Hi Peter,
My doubt is about the results I found. My fin is very similar to a wing, where I have a flat surface on the botton and a curved surface on top. I would like to know the drag and the lift forces generated by the fin when subjected to a water flow (interely submerged in the fluid). The pressure profile over the fin seems consistent to me, but I not knowing how to see the vector forces (in newton) resulting from the pressure around the fin.
Hamed taught me a procedure (described bellow) that worked but I think the values are too high to be the forces exerted on a fin of 110 mm with speed of 1 m\s.
The procedure a used was:
Solver 2
Procedure = "SaveData" "SaveScalars"
Filename = dragforce.dat
Operator 1 = boundary sum
Variable 1 = Flow Solution Loads 1
Variable 2 = Flow Solution Loads 2
End
and the results I found was:
Variables in columns of matrix: dragforce.dat
1: boundary sum: flow solution loads 1 over bc 1
2: boundary sum: flow solution loads 1 over bc 2
3: boundary sum: flow solution loads 1 over bc 3
4: boundary sum: flow solution loads 1 over bc 4
.dat file
2.153568617542E+003 2.644249973207E+005 2.980330116155E+005 0.000000000000E+000
So I Thought that this results was the sum of the pressures boundary and not the forces.
Thank you,
Best regards,
Rodrigo
How to calculate the forces due the pressure in navierstoke

 Posts: 16
 Joined: 04 May 2010, 18:20

 Posts: 16
 Joined: 04 May 2010, 18:20
Re: How to calculate the forces due the pressure in navierstoke
Hi Hamed, Peter,
I was commiting a mistake. I was forgetting to put a command on the sif file. The two procedures described above are exatly what I was looking for.
Thank you very much.
Best regards,
Rodrigo
I was commiting a mistake. I was forgetting to put a command on the sif file. The two procedures described above are exatly what I was looking for.
Thank you very much.
Best regards,
Rodrigo
Re: How to calculate the forces due the pressure in navierstoke
Hello,
I was wondering how you managed to resolve this issue. I am trying to validate with a NACA 0012 airfoil. For a zero angle of attack, I get the following in my "dragforce.dat" file (see my attached .sif to see what this means)
5.029592858741E+000 5.218212250599E001 3.275385306949E009
This leads me to believe that the third parameter has something to do with the lift (which should be zero in theory). But, when I change the AoA to say 10 degrees, I get:
9.434822856886E+000 1.246319643055E+001 2.997330903905E009
This is what confuses me. What, exactly do the parameters mean? And is it possible to get the lift and drag coefficients without digging into the results file?
PS  I have one more question: when a boundary condition is not specified explicitly in the .sif file for NavierStokes flow, what becomes the default BC?
Best,
Dave
I was wondering how you managed to resolve this issue. I am trying to validate with a NACA 0012 airfoil. For a zero angle of attack, I get the following in my "dragforce.dat" file (see my attached .sif to see what this means)
5.029592858741E+000 5.218212250599E001 3.275385306949E009
This leads me to believe that the third parameter has something to do with the lift (which should be zero in theory). But, when I change the AoA to say 10 degrees, I get:
9.434822856886E+000 1.246319643055E+001 2.997330903905E009
This is what confuses me. What, exactly do the parameters mean? And is it possible to get the lift and drag coefficients without digging into the results file?
PS  I have one more question: when a boundary condition is not specified explicitly in the .sif file for NavierStokes flow, what becomes the default BC?
Best,
Dave
Code: Select all
Header
Mesh DB "airfoil"
End
Simulation
Coordinate System = Cartesian 2D
Simulation Type = Steady
Steady State Max Iterations = 20
Output Intervals = 1
Post File = "rigid.ep"
End
Body 1
Material = 1
Equation = 1
End
Material 1
Viscosity = 0.00002
Density = 1.2
End
Solver 1
Exec Solver = "Always"
Equation = "NavierStokes"
Variable = "Flow Solution"
Variable Dofs = 3
Linear System Solver = "Iterative"
Linear System Iterative Method = "TFQMR"
Linear System Max Iterations = 5000
Linear System Convergence Tolerance = 1.0e8
Linear System Abort Not Converged = True
Linear System Preconditioning = "ILU0"
Linear System Residual Output = 1
Steady State Convergence Tolerance = 1.0e02
Stabilize = True
Nonlinear System Convergence Tolerance = 1.0e05
Nonlinear System Max Iterations = 8
Nonlinear System Newton After Iterations = 3
Nonlinear System Newton After Tolerance = 1.0e02
Nonlinear System Relaxation Factor = 1
Linear System Precondition Recompute = 1
Calculate Loads = logical true
End
Solver 2
Procedure = "SaveData" "SaveScalars"
Filename = dragforce.dat
Operator 1 = boundary sum
Variable 1 = flow solution loads 1
operator 2 = boundary sum
variable 2 = flow solution loads 2
operator 3 = boundary sum
variable 3 = flow solution loads 3
End
Equation 1
Active Solvers(2) = 1 2
End
!inlet
Boundary Condition 1
Target Boundaries(1) = 2
Velocity 1 = 20.0000
Velocity 2 = 0.00000
End
!outlet
Boundary Condition 2
Target Boundaries(1) = 4
Velocity 2 = 0.00000
End
!airfoil
Boundary Condition 3
Target Boundaries(1) = 5
Velocity 1 = 0.00000
Velocity 2 = 0.00000
Save Scalars = Logical True
end

