1
1- I guess values on diagram are given the same way as on a panel cut or reduced results. Probably they choose the center of the last row (up and below) of FE to avoid conflict regions that always appears near de edges of each story where the incoming slabs get their support.
Setting panel cuts on 0.5m and 7.5m height , will give the same values found on core wall diagram
FE method will never give you a 100% correct result. But of course if you refine the mesh, results will get a LOT better. For a 5cm mesh size both models give an almost perfect moment at the bottom.
And if you assign the horizontal loads on the middle of the wall instead of the corners , results will be a lot better also on the upper side of the wall
Of course a 5cm mesh on a 8mx5m wall is not practical unless you are working on a NASA supercomputer 
. So in these particular cases you have to balance your mesh density in a way that you get reasonably fast and aproximately accurate results.
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Rafael is 100% right. Initially (in older versions of RSA) the cut to obtain values for the core wall diagram wad made very close to the panel edge (you can find some complains about this fact on this forum 
) but the results obtained in this way were by far less accurate comparing to these done at the centers of the first row of surface elements so the corresponding change was made.
If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.
Artur Kosakowski
Hi @Artur.Kosakowski @Rafacascudo
Rafael is 100% right. Initially (in older versions of RSA) the cut to obtain values for the core wall diagram wad made very close to the panel edge (you can find some complains about this fact on this forum 
) but the results obtained in this way were by far less accurate comparing to these done at the centers of the first row of surface elements so the corresponding change was made.
I know That the reduced cut forces will have big variation base on mesh size and shape.of the mesh .But If you tried to consider square mesh You will obtain good result with good accuracy For the panel Cut result At Any place You make Cut and this will make this issue more practical.
But By Having the result from Core wall on center of mesh up and down this mean that this core wall result is useless because you cant obtain the bottom moment of each level and the result will be more far from the actual and this will be un trusted and not safe to design the core wall base on the core wall result diagram .There fore we really need to understand why cant the core wall results cant be obtained at top and bottom level though we know that its easy to have cut for the core wall on the top and bottom by panel cut and get the accurate result.
Just to let every body understand my point I will give example:
If Have tower with core wall and with 4m story height for functionality and practicality reason we use mesh with as 1 m Square type means that the result of the core wall will be given on the base at 0.5 m height from the base level and this will be not correct at all and suitable to design the core wall.
I know That the reduced cut forces will have big variation base on mesh size and shape.of the mesh .But If you tried to consider square mesh You will obtain good result with good accuracy For the panel Cut result At Any place You make Cut and this will make this issue more practical.
I wish that was true
Please check: https://forums.autodesk.com/t5/robot-structural-analysis-forum/core-non-consistent-results/m-p/45281...
But By Having the result from Core wall on center of mesh up and down this mean that this core wall result is useless because you cant obtain the bottom moment of each level and the result will be more far from the actual and this will be un trusted and not safe to design the core wall base on the core wall result diagram .There fore we really need to understand why cant the core wall results cant be obtained at top and bottom level though we know that its easy to have cut for the core wall on the top and bottom by panel cut and get the accurate result.
Just to let every body understand my point I will give example:
If Have tower with core wall and with 4m story height for functionality and practicality reason we use mesh with as 1 m Square type means that the result of the core wall will be given on the base at 0.5 m height from the base level and this will be not correct at all and suitable to design the core wall.
This is indeed a valid point so you may consider the following options:
1. Freeze the mesh and moving most top and bottom nodes of the 2nd row of surface elements surface elements closer to the panel/wall top and bottom edge
2. Select the outermost rows of surface elements of core walls and use mesh refinement option
I hope you find them helpful.
If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.
Artur Kosakowski
Just want to know what is the difficulty by having them on the top and bottom edge since it can be done ?
Hi Mustafa,
It can be done but for the multistory building with the shape function that defines surface elements as implemented in Robot the results may be like this (edges vs. centers of elements):
Considering all pros and cons the decision was to change the position of the cut from the edges to the centers of the elements.
If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.
Artur Kosakowski
This my first time seeing the results of the core walls is bigger than the reactions any way and for me and for safety reasons its much more better to have it the result at the edge not in first finite element center . To design the core for bigger results better than design it for smaller results.
And If you notice that changing of this core wall result presentation since 2014 to be on center of finite element didn't fix anything
though its become worth.
As a designer I strongly recommend to return it back as what is was before or to add this issue as option.
According to my knowledge the change was intended to deal with this sort of situation:
but as always I have forwarded your suggestion/request to the development team.
