Problem obtaining normal vectors on blade loading line
 

Dear all

I am currently investigating the flow field in an axial flow fan using Ansys software. The solving is done in Fluent and I am currently conducting some post processing in CFD-Post. My problem involves obtaining the face normal vectors on the "blade loading" line (a line along the blade surface at a specified radius as shown in the picture). For some reason I am able to obtain information such as the shear stress, static pressure etc., but when I try to graph and export the normal vector components (Normal X, Normal Y, Normal Z) as CSV files, it just gives an answer of 0 all along the blade surface for each of the components.

It seems that obtaining the normal vectors should be a straightforward task, yet I am struggling. I've tried searching the user manual and some of the other threads, but cannot find a solution to the problem. Is it due to the fact that turbomode is used? Or maybe that some of the mesh information is not passed on from Fluent?

Help would be a appreciated.

Kind regards
Francois Louw

No, I suspect the problem is that you are exporting parameters along a line and the normal vector along a line is not defined. Surface normal is defined for a surface, so you will have to use a surface object to get the surface normals.

One idea to try would be to export the line feature you have created, then export the surface normals of the blade surface. Then using a matlab/python/fortran/whatever program match each point on the line with its nearest surface point and get the surface normal. A little ugly but should be do-able.

Hi Glenn

Ah! Thank you very much. I suspect you are right and think what you have suggested is most probably the best way of finding the face normals. It would have been neat if CFX was able to do this (linking the line nodes to the nearest face nodes) since it gives you the option to export a normal on the line, only with no result.

I do some postprocessing of results in Python and will try to give it a shot using it. I'll maybe post something again to say whether it worked or not. I suppose it will take some time.

Lastly, thank you for your reply and all your other posts as well. It really is helpful.

Kind regards
Francois Louw

Found some from of solution
 

I said I would reply if I found some solution for the problem I posted in the previous posts... Sorry for the delay.

I was after the normal forces and vectors at a certain span location on the fan blade I was modelling. After some playing around and help from Glenn, I was able to obtain the 'Normalized force components' at a certain specified location (in my case a 'turbo line' at a certain radius along the blade profile), which is a force value given in N per m length. I was able to obtain this by first setting up a 'balde loading' plot in the 'turbo' tab of CFD-post and plotting any random values ('Normalized force' values cannot be selected in turbo mode for some reason). Thereafter I went back to the 'outline' tab where the 'blade loading chart' appears in the tree. By editing this chart one can edit the plotting variables. Only in the 'outline' tab can one select the 'Normalized force on blade loading line' and all of its components, as well as the boundary face normals.

I don't know whether this is trivial, but hope the post helps anyone in the future.

Regards
Francois

Thank you for posting this workaround. The options in the 'turbo' mode are so limited, which is driving me nuts. Why wouldn't they just give us the same options as in the 'Outline' tab?! I'm on version 17 by the way.
I am currently still struggling to get a blade loading chart from only ONE blade and not all 4 in one chart. I modeled/meshed one blade and did a turbo rotation in Pre and now I am stuck with all 4 blades at once anywhere in Post :mad:

Hi, my friend. Did you solve your problem? I hope you did. I have similar trouble with CFD-Post, I have a full geometry of a pump and I even can not get a blade loading chart of any blade. we can only use TURBO TAB with periodic geometries in order to get turbo charts, can not we? If so, how can I get turbo chart and report with a simulation of a full pump geometry? Thank you in advance.

I haven't found a solution yet.

However, I have found a way how to evaluate pressure, forces, etc. via expressions for each blade: In the Outline tab there is one drop down menu called 'Mesh Regions'. There I find items such as 'BLADE', 'BLADE 2', etc. That means I can write expressions such as
force_z()@BLADE 2

Maybe we can manually create a blade loading chart with that workaround?

Thank you for your reply, expression is a good tool for us to calculate. However, in my opinion, expression only gives us 1 average value of pressure or force for 1 blade. Meanwhile, in order to get a chart, we need a set of pressure or force values on 1 blade. So, it can not solve our problem thoroughly.:D:D:D

yes, I agree. It also annoys me that I cannot evaluate the suction side and pressure side separately. I can only get force, pressure etc on a COMPLETE blade.
One thought about a 'manual' blade loading chart: maybe we can create some kind of poly line at a certain radius of the blade. A line made with several points along the surface of the blade and evaluate the values at each point. But I haven't tried that yet.
I'm afraid that this would be a tedious work - and also that we would have to create such a poly line for each degree of rotation :(

Right, my friend. If there is no way else, we have to try your method despite it's time-consuming. By the way,do you have any idea about the problem I post in this topic. I even can not initialize my model.
http://www.cfd-online.com/Forums/cfx...tml#post596711

okay... I found a workaround I think. Still need to refine it and double check but I think I'm on the right track here:

1. create a "Turbo Surface" at a constant span like 0.7
2. create a "Polyline" and select as method "Boundary Intersection". Use "BLADE" (or BLADE 2, BLADE 3, etc from the [...] menu and "Mesh Regions") as 'Boundary List' and 'Intersect With' "Turbo Surface 1".
3. create a chart with type "xy" and use Polyline 1 on the x-axis and pressure etc on the y-axis.

Comments are welcome