 Site Admin
 Posts: 3737
 Joined: 22 Aug 2009, 11:57
 Antispam: Yes
 Location: Espoo, Finland
 Contact:
Re: How to calculate the forces due the pressure in navierstoke
Hi
1) In 2D the third component (in 3D the 4th) of "Flow Solution Loads" is the residual coming from the continuity equation. So it does not have much relevance. The two first components are Fx and Fy.
2) Natural BC i.e. zero traction.
Peter
1) In 2D the third component (in 3D the 4th) of "Flow Solution Loads" is the residual coming from the continuity equation. So it does not have much relevance. The two first components are Fx and Fy.
2) Natural BC i.e. zero traction.
Peter

 Posts: 72
 Joined: 10 Nov 2009, 19:17
Re: How to calculate the forces due the pressure in navierstoke
May I resurrect this thread.... (it seemed more apt to add my query here rather than open a new topic)
I am using the fluidic force, with the boundary sum over surfaces. Now the output force is in x y and z directions, as opposed to normal (or parallel) to the surface (which is fine, one can calculate the normal).
My question now relates to the normal used by elmer in the calculation of the loads, that in equation 33.1 of the ElmerModelsManual. My results seem to indicate that this ''normal'' is not normal to the surface, rather it is a unit vector (or unit normal) along the axes. Is this the correct conclusion?
Thanks,
John
I am using the fluidic force, with the boundary sum over surfaces. Now the output force is in x y and z directions, as opposed to normal (or parallel) to the surface (which is fine, one can calculate the normal).
My question now relates to the normal used by elmer in the calculation of the loads, that in equation 33.1 of the ElmerModelsManual. My results seem to indicate that this ''normal'' is not normal to the surface, rather it is a unit vector (or unit normal) along the axes. Is this the correct conclusion?
Thanks,
John

 Site Admin
 Posts: 3737
 Joined: 22 Aug 2009, 11:57
 Antispam: Yes
 Location: Espoo, Finland
 Contact:
Re: How to calculate the forces due the pressure in navierstoke
Hi
If you're referring to the "calculate loads" method, there is no explicit forming of the normal vector. Rather what you get as the residual is known to correspond to the term \sigma \cdot \vec{n}. It's actually difficult to assign this force to different the boundary elements when computing the force in the corners. Maybe somebody with more insight in the FE method can comment how the normal that is only present implicitely in the weak form should optimally be computed?
In the fluidic force (currently 36.1.?) the normal is formed for each boundary element for which the integration is performed. The product within the integral is a tensor product so the outcome is still a vector with three components. Or perhaps I don't understand the question correctly...
Peter
If you're referring to the "calculate loads" method, there is no explicit forming of the normal vector. Rather what you get as the residual is known to correspond to the term \sigma \cdot \vec{n}. It's actually difficult to assign this force to different the boundary elements when computing the force in the corners. Maybe somebody with more insight in the FE method can comment how the normal that is only present implicitely in the weak form should optimally be computed?
In the fluidic force (currently 36.1.?) the normal is formed for each boundary element for which the integration is performed. The product within the integral is a tensor product so the outcome is still a vector with three components. Or perhaps I don't understand the question correctly...
Peter

 Posts: 72
 Joined: 10 Nov 2009, 19:17
Re: How to calculate the forces due the pressure in navierstoke
ApologiesI am using an old (about 1 year old) version of the models manualhence the 33.1 rather than 36.1 in the most recent version.
So, as I understand, the fluid force is computed normal to each boundary element, then when it is displayed in the user specified output file for the boundary sum one can get 3 components. It is my understanding that the components were the fluid force in the x, y, and z directions (IE not normal to the surface).
Maybe my question is best served by an example. Below is a screengrab from elmer, the compass shows the direction of the axes (red cone is x, green y) I have a flow of fluid coming from the boundary to the rightmost of the screen (therefore flow along negative x).
I wish to calculate the fluid force on the cantilever beam. One part of the cantilever is selected. I take into account the top, bottom, and edges of the beam and use the boundary sum of the fluid force for the total fluid force on each area. Attached is the output file using the fluid force/boundary sum method for the ''flow solution loads 1'' 2 and 3 using the following code in the sif file:
Now, if in the output file we take the second line corresponding to ''flow solution loads 2'', which I believe to be that along the y axis, and we wish tocalculate the total fluidic force in that direction. If the results displayed are along the y axis the we must add all the values (IE side1+side2+bottom+top= 2.231074766653E008 + (2.336941529793E008) + (2.397792564864E008) + (9.446020778595E010) = 7.06E08). But, If the output is somehow normal to the surface one has to take account of this, then one presumably has to do total=side1+side2+bottomtop= 6.87E08. If this latter is the case then I would have expected that side1 and 2 would have the same magnitude but different signstheir values should be the same as the setup is symmetrical with fluid flowing along x.
I hope I have managed to explain this, though I suspect not in the clearest manner. The nub of the matter is how to treat those 4 numbers in the output file.
Thankyou, John
So, as I understand, the fluid force is computed normal to each boundary element, then when it is displayed in the user specified output file for the boundary sum one can get 3 components. It is my understanding that the components were the fluid force in the x, y, and z directions (IE not normal to the surface).
Maybe my question is best served by an example. Below is a screengrab from elmer, the compass shows the direction of the axes (red cone is x, green y) I have a flow of fluid coming from the boundary to the rightmost of the screen (therefore flow along negative x).
I wish to calculate the fluid force on the cantilever beam. One part of the cantilever is selected. I take into account the top, bottom, and edges of the beam and use the boundary sum of the fluid force for the total fluid force on each area. Attached is the output file using the fluid force/boundary sum method for the ''flow solution loads 1'' 2 and 3 using the following code in the sif file:
Code: Select all
Solver 2
Procedure = "SaveData" "SaveScalars"
Filename = fluidforceh100.dat
Operator 1 = boundary sum
Variable 1 = Flow Solution Loads 1
End
I hope I have managed to explain this, though I suspect not in the clearest manner. The nub of the matter is how to treat those 4 numbers in the output file.
Thankyou, John