Drag calculation and mass flow rate with angled meshes
Hi Neks, I am trying to run a simulation case similar to the turbulent channel flow case. I initially ran a simulation on the normal turbulent channel flow domain (with the geometry like the fig on the left). I used the parameter p55 in the rea file to ensure that the bulk velocity of the flow is 1 in the domain, and used the parameter p02 to set the turbulent Reynolds number, Re_tau to my required value of 180. I used the sub-routine drag_calc to find the mean shear on the wall, from which I calculated the shear stress and then the Re_tau and u_tau values. However, recently I was trying the same thing on a slightly different domain (fig to the right). --------------------------------------------------------------------- --------------------------------------------------------------------- | | / / ^ Y | | / / | | | / / |_____> X | | / / | | / / --------------------------------------------------------------------- --------------------------------------------------------------------- This domain is almost the same as the first except now there is an angle of 30 degrees in the mesh grid about the z-axis. Please note that the perpendicular distance between the walls normal to the y-direction remains the same for both the domains. In this domain if I use the same p55 and p02 parameters that I use for the orthogonal domain, then Re_tau, calculated as described above, is increasing to higher values (~220). If I reduce the parameter p55 to lesser values, then the Re_tau value is restored to 180. I could not figure out why exactly this was happening, and whether this difference is now because my way of calculating the Re_tau is not valid anymore in the angled domain. Or is the change because the mass flow rate is actually higher in the angled domain? If the case is latter, then why is the mass flow rate increasing just due to the angling of the mesh? I went through the sub-routines drag_calc, vol_flow and set_obj (to see if the integral object needs to be changed) in moderate detail, but could not figure out the reasons for this. Any help in this might be appreciated, as I want to establish the reason, so that I can trust the accuracy of the results of this simulation. Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering
Hi Pardyumna, Nek supports two fixed flow-rate modes: .prescribed flow rate .prescribed average velocity. You toggle between these modes according to the sign of parameter 54. If p54 < 0, you are prescribing mean velocity If p54 > 0, you are prescribing flow rate. The flow rate may not work in your case because of the fact that your domain "length" ( := xmax - xmin) is not the same as your periodic pitch. The mean velocity is computed is: \int u dV / \int dV and I believe that should work OK. Flow rate needs an estimate of the length of the domain Q(x) = \int_A u dA = constant (by mass conservation) Q := (1/Lx) \int_0^Lx Q(x) dx = (1/Lx) * \int_Omega u dV In your case, Lx is the periodic pitch, and not equal to (xmax-xmin). However, Nek does not know how to find the periodic pitch. It is using Lx = xmax-xmin, which is incorrect for your geometry. Which one are your using? Best, Paul ________________________________ From: [email protected] [[email protected]] on behalf of [email protected] [[email protected]] Sent: Tuesday, September 20, 2016 7:24 AM To: [email protected] Subject: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Neks, I am trying to run a simulation case similar to the turbulent channel flow case. I initially ran a simulation on the normal turbulent channel flow domain (with the geometry like the fig on the left). I used the parameter p55 in the rea file to ensure that the bulk velocity of the flow is 1 in the domain, and used the parameter p02 to set the turbulent Reynolds number, Re_tau to my required value of 180. I used the sub-routine drag_calc to find the mean shear on the wall, from which I calculated the shear stress and then the Re_tau and u_tau values. However, recently I was trying the same thing on a slightly different domain (fig to the right). --------------------------------------------------------------------- --------------------------------------------------------------------- | | / / ^ Y | | / / | | | / / |_____> X | | / / | | / / --------------------------------------------------------------------- --------------------------------------------------------------------- This domain is almost the same as the first except now there is an angle of 30 degrees in the mesh grid about the z-axis. Please note that the perpendicular distance between the walls normal to the y-direction remains the same for both the domains. In this domain if I use the same p55 and p02 parameters that I use for the orthogonal domain, then Re_tau, calculated as described above, is increasing to higher values (~220). If