If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.
Artur Kosakowski
I did Research about this issue and I found that there is mistake When RSA calculating The reduced result of panel cut
For the same example of the core wall the one you where showing me The Rsult which is related to link
I took the lower core have walls no 1 2 3 4 then I made section which exactly at finite element center z level 0.375m as shown in the picture :
I study this section in order to know what is happening because I am really not believing that this error will be encountered in finite element method
(Result bigger than Actual)
The study is came first by studying the way RSA Calculating the Reduced result attached in this link
http://help.autodesk.com/view/RSAPRO/2018/ENU/?guid=GUID-2C7F8C26-C452-46A3-9A0D-07C9B278233A
Then I did this steps in order to understand :
I changed the X local for the walls to be according Z global axis then I make model calculation I study case no 1 Which the reduced result of Fy is 1300.63 Kn which bigger than the force 1200 kn .
Because this core is symmetric so I took each two paralleled walls individual Then I compared it with the whole.
I took the 2 walls no 2 and (this 2 walls are parallel to Y ) in a window then I view the section Nxy :
Because that this 2 walls are parallel to y So :
Reduced Fy = integral value of Nxy of the map cut But RSA doesn't calculate it correctly see the picture :
So Fy=1111.51 KN Not 1270.60 KN.
I took the other 2 wall no 1 and 3 then The two walls are perpendicular on the y direction So
The Reduced Fy force = integral Value of Qz (shear force not membrane)
So Reduced Fy = 8.79 KN Not -30.03 KN
There Fore The Total Core Wall Reduced Fy Force
Fy = -1111.51+8.79 =-1102.72 KN
Not 1270.60+30.03 =1300.63 which same core wall result.
There Fore I think Everybody know why this Error encountered .
@Artur.Kosakowski awaiting for your feed back.
Hi Mustafa,
IMHO you need to consider the direction of shear in (perpendicular) walls and mind the averaging settings.
If you find your post answered press the Accept as Solution button please. This will help other users to find solutions much faster. Thank you.
Artur Kosakowski
Hi Mustafahesenow ,
The difference is that you are getting results using "global smothing". If you choose "smoothing within a panel" instead , results will agree with those found on "diagrams for core walls".
So probably , "diagrams for core walls" is using that setting ( smoothing within a panel") to achieve its results. Maybe it would be a good idea to bring this choice of settings (no smothing , global smoothing, etc) also to "diagrams for core walls" dialog window.
Rafael Medeiros
Did you find this post helpful? Feel free to Like this post.
Did your question get successfully answered? Then click on the ACCEPT SOLUTION button.
Hi @Rafacascudo @Artur.Kosakowski
1-With considering No smoothing we will get Accurate results
2- With Considering Global Smoothing
2- With Considering Smoothing within the panel
There Fore The Best option to calculate the reduced Forces and moment for panel Cut and need to be implemented on core wall result from
top edge and bottom bottom edge is Calculation this Values base in Global smoothing cut option .
Because If we make cut on the base of the core wall we will get this result :
Please @Artur.Kosakowski confirm it and Let it be modified.
Hi Mustafa,
This needs some more tests but definitely at the element centers rather than at the edges.
Artur Kosakowski
After All of this discussion I really want to know what the point if have it in the center of finite element not in the edge .
Its useless if at center of finite elements .
Hi Mustafa,
The only reason is that despite they are not at the edge they are more accurate. If you look at the picture I attached to my previous post you will see that the results defined at the centers give approx. 1200 kN (green frames) which correspond to the total value of loads whereas the ones 1 cm above the supports more than that (yellow frames). Mind that the results in the surface elements are not calculated in nodes but in the Gauss points instead and then extrapolated to nodes which is less accurate at the locations of boundary conditions.
In other words IMHO what apparently seems illogical may actually be sensible
Artur Kosakowski
I Had attached this picture showing that with global smoothing the result with global smoothing will be more accurate than the others.
Please let me draw your attention that The result of the core walls if it keeped like that It will be relate and depended with the mesh size
and this very critical mistake especially when you have towers and high rise building (you cant increase the mesh division to consider this only for core wall results)
For me as a designer it will be very nice to calculate it above and under wedge with 1cm only with global smoothing or no smoothing (not related to mesh size cos this will be un controllable)
I would really love also to make the normalize option embedded in the viewing the core wall result diagram and and reduced forces in panel cut So the result will be updated and changed due the choose of type of smoothing above or under 1cm from the edge.
