Section fiber stress results visualization
Section fiber stress results visualization
Hello STKO Team,
I am trying to model a piping system and trying to visualize the portions of the pipe which would fail first or lets say the potions with the most stress. The stresses are as a result of Gravity Analysis and Time History Analysis.
For the Gravity Analysis, i have input the masses as node forces(Since i cannot run gravity analysis with giving masses as node forces) and for the time history analysis i have input the masses as line masses.
I have also length interactions, Zero length elements for modelling the spring under the supports. The spring behavior is expected in only lets say global z direction and for the other two, i used equal dof condition.
I have the following questions.
> Is it ok to specify masses via both node forces and line masses. I assumed that the gravity analysis will only take the masses( specified as node forces) and TH Analysis will only take the line masses automatically. Am i correct for this assumption?
> While defining the ZL Physical property we have to select among dirn 1, 2 and 3(3d, only displacement), whereas for the definition of equal dofs we see ux, uy and uz. My question is are these are local axes or global axes? I remember vaguely seeing it in one of your webinars but i cannot find it again. > The stresses values are not in line with the expected values. Could you possibly please check the model? I do not know what i am doing wrong.
> for checking the section forces like N, My, Mz and T, i can see it via the surface color map plot as well as the gauss point plot. Are they both the same ?
> Is it possible to view the max stress, max reaction forces etc. for a Time History analysis without having to see time steps one by one? Yes it should be point of max acceleration but still i am curious if we can just find the max.
> I used the following analysis steps. Gravity analysis followed by TH analysis. My question is should i be using wipe analysis option after the Gravity analysis or not, i want to see the cumulative effect of both of them? I compared the displacements and reaction forces in all 3 directions, with and without the wipe analysis option being selected, but the results were same. It should not be this, right?
I tried clearing the doubts via your videos or online help, but i was not able to find these fine points. It would be really helpful if you could help me on this. I am attaching the scd file as well in zip.
I am trying to model a piping system and trying to visualize the portions of the pipe which would fail first or lets say the potions with the most stress. The stresses are as a result of Gravity Analysis and Time History Analysis.
For the Gravity Analysis, i have input the masses as node forces(Since i cannot run gravity analysis with giving masses as node forces) and for the time history analysis i have input the masses as line masses.
I have also length interactions, Zero length elements for modelling the spring under the supports. The spring behavior is expected in only lets say global z direction and for the other two, i used equal dof condition.
I have the following questions.
> Is it ok to specify masses via both node forces and line masses. I assumed that the gravity analysis will only take the masses( specified as node forces) and TH Analysis will only take the line masses automatically. Am i correct for this assumption?
> While defining the ZL Physical property we have to select among dirn 1, 2 and 3(3d, only displacement), whereas for the definition of equal dofs we see ux, uy and uz. My question is are these are local axes or global axes? I remember vaguely seeing it in one of your webinars but i cannot find it again. > The stresses values are not in line with the expected values. Could you possibly please check the model? I do not know what i am doing wrong.
> for checking the section forces like N, My, Mz and T, i can see it via the surface color map plot as well as the gauss point plot. Are they both the same ?
> Is it possible to view the max stress, max reaction forces etc. for a Time History analysis without having to see time steps one by one? Yes it should be point of max acceleration but still i am curious if we can just find the max.
> I used the following analysis steps. Gravity analysis followed by TH analysis. My question is should i be using wipe analysis option after the Gravity analysis or not, i want to see the cumulative effect of both of them? I compared the displacements and reaction forces in all 3 directions, with and without the wipe analysis option being selected, but the results were same. It should not be this, right?
I tried clearing the doubts via your videos or online help, but i was not able to find these fine points. It would be really helpful if you could help me on this. I am attaching the scd file as well in zip.
 Attachments

