# CFD Post: Difference between calculated surface values using different methods

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

 July 7, 2013, 06:16 #2 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,669 Rep Power: 84 I have heard of problems with the force and torque calculations before but have never got to the bottom of it, so I do not know the cause. It might be a bug in CFD-Post. I would report it to ANSYS support.

 July 7, 2013, 15:00 #3 Senior Member   Join Date: Dec 2009 Posts: 129 Rep Power: 10 same here Glenn, mention of it but never really researched in depth. I do know accurate torque calculation is sensitive to mesh quality/density and currently seeing how sensitive it is to yplus levels (boundary layer resolution). Plot the Force on the blade surface and set range to local. If you notice localized spikes in the force you may need to refine your mesh. Plot the mesh lines and it will be apparent. Plot the pressure the same way and it is typically smooth in contrast. I am curious, are you using blade1 as the location for the contour or something else? Maybe a bit off topic, but one may need to check the following, because there is an expert parameter necessary during the solver if a reference pressure is used. It will print in the out file when reviewed it carefully. Pressure integrals exclude the reference pressure. To include it, set the expert parameter 'include pref in forces = t'.

 July 7, 2013, 15:29 #4 Senior Member   Join Date: Dec 2009 Posts: 129 Rep Power: 10 just opened and checked torques on a blade. Created Surface Group from mesh regions for the blade. Torque on Surface Group 1 torque_z_Coordinate Frame 1()@Surface Group 1 -0.114972 [N m] Created two Contours using Surface Group 1 as location: One with 2 levels, other with 5 levels. Wrote some expressions torque_z_Coordinate Frame 1()@Surface Group 1 - torque_z_Coordinate Frame 1()@User Surface 0 = -0.000747375 [N m] (so small difference) then torque_z_Coordinate Frame 1()@User Surface 0 - (torque_z_Coordinate Frame 1()@User Surface 1 + torque_z_Coordinate Frame 1()@User Surface 2 + torque_z_Coordinate Frame 1()@User Surface 3 + torque_z_Coordinate Frame 1()@User Surface 4) = -9.68575e-008 [N m] So difference between the User Surfaces created from the contour is minimal. difference between the Surface Group of mesh regions and User Surface from single contour level, minor difference for my calculation. Difference between the sum of individual torques for the mesh regions compared to the Surface Group = 0.0 (no difference). so my question remains, what surface/s is being used for the contour.

July 7, 2013, 16:19
#5
Member

Shawn
Join Date: Oct 2011
Posts: 56
Rep Power: 5
blade1 is being used as the location for the contour, after which I've selected the user surface to use contour #2 from that contour. There do not appear to be any discontinuities in the plot of Force Y on the surface of blade 2. However, there is something wonky going on near the symmetry plane.

In the attached images, blade1 is green, blade3 is blue and blade 2 has a contour plot of Force Y.

This is for a vertical axis turbine. A center domain spins inside a stationary outer domain. Flow direction is along the x-axis. Blade2 is therefore traveling directly upstream at the particular moment in time shown.

(On a separate note, it looks like the ANSYS customer portal login page was hacked, also in the attached images)
Attached Images
 blade1ContourForce.jpg (45.2 KB, 32 views) blade1TableValues.jpg (52.3 KB, 24 views) blade1Symmetry.jpg (48.3 KB, 27 views) ansysCustomerPortalHacked.jpg (67.5 KB, 24 views)

 July 7, 2013, 18:23 #6 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,669 Rep Power: 84 The ANSYS Customer page appears to be back on line as normal. What is happening near the symmetry plane?

July 7, 2013, 20:08
#7
Member

Shawn
Join Date: Oct 2011
Posts: 56
Rep Power: 5
That's odd, the 'hacked' version still loads for me at https://www1.ansys.com/customer/default.asp and also on another computer at a separate location that I just logged into.

