, you set: - reference pressure on 1 atm, - outlet pressure 0 Pa - inlet mass flow and temperature The outcome will be pressure required to get the massflow through at that condition. You can repeat the calculation at elevated conditions by increasing the reference pressure and elevated inlet temperature. Then with the same mass flow, the outcome will be pressure required to get the massflow through at that condition. If you are not satisfied with the outcome, you can increase or decrease the massflow to get the inlet pressure you want. Alternatively, you set the inlet pressure and you get the massflow as a result. It is just a matter of trial and error.

 September 29, 2020, 09:48 #6 Senior Member   Join Date: Jun 2009 Posts: 1,471 Rep Power: 27 I think I now understood the question. Let me rephrase it as Are the inlet conditions using local conditions, or the operating conditions as stated in Fluent (CFX does use such vocabulary)? The concept of operating conditions in Fluent, or Reference Pressure in CFX, is used to determine a level for shifting values in order to control numerics. In theory, the engineering solution should be independent of any operating conditions settings used. The answer for the original question is: the boundary conditions is always evaluated using local conditions. Just be careful that the input values must be consistent with the operating conditions. Example using CFX, if you set your domain Reference Pressue to 1 atm, all your boundary absolute pressure values must be expressed as gauge pressure, i.e. Relative Pressure = MyTrueAbsPresValue - Reference Pressure If your Reference Pressure is set to 0 [any], your Relative Pressure is your Absolute Pressure. There is no need to recompute your inlet conditions using the algorithm you described. Hopefully I understood the question correctly this time around. __________________ Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.

 Tags cfx, conditions, fluent, mass flow