 for forum.zip
 (232.47 KiB) Downloaded 103 times

 sectiion fiber stress.JPG (129.73 KiB) Viewed 5045 times
Re: Section fiber stress results visualization
The "weight" must be modelled as a force (otherwise you would need to do the gravity analysis as a dynamic analysis with the gravity acceleration... instead we typically do it as a static analysis, therfore you need a load).> Is it ok to specify masses via both node forces and line masses. I assumed that the gravity analysis will only take the masses( specified as node forces) and TH Analysis will only take the line masses automatically. Am i correct for this assumption?
Then, the masses that you assign will generate inertia forces during dynamic excitation
By default, they use the global axes. Unless you assign a custom Local Axes to the interaction> While defining the ZL Physical property we have to select among dirn 1, 2 and 3(3d, only displacement), whereas for the definition of equal dofs we see ux, uy and uz. My question is are these are local axes or global axes? I remember vaguely seeing it in one of your webinars but i cannot find it again.
The model seems correct from a modeling point of view. Now it's up to you to understand if your loads/BC/units are all consistent with the example you are trying to simulate> The stresses values are not in line with the expected values. Could you possibly please check the model? I do not know what i am doing wrong.
Yes, but in general the results on gauss points viewed in surface color maps are extrapolated to the nodes. So if you use an integration scheme with gauss points that do not coincide with the element nodes, they could be slightly differet. This should not be an issue with beams, because you typically use Lobatto Integration.> for checking the section forces like N, My, Mz and T, i can see it via the surface color map plot as well as the gauss point plot. Are they both the same ?
The easiest way is to select all the points of interest, extract the results to obtain a chart and identify what's the max/min etc..> Is it possible to view the max stress, max reaction forces etc. for a Time History analysis without having to see time steps one by one? Yes it should be point of max acceleration but still i am curious if we can just find the max.
Re: Section fiber stress results visualization
Thank you for the response. It cleared most of my doubts. However i still have two more questions and would appreciate your responses on this.
> Can you please answer this question, which i previously asked.
'' Gravity analysis followed by TH analysis. My question is should i be using wipe analysis option after the Gravity analysis or not, i want to see the cumulative effect of both of them? I compared the displacements and reaction forces in all 3 directions, with and without the wipe analysis option being selected, but the results were same. It should not be this, right? ''
> For this model if i apply the Ground Motion in x to the original supports and few more supports , during the analysis steps, the following error is showing up. As i understand it, it is because of the Toi value set in Norm displacement increment test. However the algorithm, i guess tries to reduce the increment factor, in order to fulfill the condition. But the analysis keeps going on and completes.
Does this mean that my model results are correct or wrong because of failure at this time step, beacuse i can see an error flag is also being generated? I am attaching the updated model with GM in x dirn.
Thanks and regards
> Can you please answer this question, which i previously asked.
'' Gravity analysis followed by TH analysis. My question is should i be using wipe analysis option after the Gravity analysis or not, i want to see the cumulative effect of both of them? I compared the displacements and reaction forces in all 3 directions, with and without the wipe analysis option being selected, but the results were same. It should not be this, right? ''
> For this model if i apply the Ground Motion in x to the original supports and few more supports , during the analysis steps, the following error is showing up. As i understand it, it is because of the Toi value set in Norm displacement increment test. However the algorithm, i guess tries to reduce the increment factor, in order to fulfill the condition. But the analysis keeps going on and completes.
Does this mean that my model results are correct or wrong because of failure at this time step, beacuse i can see an error flag is also being generated? I am attaching the updated model with GM in x dirn.
Thanks and regards
 Attachments