As for the symmetry plane, I was expecting there to be nearly zero-gradient in the forces perpendicular to the symmetry plane. The attached image shows Force Y plotted on the blade nearest the symmetry end of the blade. The blade is a 2D extruded mesh and the plot of Force Y on the surface looks good up to the nearest plane of nodes from the symmetry plane. On the layer closest to the symmetry plane the values of force appear significantly different from layers 2 and 3.

Pressure values have zero gradient perpendicular to the symmetry plane though. I wonder if the pressure and viscous forces have been separated.
Attached Images

 July 7, 2013, 20:35 #8 Senior Member   Join Date: Dec 2009 Posts: 129 Rep Power: 10 go directly to https://support.ansys.com But I am having trouble accessing the Service Request portion.

 July 8, 2013, 08:00 #9 Super Moderator   Glenn Horrocks Join Date: Mar 2009 Location: Sydney, Australia Posts: 10,669 Rep Power: 84 Assuming we are looking at the end of the blade with a symmetry plane then your images are strange, the normal gradient of all variables at asymmetry plane should be zero. Are you sure this is adequately converged? And the symmetry plane is perpendicular to the blades?

 July 8, 2013, 15:45 #10 Member   Shawn Join Date: Oct 2011 Posts: 56 Rep Power: 5 The solution is very well converged at this point and the symmetry plane is normal to the blade. I can't say that it's 100% converged, but the average torque over the whole turbine is changing less than 0.1% per revolution and this is after more than 15 revolutions. I plotted pressure on the blade surface and it appeared spot on, no normal gradient whatsoever.

 July 29, 2013, 19:44 #11 Member   Shawn Join Date: Oct 2011 Posts: 56 Rep Power: 5 I ended up talking with Ansys CFX support. The CFX solver code and Post have slightly different ways that values of Force and Torque are calculate. The monitor points and anything else accessible by the solver (for example surfaces that existing during the solution stage) are more accurate than surfaces created afterwards in Post. The differences are apparently mostly due to the wall shear calculation. So, in order to get torque strips on the blades, I have to separately integrate and sum the pressure and wall shear within Post. What would that CEL expression look like?

 July 30, 2013, 13:07 #12 Member   Shawn Join Date: Oct 2011 Posts: 56 Rep Power: 5 The bahaviour of Post regarding forces can be found here (http://www.sharcnet.ca/Software/Flue.../i1308522.html) and states that: CFD-Post calculates the approximate force as follows:If the locator is a wall boundary, the force is equal to the pressure force. For all other locators, the force is equal to the pressure force plus the mass flow force (due to the advection of momentum). In all cases, if wall shear data exists in the results file, the viscous force is added to the calculated force. So my forces/torques are missing the viscous forces because my blades are walls or because the wall shear data is not included in the results file, most likely the former because I've output all variables to the results file. To remedy this problem, the forces can be calculated by integrating the pressure and wall shear force components in the X and Y (or any arbitrary) directions: Fx = areaInt_x(Pressure)@locator + areaInt(Wall Shear X)@locator Fy = areaInt_y(Pressure)@locator + areaInt(Wall Shear Y)@locator and the torque can be calculated as: Tz due to Fx: areaInt_x(Pressure * Y)@locator + areaInt(Wall Shear X * Y)@locator Tz doe to Fy: areaInt_y(Pressure * X)@locator + areaInt(Wall Shear Y * X)@locator jthiakz likes this.

 Thread Tools Display Modes Linear Mode

 Posting Rules You may not post new threads You may not post replies You may not post attachments You may not edit your posts BB code is On Smilies are On [IMG] code is On HTML code is OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post saisanthoshm88 CFX 10 September 23, 2014 09:10 nore5 Main CFD Forum 0 May 10, 2013 12:45 nore5 OpenFOAM Running, Solving & CFD 0 May 10, 2013 12:43 ouafa Open Source Meshers: Gmsh, Netgen, CGNS, ... 7 May 21, 2010 12:43 snoopy CFX 10 December 28, 2009 03:58

All times are GMT -4. The time now is 23:08.