Good day to you Sir @FEAnalyst,
Regarding Tutorial 30 Shell buckling, I just downloaded the model link from youtube, then all the Buckling step set up just the same with you. However the results of buckling factor is different. I would like to confirm the following:
Buckling Factor that I got, see below snap shot: BF 852625, DISP ALL +0.01457mm, Deformed shape is different.
My global coordinates direction is Y-vertical
While in you tube Z-Vertical
Appreciate sir if you could advise me how to change global coordinates into Z-Vertical.
Thank you sir and appreciate for your helpful inputs.
Is it the same mode shape ? Linear buckling results in CalculiX can be highly mesh sensitive, make sure that you use the same meshing settings. Also, check all the other settings, especially boundary conditions and load.
The model is oriented in the same way in both cases. You just have to rotate the view using the middle mouse button or keyboard arrows.
P.S. It’s not a tip for users but a question so it should belong to the general (blue category).
Dear Sir, I apologized, I will be very careful next time and will try to use the appropriate topic category. I’m sorry about that .
Also After checking and comparing the model, all setting are the same with you. Except that due to many trial I did not notice that the model I am using is already imported the Imperfection.inp. That is the reason why the buckling I got is smaller than the original model.
After that I notice that I need to take a rest due to 15days consecutive of studying.
Thank you and always appreciate your great kindness for sharing your wonderful talent.
No problem at all, I can correct the category if needed, just wanted to let you know how it works here.
I’m glad that you solved the problem. It’s good to have a reference so that you know when some mistakes were made. That’s also why I always include analytical solutions in my tutorials.
Yes Sir @FEAnalyst I was so glad when I got that. I was so relieved and really happy about the results. Although my PC just reach 51modes, but the capacity I got is same with you, then after that the capacity curve drop down.
Sir in that case is it normal that modes will not be completely the same even though my model and setting are 100% equal from your settings. Because in your case upto 58modes and your Von mises stress is 485.3MPa
differ from what I got 516.6MPa. But I’m not worried about that since I am interested on the Peak capacity only.
Also can I still apply the method of applying material imperfection (same method of Tut 30) for the case of Tensile force? Just concern Sir, that if I apply the imperfection for the Tensile, the imperfection may acting as the stiffener and when apply the Tension, that imperfection may straightened then the solver will stop in the iteration and convergence? Appreciate Sir from your inputs and advice.
Thank you…
There can be some small differences. The mesh is not exactly the same (those simulations are really mesh sensitive) and each run introduces some round-off errors.
Give it a try. But then it won’t be a buckling case as that happens under compression.
Dear Sir @FEAnalyst,
Sir Jakub, I hope this message finds you well. Regarding my attempt to check the results for Equilibrium path aiming to replicate for the case of member purely tension load and checking what will be the results.
I carefully followed the steps outlined in the tutorial 30, but I’m encountering a difference in the resulting equilibrium path. While the tutorial shows the capacity chart dropping down after reaching a peak, mine continues to climb upwards as the load increases.
I’ve attached a screenshot of my results for your reference.
I would be very grateful for any advice you could give on how to achieve the expected descending equilibrium path. I’ve already tried increasing the load to 8MN, hoping it would trigger the downward trend, but it hasn’t been successful.
Could there be any other factors I haven’t considered that might be causing this discrepancy? Any insights or suggestions you could share would be immensely valuable to me.
How to meet the descending equilibrium path or at least stabilized the Equilibrium path such as shown below snap shot:
Thank you for your time and support.
Best Regards,
jess
It’s a completely different model - lug subjected to tension (applied in what way?) so the equilibrium path will be different. Mine drops down because the structure buckles and loses capacity. Your structure doesn’t buckle and keeps its capacity. So I think that you shouldn’t try to achieve similar results as in the tutorial but rather carry out a different nonlinear analysis (geometric nonlinearity is important so make sure that Nlgeom is on), only following the tips like how to plot displacement vs force. Most likely, you won’t need the geometric imperfections either. Unless you force this structure to buckle due to compression somehow. From what I know, ASME includes out-of-plane buckling (called dishing) as one of the failure modes of lifting lugs but you would have to check what boundary conditions and loads are needed to account for that.
Dear Sir understood and well noted.