I reduce the parameter p55 to lesser values, then the Re_tau value is restored to 180. I could not figure out why exactly this was happening, and whether this difference is now because my way of calculating the Re_tau is not valid anymore in the angled domain. Or is the change because the mass flow rate is actually higher in the angled domain? If the case is latter, then why is the mass flow rate increasing just due to the angling of the mesh? I went through the sub-routines drag_calc, vol_flow and set_obj (to see if the integral object needs to be changed) in moderate detail, but could not figure out the reasons for this. Any help in this might be appreciated, as I want to establish the reason, so that I can trust the accuracy of the results of this simulation. Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering
Hi Paul, Thank you for your reply. I am indeed using the flow rate parameter, that is p54 > 0. From your reply, then can I assume that prescribing the mean velocity should lead to reliable results? Also it struck me when reading your reply, so I am directly asking you. If the Lx =xmax - xmin is incorrect for an angled domain, then will it in anyway affect the periodic boundary conditions. I still want the same periodic conditions, as they were in the orthogonal turbulent channel flow case (periodic about the x-axis direction). That is the velocity profile in the right-most elements should be implanted onto the left-most profile. Will this happen reliably or could there be any factors that might cause a problem? Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected] [mailto:[email protected]] On Behalf Of [email protected] Sent: Tuesday, September 20, 2016 4:04 PM To: [email protected] Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pardyumna, Nek supports two fixed flow-rate modes: .prescribed flow rate .prescribed average velocity. You toggle between these modes according to the sign of parameter 54. If p54 < 0, you are prescribing mean velocity If p54 > 0, you are prescribing flow rate. The flow rate may not work in your case because of the fact that your domain "length" ( := xmax - xmin) is not the same as your periodic pitch. The mean velocity is computed is: \int u dV / \int dV and I believe that should work OK. Flow rate needs an estimate of the length of the domain Q(x) = \int_A u dA = constant (by mass conservation) Q := (1/Lx) \int_0^Lx Q(x) dx = (1/Lx) * \int_Omega u dV In your case, Lx is the periodic pitch, and not equal to (xmax-xmin). However, Nek does not know how to find the periodic pitch. It is using Lx = xmax-xmin, which is incorrect for your geometry. Which one are your using? Best, Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 7:24 AM To: [email protected]<mailto:[email protected]> Subject: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Neks, I am trying to run a simulation case similar to the turbulent channel flow case. I initially ran a simulation on the normal turbulent channel flow domain (with the geometry like the fig on the left). I used the parameter p55 in the rea file to ensure that the bulk velocity of the flow is 1 in the domain, and used the parameter p02 to set the turbulent Reynolds number, Re_tau to my required value of 180. I used the sub-routine drag_calc to find the mean shear on the wall, from which I calculated the shear stress and then the Re_tau and u_tau values. However, recently I was trying the same thing on a slightly different domain (fig to the right). --------------------------------------------------------------------- --------------------------------------------------------------------- | | / / ^ Y | | / / | | | / / |_____> X | | / / | | / / --------------------------------------------------------------------- --------------------------------------------------------------------- This domain is almost the same as the first except now there is an angle of 30 degrees in the mesh grid about the z-axis. Please note that the perpendicular distance between the walls normal to the y-direction remains the same for both the domains. In this domain if I use the same p55 and p02 parameters that I use for the orthogonal domain, then Re_tau, calculated as described above, is increasing to higher values (~220). If I reduce the parameter p55 to lesser values, then the Re_tau value is restored to 180. I could not figure out why exactly this was happening, and whether this difference is now because my way of calculating the Re_tau is not valid anymore in the angled domain. Or is the change because the mass flow rate is actually higher in the angled domain? If the case is latter, then why is the mass flow rate increasing just due to the angling of the mesh? I went through the sub-routines drag_calc, vol_flow and set_obj (to see if the integral object needs to be changed) in moderate detail, but could not figure out the reasons for this. Any help in this might be appreciated, as I want to establish the reason, so that I can trust the accuracy of the results of this simulation. Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering
Hi Pradyumna, Periodicity is pretty robust in nek. As long as the pair of periodic faces has the same normal vector and are of the same area, then it should work. Yes - I believe that using the correct Ubar will work for you. Another point, which I discovered just last week: If you are applying a shear in usrdat2 (which would be a normal thing to do), you need to make certain you set param(59)=1 in the .usr file. This turns off the "fast" operator evaluation that is valid only for element that are proper rectilinear bricks. The code detects such bricks when they are read from the .rea file, but the mechanism uses information that is not touched by standard morphing procedures. I'm working on a fix for this, but for now you should set param(59)=1, which will turn off the fast mode. Paul ________________________________ From: [email protected] [[email protected]] on behalf of [email protected] [[email protected]] Sent: Tuesday, September 20, 2016 9:32 AM To: [email protected] Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Paul, Thank you for your reply. I am indeed using the flow rate parameter, that is p54 > 0. From your reply, then can I assume that prescribing the mean velocity should lead to reliable results? Also it struck me when reading your reply, so I am directly asking you. If the Lx =xmax – xmin is incorrect for an angled domain, then will it in anyway affect the periodic boundary conditions. I still want the same periodic conditions, as they were in the orthogonal turbulent channel flow case (periodic about the x-axis direction). That is the velocity profile in the right-most elements should be implanted onto the left-most profile. Will this happen reliably or could there be any factors that might cause a problem? Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected] [mailto:[email protected]] On Behalf Of [email protected] Sent: Tuesday, September 20, 2016 4:04 PM To: [email protected] Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pardyumna, Nek supports two fixed flow-rate modes: .prescribed flow rate .prescribed average velocity. You toggle between these modes according to the sign of parameter 54. If p54 < 0, you are prescribing mean velocity If p54 > 0, you are prescribing flow rate. The flow rate may not work in your case because of the fact that your domain "length" ( := xmax - xmin) is not the same as your periodic pitch. The mean velocity is computed is: \int u dV / \int dV and I believe that should work OK. Flow rate needs an estimate of the length of the domain Q(x) = \int_A u dA = constant (by mass conservation) Q := (1/Lx) \int_0^Lx Q(x) dx = (1/Lx) * \int_Omega u dV In your case, Lx is the periodic pitch, and not equal to (xmax-xmin). However, Nek does not know how to find the periodic pitch. It is using Lx = xmax-xmin, which is incorrect for your geometry. Which one are your using? Best, Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 7:24 AM To: [email protected]<mailto:[email protected]> Subject: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Neks, I am trying to run a simulation case similar to the turbulent channel flow case. I initially ran a simulation on the normal turbulent channel flow domain (with the geometry like the fig on the left). I used the parameter p55 in the rea file to ensure that the bulk velocity of the flow is 1 in the domain, and used the parameter p02 to set the turbulent Reynolds number, Re_tau to my required value of 180. I used the sub-routine drag_calc to find the mean shear on the wall, from which I calculated the shear stress and then the Re_tau and u_tau values. However, recently I was trying the same thing on a slightly different domain (fig to the right). --------------------------------------------------------------------- --------------------------------------------------------------------- | | / / ^ Y | | / / | | | / / |_____> X | | / / | | / / --------------------------------------------------------------------- --------------------------------------------------------------------- This domain is almost the same as the first except now there is an angle of 30 degrees in the mesh grid about the z-axis. Please note that the perpendicular distance between the walls normal to the y-direction remains the same for both the domains. In this domain if I use the same p55 and p02 parameters that I use for the orthogonal domain, then Re_tau, calculated as described above, is increasing to higher values (~220). If I reduce the parameter p55 to lesser values, then the Re_tau value is restored to 180. I could not figure out why exactly this was happening, and whether this difference is now because my way of calculating the Re_tau is not valid anymore in the angled domain. Or is the change because the mass flow rate is actually higher in the angled domain? If the case is latter, then why is the mass flow rate increasing just due to the angling of the mesh? I went through the sub-routines drag_calc, vol_flow and set_obj (to see if the integral object needs to be changed) in moderate detail, but could not figure out the reasons for this. Any help in this might be appreciated, as I want to establish the reason, so that I can trust the accuracy of the results of this simulation. Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering
Paul, I am not using the usrdat2 sub-routine for now. But in any case, I will set p59 = 1. I am only using the function ffx in the sub-routine userf. But I checked the vol_flow routine and could not find anything that should affect ffx in the angled domain. So I will keep it. Do you agree? Best regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected] [mailto:[email protected]] On Behalf Of [email protected] Sent: Tuesday, September 20, 2016 4:43 PM To: [email protected] Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pradyumna, Periodicity is pretty robust in nek. As long as the pair of periodic faces has the same normal vector and are of the same area, then it should work. Yes - I believe that using the correct Ubar will work for you. Another point, which I discovered just last week: If you are applying a shear in usrdat2 (which would be a normal thing to do), you need to make certain you set param(59)=1 in the .usr file. This turns off the "fast" operator evaluation that is valid only for element that are proper rectilinear bricks. The code detects such bricks when they are read from the .rea file, but the mechanism uses information that is not touched by standard morphing procedures. I'm working on a fix for this, but for now you should set param(59)=1, which will turn off the fast mode. Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 9:32 AM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Paul, Thank you for your reply. I am indeed using the flow rate parameter, that is p54 > 0. From your reply, then can I assume that prescribing the mean velocity should lead to reliable results? Also it struck me when reading your reply, so I am directly asking you. If the Lx =xmax - xmin is incorrect for an angled domain, then will it in anyway affect the periodic boundary conditions. I still want the same periodic conditions, as they were in the orthogonal turbulent channel flow case (periodic about the x-axis direction). That is the velocity profile in the right-most elements should be implanted onto the left-most profile. Will this happen reliably or could there be any factors that might cause a problem? Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected]<mailto:[email protected]> [mailto:[email protected]] On Behalf Of [email protected]<mailto:[email protected]> Sent: Tuesday, September 20, 2016 4:04 PM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pardyumna, Nek supports two fixed flow-rate modes: .prescribed flow rate .prescribed average velocity. You toggle between these modes according to the sign of parameter 54. If p54 < 0, you are prescribing mean velocity If p54 > 0, you are prescribing flow rate. The flow rate may not work in your case because of the fact that your domain "length" ( := xmax - xmin) is not the same as your periodic pitch. The mean velocity is computed is: \int u dV / \int dV and I believe that should work OK. Flow rate needs an estimate of the length of the domain Q(x) = \int_A u dA = constant (by mass conservation) Q := (1/Lx) \int_0^Lx Q(x) dx = (1/Lx) * \int_Omega u dV In your case, Lx is the periodic pitch, and not equal to (xmax-xmin). However, Nek does not know how to find the periodic pitch. It is using Lx = xmax-xmin, which is incorrect for your geometry. Which one are your using? Best, Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 7:24 AM To: [email protected]<mailto:[email protected]> Subject: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Neks, I am trying to run a simulation case similar to the turbulent channel flow case. I initially ran a simulation on the normal turbulent channel flow domain (with the geometry like the fig on the left). I used the parameter p55 in the rea file to ensure that the bulk velocity of the flow is 1 in the domain, and used the parameter p02 to set the turbulent Reynolds number, Re_tau to my required value of 180. I used the sub-routine drag_calc to find the mean shear on the wall, from which I calculated the shear stress and then the Re_tau and u_tau values. However, recently I was trying the same thing on a slightly different domain (fig to the right). --------------------------------------------------------------------- --------------------------------------------------------------------- | | / / ^ Y | | / / | | | / / |_____> X | | / / | | / / --------------------------------------------------------------------- --------------------------------------------------------------------- This domain is almost the same as the first except now there is an angle of 30 degrees in the mesh grid about the z-axis. Please note that the perpendicular distance between the walls normal to the y-direction remains the same for both the domains. In this domain if I use the same p55 and p02 parameters that I use for the orthogonal domain, then Re_tau, calculated as described above, is increasing to higher values (~220). If I reduce the parameter p55 to lesser values, then the Re_tau value is restored to 180. I could not figure out why exactly this was happening, and whether this difference is now because my way of calculating the Re_tau is not valid anymore in the angled domain. Or is the change because the mass flow rate is actually higher in the angled domain? If the case is latter, then why is the mass flow rate increasing just due to the angling of the mesh? I went through the sub-routines drag_calc, vol_flow and set_obj (to see if the integral object needs to be changed) in moderate detail, but could not figure out the reasons for this. Any help in this might be appreciated, as I want to establish the reason, so that I can trust the accuracy of the results of this simulation. Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering
Hi Pradyumna, If you are using p54/p55, you should set ffx (ffy,ffz) to 0. Nek will adjust the mean pressure drop to sustain your requested flow rate. You can find what this is, as a function of time, by: grep volf logfile Column 1 is step number Column 2 is time Column 3 is ffx (unless you prescribed ffx, then c2 will be ffx - what you prescribed). Paul ________________________________ From: [email protected] [[email protected]] on behalf of [email protected] [[email protected]] Sent: Tuesday, September 20, 2016 9:55 AM To: [email protected] Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Paul, I am not using the usrdat2 sub-routine for now. But in any case, I will set p59 = 1. I am only using the function ffx in the sub-routine userf. But I checked the vol_flow routine and could not find anything that should affect ffx in the angled domain. So I will keep it. Do you agree? Best regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected] [mailto:[email protected]] On Behalf Of [email protected] Sent: Tuesday, September 20, 2016 4:43 PM To: [email protected] Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pradyumna, Periodicity is pretty robust in nek. As long as the pair of periodic faces has the same normal vector and are of the same area, then it should work. Yes - I believe that using the correct Ubar will work for you. Another point, which I discovered just last week: If you are applying a shear in usrdat2 (which would be a normal thing to do), you need to make certain you set param(59)=1 in the .usr file. This turns off the "fast" operator evaluation that is valid only for element that are proper rectilinear bricks. The code detects such bricks when they are read from the .rea file, but the mechanism uses information that is not touched by standard morphing procedures. I'm working on a fix for this, but for now you should set param(59)=1, which will turn off the fast mode. Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 9:32 AM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Paul, Thank you for your reply. I am indeed using the flow rate parameter, that is p54 > 0. From your reply, then can I assume that prescribing the mean velocity should lead to reliable results? Also it struck me when reading your reply, so I am directly asking you. If the Lx =xmax – xmin is incorrect for an angled domain, then will it in anyway affect the periodic boundary conditions. I still want the same periodic conditions, as they were in the orthogonal turbulent channel flow case (periodic about the x-axis direction). That is the velocity profile in the right-most elements should be implanted onto the left-most profile. Will this happen reliably or could there be any factors that might cause a problem? Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected]<mailto:[email protected]> [mailto:[email protected]] On Behalf Of [email protected]<mailto:[email protected]> Sent: Tuesday, September 20, 2016 4:04 PM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pardyumna, Nek supports two fixed flow-rate modes: .prescribed flow rate .prescribed average velocity. You toggle between these modes according to the sign of parameter 54. If p54 < 0, you are prescribing mean velocity If p54 > 0, you are prescribing flow rate. The flow rate may not work in your case because of the fact that your domain "length" ( := xmax - xmin) is not the same as your periodic pitch. The mean velocity is computed is: \int u dV / \int dV and I believe that should work OK. Flow rate needs an estimate of the length of the domain Q(x) = \int_A u dA = constant (by mass conservation) Q := (1/Lx) \int_0^Lx Q(x) dx = (1/Lx) * \int_Omega u dV In your case, Lx is the periodic pitch, and not equal to (xmax-xmin). However, Nek does not know how to find the periodic pitch. It is using Lx = xmax-xmin, which is incorrect for your geometry. Which one are your using? Best, Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 7:24 AM To: [email protected]<mailto:[email protected]> Subject: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Neks, I am trying to run a simulation case similar to the turbulent channel flow case. I initially ran a simulation on the normal turbulent channel flow domain (with the geometry like the fig on the left). I used the parameter p55 in the rea file to ensure that the bulk velocity of the flow is 1 in the domain, and used the parameter p02 to set the turbulent Reynolds number, Re_tau to my required value of 180. I used the sub-routine drag_calc to find the mean shear on the wall, from which I calculated the shear stress and then the Re_tau and u_tau values. However, recently I was trying the same thing on a slightly different domain (fig to the right). --------------------------------------------------------------------- --------------------------------------------------------------------- | | / / ^ Y | | / / | | | / / |_____> X | | / / | | / / --------------------------------------------------------------------- --------------------------------------------------------------------- This domain is almost the same as the first except now there is an angle of 30 degrees in the mesh grid about the z-axis. Please note that the perpendicular distance between the walls normal to the y-direction remains the same for both the domains. In this domain if I use the same p55 and p02 parameters that I use for the orthogonal domain, then Re_tau, calculated as described above, is increasing to higher values (~220). If I reduce the parameter p55 to lesser values, then the Re_tau value is restored to 180. I could not figure out why exactly this was happening, and whether this difference is now because my way of calculating the Re_tau is not valid anymore in the angled domain. Or is the change because the mass flow rate is actually higher in the angled domain? If the case is latter, then why is the mass flow rate increasing just due to the angling of the mesh? I went through the sub-routines drag_calc, vol_flow and set_obj (to see if the integral object needs to be changed) in moderate detail, but could not figure out the reasons for this. Any help in this might be appreciated, as I want to establish the reason, so that I can trust the accuracy of the results of this simulation. Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering
Paul, Thank you I will do that. Best regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected] [mailto:[email protected]] On Behalf Of [email protected] Sent: Tuesday, September 20, 2016 5:48 PM To: [email protected] Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pradyumna, If you are using p54/p55, you should set ffx (ffy,ffz) to 0. Nek will adjust the mean pressure drop to sustain your requested flow rate. You can find what this is, as a function of time, by: grep volf logfile Column 1 is step number Column 2 is time Column 3 is ffx (unless you prescribed ffx, then c2 will be ffx - what you prescribed). Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 9:55 AM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Paul, I am not using the usrdat2 sub-routine for now. But in any case, I will set p59 = 1. I am only using the function ffx in the sub-routine userf. But I checked the vol_flow routine and could not find anything that should affect ffx in the angled domain. So I will keep it. Do you agree? Best regards, c From: [email protected]<mailto:[email protected]> [mailto:[email protected]] On Behalf Of [email protected]<mailto:[email protected]> Sent: Tuesday, September 20, 2016 4:43 PM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pradyumna, Periodicity is pretty robust in nek. As long as the pair of periodic faces has the same normal vector and are of the same area, then it should work. Yes - I believe that using the correct Ubar will work for you. Another point, which I discovered just last week: If you are applying a shear in usrdat2 (which would be a normal thing to do), you need to make certain you set param(59)=1 in the .usr file. This turns off the "fast" operator evaluation that is valid only for element that are proper rectilinear bricks. The code detects such bricks when they are read from the .rea file, but the mechanism uses information that is not touched by standard morphing procedures. I'm working on a fix for this, but for now you should set param(59)=1, which will turn off the fast mode. Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 9:32 AM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Paul, Thank you for your reply. I am indeed using the flow rate parameter, that is p54 > 0. From your reply, then can I assume that prescribing the mean velocity should lead to reliable results? Also it struck me when reading your reply, so I am directly asking you. If the Lx =xmax - xmin is incorrect for an angled domain, then will it in anyway affect the periodic boundary conditions. I still want the same periodic conditions, as they were in the orthogonal turbulent channel flow case (periodic about the x-axis direction). That is the velocity profile in the right-most elements should be implanted onto the left-most profile. Will this happen reliably or could there be any factors that might cause a problem? Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering From: [email protected]<mailto:[email protected]> [mailto:[email protected]] On Behalf Of [email protected]<mailto:[email protected]> Sent: Tuesday, September 20, 2016 4:04 PM To: [email protected]<mailto:[email protected]> Subject: Re: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Pardyumna, Nek supports two fixed flow-rate modes: .prescribed flow rate .prescribed average velocity. You toggle between these modes according to the sign of parameter 54. If p54 < 0, you are prescribing mean velocity If p54 > 0, you are prescribing flow rate. The flow rate may not work in your case because of the fact that your domain "length" ( := xmax - xmin) is not the same as your periodic pitch. The mean velocity is computed is: \int u dV / \int dV and I believe that should work OK. Flow rate needs an estimate of the length of the domain Q(x) = \int_A u dA = constant (by mass conservation) Q := (1/Lx) \int_0^Lx Q(x) dx = (1/Lx) * \int_Omega u dV In your case, Lx is the periodic pitch, and not equal to (xmax-xmin). However, Nek does not know how to find the periodic pitch. It is using Lx = xmax-xmin, which is incorrect for your geometry. Which one are your using? Best, Paul ________________________________ From: [email protected]<mailto:[email protected]> [[email protected]] on behalf of [email protected]<mailto:[email protected]> [[email protected]] Sent: Tuesday, September 20, 2016 7:24 AM To: [email protected]<mailto:[email protected]> Subject: [Nek5000-users] Drag calculation and mass flow rate with angled meshes Hi Neks, I am trying to run a simulation case similar to the turbulent channel flow case. I initially ran a simulation on the normal turbulent channel flow domain (with the geometry like the fig on the left). I used the parameter p55 in the rea file to ensure that the bulk velocity of the flow is 1 in the domain, and used the parameter p02 to set the turbulent Reynolds number, Re_tau to my required value of 180. I used the sub-routine drag_calc to find the mean shear on the wall, from which I calculated the shear stress and then the Re_tau and u_tau values. However, recently I was trying the same thing on a slightly different domain (fig to the right). --------------------------------------------------------------------- --------------------------------------------------------------------- | | / / ^ Y | | / / | | | / / |_____> X | | / / | | / / --------------------------------------------------------------------- --------------------------------------------------------------------- This domain is almost the same as the first except now there is an angle of 30 degrees in the mesh grid about the z-axis. Please note that the perpendicular distance between the walls normal to the y-direction remains the same for both the domains. In this domain if I use the same p55 and p02 parameters that I use for the orthogonal domain, then Re_tau, calculated as described above, is increasing to higher values (~220). If I reduce the parameter p55 to lesser values, then the Re_tau value is restored to 180. I could not figure out why exactly this was happening, and whether this difference is now because my way of calculating the Re_tau is not valid anymore in the angled domain. Or is the change because the mass flow rate is actually higher in the angled domain? If the case is latter, then why is the mass flow rate increasing just due to the angling of the mesh? I went through the sub-routines drag_calc, vol_flow and set_obj (to see if the integral object needs to be changed) in moderate detail, but could not figure out the reasons for this. Any help in this might be appreciated, as I want to establish the reason, so that I can trust the accuracy of the results of this simulation. Thanks and regards, Pradyumna M K Prasad TU Delft, Student: Masters in Aerospace Engineering
participants (1)
-
nek5000-users＠lists.mcs.anl.gov