Hi Karamba forums, I have a problem where my results arent as close to FEM-design as I would have hoped for. I am working with a live link so the geometry should be the same, I have double checked the obvious reasions such as boundary, cross sections, materials, rigid element connections etc.

From FEM-design I get very slightly lower reaction forces, and if I lock the bridge in x direction in FEM design and Karamba, on both ends of the bridge. I get -75kN in Karamba and in FEM-design I get 18.6kN.

Furthermore the utilization differs always about 10% for different profiles (in the pictures 44% in FEM-design and 52% in Karamba), and the normal forces always differ, especially in tension 301kN vs 645kN. The maximum nodal displacement differs slightly aswell 34mm vs 39mm. I appreciate any help or input, thanks in advance

Edit: I would also like to know how Karamba calculates the utilization, thanks!

Dear @Rick8,
I do not have access to the ‘FEM-design’ program so it is hard for me to say what causes the difference of results.

Try a divide and conquer strategy: reduce the structure as much as possible (consider each load separately, remove support conditions, isolate one truss wall, reduce the truss to a beam,…) until the results coincide. Then focus on the point where the results start to differ.

The utilization which comes out of the BeamView-component is the ratio between stress and strength and does not include buckling. The utilization which comes out of the ‘Utilization’-component is calculated according to EC3, is based on the cross section as a whole and includes buckling via the beam buckling length.

Hi Clemens thanks for your advice, I have reduced the problem to being solely the shell bridge deck now, here is a new file, I would really appreciate if you could take a look at how the shells are modelled and if you think that the behaviour is correct? In FEM-design I get 693 mm deflection for dead load only, many thanks

Vertical reactions are always the same after I changed the gravity to -0.982, but the horizontal still differs, in this case 144 kN vs karambas 150kN.

Update: I remade the mesh for the bridge deck and made some important connections much finer, but now that I am getting the same results, its making me question why the deflection went from 23cm (in previous file) to 69.3 cm (the same as in FEM-design), when I made the mesh finer and imrpoved the connections, looking forward to any input, thanks.

I attached the file but it may take a minute to open as the mesh in now very fine for the longitudinal stiffeners. helpresults3.gh (138.6 KB)

Update again: the same results as the last file can be had in the second if I increase the the mesh refinement to 0.1 and also plug it into the longitudinal stiffeners (which I had forgot), and also clean it up slightly. So this makes me wonder why the displacement would increase so much with a finer mesh, I would appreciate if someone could just look at it and see if it is done correctly, and has a reasonable behaviour.

Without any deep dive into this particular issue, I suspect it is due to different shell elements and the meshing parameters.

Please see this blog post (it is a great blog altogether!) about triangular meshes and why they are “stiffer” than quads.

So if you narrow the problem down to just mesh differences and modify the meshes to be the same between two FEA software, the results should be the same too.

Hi again Clemens, I have finally managed to resolve all differences but there is one that remain and that is the utilization, is there anyway I can view the calculations of Karamba? From Karamba I am getting 53.3% vs 36.2% of Fem-design, with near identical moments, and normal forces. Here are the Fem-design calculations, would you say the process is the same?

Dear @Rick8,
thanks for the very detailed design calculation! I will go through it a.s.a.p.

Please find attached the source-code which is used in the current version of Karamba3D for calculating the utilization according to EC3: UtilChecker_EC3.zip (6.9 KB)
The archive contains the C++ code which consists mostly of formulas.

Did you check whether the beams you compare have the same buckling length?

With the “Utilization”-component (see here) and “Details?” set to “true” you can get out details from the Karamba3D calculation.

Hi Clemens I had the time now to read through your code, correct me if I am wrong but isnt this an error? I think that it should be (lam_z_bar)^2 instead of sqrt(lam_z_bar), here is a snippet of the Eurocode. This is what makes up the difference in utilization when i plug your phi into the FEM-design calculations, regards Rick.

Thank you for the clarification. I am again unsure where the difference lies in utilization now, because as I wrote earlier, I am getting near identical stresses, but utilization always varies 10-20%, I have checked the buckling lengths and they are always equal to the beam lengths in both softwares. I will try to look at the capacity of a corresponding truss and the stats from “details” Regards Rick.

If you have time to spare, I would appreciate if you could take a look at it aswell, here is the Karamba details and the respective members calculations from FEM-design (it is the top cord mid span, 180x6.3 SHS). As you can see capacity varies everywhere, and the interaction factors also differs alot (k11=kyy, k12=kyz, k21=kzy, k22=kzz). For this model the utilization is 86.6% in Karamba and 73% in FEM-design. Here are also some stress comparison, regards Rick.

I believe you have different methods for solving the interaction factors. Your screenshot shows that FEM-Design is using Method 1 (or Annex A) whereas Karamba3d uses Method 2 (or Annex B). I believe that has something to do with the difference.

Hi Clemens and Tuomas,I have checked the calculations again, and I believe that one of the differences is due to Karamba using 1.1 as gamma M1, also Karamba seem to round tensile strengths of material, for s355 the tensile strength is 360MPa or 36kN/cm^2. Now what remains are the interaction factors, which are derived from sectional constants, together with lambda which should be similiar as chi is 0.71 vs 0.72 (Difference here is probably due to 360 vs 355MPA) in Karamba and FEM-design respectively, does Karamba use method 2, and if so I still assume they shouldnt differ much at all?

I will take a look at that component I havent used it at all, thanks, regards Rick

Edit: I assume beam utilization component is the same? here it says that gamma M0 is 1 and M1 is 1.1, also Swayframe is True, with gamma M1 set to 1, capacity is basically the same, minor difference due to tensile strength (why is this rounded up?). So now only interaction factors remains

You can try and see if FEM-Design has an option to switch between the two methods to find interaction factors. In the Verification examples of FEM-Design, 9.6.3, both methods are considered. So it might be there is a setting that affects this, or then it runs with the chosen National Annex.

In Karamba3d manual it is stated that:
" The interaction values for the cross section forces…and so on get calculated according to EN 1993-1-1 appendix B"

Thank you, hopefully these are my last questions I have followed the Eurocode calculations to receive the Karamba results. FEM-design retrieves their interaction factors by method 1, class 1 & 2, while Karamba retrieves the interaction factors by method 2, class 3 & 4. The method do not differ much when I compare them with the same class, so the main difference is coming from the classifications.

I then tried the component Clemens suggested, so that I can change from elastic to plastic analysis, and hopefully this will result in class 1 & 2. I am not sure if this is the right implementation of it. Am I supposed to use it in place of the Analyze component? Which I had previously connected to the utilization of elements component, it also seem that I have to define Gamma for both of these components. Setup like this, I am getting quite different utilization 69% vs FEM-designs 73%, but the interaction factors remain as they where before. Thanks for your time, regards

Edit: I just noticed that the same settings are also in the utilization component, when changing here it influences the interaction factors closely to those from method 1 now, when elast is set to false, only 3% in difference now

Edit again: The last difference is coming from the slight difference in stresses + method 2 (I compared both, now same capacities with the two methods) as opposed to method 1, I am pretty satisfied at this point. I will try to research abit on the two different methods, thanks to you two
My final results are that Karambas method 2 is slightly more conservative (?) atleast in this case, I get 77% utilization vs 73 in FEM-design, with same capacities.