In regards to how I applied the load I model the actual pin with contact and also try to use direct load using surface traction, both are completely the same output results. The only difference modeling actual Pin with implementation of contact requires much time to complete the analysis.
For your additional information Sir, actually the results of the Prepomax is really good and wonderful as it same results with the analytical solution. Especially at the point where the equilibrium path is at the transition of Elasto-Plastic, it was so great at Step, Increment 1,14 deformation is in nice and realistic shape.
Then at the point of plastic strain range, Step Increment 1,15 deformation shape starts to go sideward instead of going upward direction. As shown on below sample for illustration only.
I humbly suggest Sir Jakub if we can possibly incorporate this in the Prepomax, will be a much more powerful and much appealing to all over the world in the FEA user community. Or maybe already in the PrePomax Calculix, I just didnt know yet how to deal with this problem properly. Any inputs Sir will be highly valuable.
Can you share a picture of your analytical calculations ? Maybe also the model (.pmx file) if you can and if you want me to take a look to see if everything is all right.
I assume that you are showing highly scaled deformation. Look at true scale shape or use lower scale factor. Then such discrepancies may become very small or even disappear at all.
Also, make sure that Nlgeom is on. If you are modeling the pin as a surface then you should make it rigid. But if it converges well and gives the same results as directly prescribed loading then the latter approach might be better.
Dear Sir Jakub, good day you. Thank you very much for your great advise. Yes Sir, I turn on the NLgeom.
Sir Jakub you said “If you are modeling the pin as a surface then you should make it rigid”.
I would like to confirm if my understanding is correct. Is this means that I have to apply constraint, rigid body, to the surface, then to be able to do this, I have to assign reference point then rigid body as shown below?
Please note that, to be able to make the .pmx file lower, I created another file completely the same of my model including all the parameter. The only difference is the mesh parameter setting; I make it 60mm to reduce the files.
Below is the mesh parameter I use in my analysis. Sir Jakub please kindly do the remeshing similar to mine (below) so that we can compare apple to apple.
Thank you Sir Jakub, and really appreciate this so many time already I ask to you. Thank you, many time.
Best Regards,
jess
Yes, but only if you were modeling the pin as a separate surface (shell) part. Here you are applying the load directly to the lug so it’s irrelevant.
Which standard are you using for those calculations ?
The results look good and symmetric with true scale deformation. You could just consider more realistic load application and that is contact with a rigid pin, as described above.
Dear Sir Jakub, thank you very much for your time for your checking and your great advice is well noted. I will try to model the pin as a separate surface (shell).
Regarding the Standard, I use AISC Code Pin Connection type such as:
For Tensile Stress: 0.60Fy and for In Plane Bending and Out of Plane Bending: 0.66Fy, Shear 0.40Fy, 0.90Fy for Bearing stress. Area consider are the net/critical area which is at pin hole region.
I also use ASME-BTH-2011 for comparison only due to basis of the requirement is AISC Code. All are align with the results, Prepomax, AISC Code, ASME-BTH-2011, ASME B30.30 and DNV. That Lug is failed for 465Tons and can only sustain the load upto 295Tons or less than 3MN.
“The results look good and symmetric with true scale deformation. You could just consider more realistic load application and that is contact with a rigid pin, as described above.” Noted Sir, thank you so much for your time and your helpful advice."
Dear Sir Jakub, good day to you. I try to model the pin with using rigid body, and I found out that there is some difficulty using rigid body if they are shared with common element. Also it does not converge and complete the analysis, with Failed Results!
By trying to make a rigid body constraints representing the pin as load distributor then simulation failed.
Even for Solid element to represent the pin using Rigid body and if they shared together in the same element and common point, simulation failed results.
I just observed that the perfect and very smooth results and simulation is modeled it by Contact. The only drawback of this is to wait the results about 6hours approx depends on nos. of element.
And another which is output is same with the contact is to apply the load directly to the surface of the pinhole. Which is more faster to converge about 1.5 hour only you can get the nice results.
This approach should be optimal but contact may introduce convergence issues. You can share the .pmx file if you want to get it fixed. But if the results of the simulation with load applied directly to the lug are sufficiently accurate (compared with the simulation where the whole pin is modeled as a deformable body) then it might be best to stay with this approach. Especially if standards allow it.
.