 GM in x.zip
 (250.5 KiB) Downloaded 113 times

 Posts: 61
 Joined: Thu Dec 09, 2021 10:53 am
Re: Section fiber stress results visualization
Hi 2006garg,
You are probably confusing "wipeAnalysis" with the "loadConstant". To keep loads from gravity analysis you selected "loadConstant" in the first analysis and you reset pseudotime to 0. Try to remove this and you will see the difference. Anyway now it is set up as you want.
You are using adaptive time step so when it is difficult to converge it is reducing the increment. It doesn't mean that your results are wrong.
Please let us know if you still have doubts
Best, Valentina
You are probably confusing "wipeAnalysis" with the "loadConstant". To keep loads from gravity analysis you selected "loadConstant" in the first analysis and you reset pseudotime to 0. Try to remove this and you will see the difference. Anyway now it is set up as you want.
You are using adaptive time step so when it is difficult to converge it is reducing the increment. It doesn't mean that your results are wrong.
Please let us know if you still have doubts
Best, Valentina
Re: Section fiber stress results visualization
Hello Valentina,
thanks once again for your reply. Your team's feedback has helped me to get the model better and better. However i have few more questions.
We are running the same analysis as given above (gravity analysis followed by Time History Analysis) for a different but similar model. As material we are Steel 02 and defined the properties as below. In this we can see that the material behaves linearly in the (2e8 and 0.001 strain) range and thereafter goes in the non linear stage. However some elements of our model were going into the non linear stage very early and not behaving like the material should behave. I checked the material assignments and all seems to be fine there. I checked this element because when trying to see the max strain in the over the time history(our goal is finding which elements fail first or are prone to failure) i saw some irregular peaks. On checking where those peaks were occurring, i came to this element and saw its stress strain curve.
This shows that it is going into non linear stage i.e. after the proportionately limit much earlier than what is specified for the material. I have no clue why this is happening. Do you have any ideas as to why this could be happening?
Thanks in advance
Regards,
Gaurav
thanks once again for your reply. Your team's feedback has helped me to get the model better and better. However i have few more questions.
We are running the same analysis as given above (gravity analysis followed by Time History Analysis) for a different but similar model. As material we are Steel 02 and defined the properties as below. In this we can see that the material behaves linearly in the (2e8 and 0.001 strain) range and thereafter goes in the non linear stage. However some elements of our model were going into the non linear stage very early and not behaving like the material should behave. I checked the material assignments and all seems to be fine there. I checked this element because when trying to see the max strain in the over the time history(our goal is finding which elements fail first or are prone to failure) i saw some irregular peaks. On checking where those peaks were occurring, i came to this element and saw its stress strain curve.
This shows that it is going into non linear stage i.e. after the proportionately limit much earlier than what is specified for the material. I have no clue why this is happening. Do you have any ideas as to why this could be happening?
Thanks in advance
Regards,
Gaurav
Re: Section fiber stress results visualization
Can you share your model to have a look?
Re: Section fiber stress results visualization
Hello, I have attached the model and also the location of the element exhibiting this behavior.
I have also attached the Max strain curve which which i found the time where it was showing peaks (first peak=1.78s). I then searched the element having this behavior at 1.78 sec and proceeded to see its max stress strain curve which is also attached.
I have one more question though. The Time history i used here is El Centro Earthquake . It has its absolute maximum acceleration at 2.06s with an absolute value of 0.31882g. Should the structure not display the max response lets say in terms of strain at this time step? If i change the factor of the time history the peaks in the max strain curve shift left or right. But the absolute value will still remain at 2.06 s. In my understanding the structure should still exhibit its max response at this time step or am i missing something here?
Your help is much appreciated.
Regards,
Gaurav
I have also attached the Max strain curve which which i found the time where it was showing peaks (first peak=1.78s). I then searched the element having this behavior at 1.78 sec and proceeded to see its max stress strain curve which is also attached.
I have one more question though. The Time history i used here is El Centro Earthquake . It has its absolute maximum acceleration at 2.06s with an absolute value of 0.31882g. Should the structure not display the max response lets say in terms of strain at this time step? If i change the factor of the time history the peaks in the max strain curve shift left or right. But the absolute value will still remain at 2.06 s. In my understanding the structure should still exhibit its max response at this time step or am i missing something here?
Your help is much appreciated.
Regards,
Gaurav
 Attachments

 new.zip
 (251.88 KiB) Downloaded 94 times
Re: Section fiber stress results visualization
Hello Team,
i was wondering if you had a look at my model and the problem we talked about. It would be really helpful if you could help me with this one. Thanks a lot!
Regards,
Gaurav
i was wondering if you had a look at my model and the problem we talked about. It would be really helpful if you could help me with this one. Thanks a lot!
Regards,
Gaurav
Re: Section fiber stress results visualization
The stressstrain diagram seems strange just because you are sampling a few points. Increase the number of increments in your analysis and the output will be smoother.
Also, in the Rayleigh damping, I would use Kinit and not Kcurr. If you make the damping dependent on the current tangent stiffness, you may have numerical issues.
Finally, you can also try to use a transient integrator with numerical damping such as the HHT.
Last, but not least, try to understand why you have strain concentration in that end. If it's physical it's ok. Otherwise you have to make sure it's not a problem of coarse mesh.
Also, in the Rayleigh damping, I would use Kinit and not Kcurr. If you make the damping dependent on the current tangent stiffness, you may have numerical issues.
Finally, you can also try to use a transient integrator with numerical damping such as the HHT.
Last, but not least, try to understand why you have strain concentration in that end. If it's physical it's ok. Otherwise you have to make sure it's not a problem of coarse mesh.