mass assignment in face

[alokbhatta]

So, my question today is related to the mass assignment leading up to the eigen value analysis of the model. The wall system on the masonry building is characterized by shell element and the mass assigned is 8e-04. I have assumed a mass density of 2200 kg/m3 in stone masonry wall. All my physical properties are in N and mm. And so, I convert kg/m3 into kg/mm3 and then multiply by thickness (350 mm) to get 8e-04 kg/mm2, which is what I am assigning as face mass in the shell element (I request you to please check my model attached for verification). However, I don't think it's right because the eigen value is giving a very high time period, when the correct time period should be around 0.1sec for a building this size. At this point, I need probable modifications to my model and help with this particular issue.
I have attached my model; can someone please see as to what I am assuming wrong? I hope my model makes sense.
Thanks in advance!
Some of my doubts include:
1) I have my properties messed up with the elastic and inelastic parameters of stone and mortar.
2) My unit conversions are incorrect.

[marafini.f]

Hi alokbhatta,
I downloaded and tried to run your model to figure out how to help. Could you check if this is the right model you wanted to send? Because the analysis steps you set up do not record any output, and only the eigen command is called, which in STKO do not provide any derived qualities from the eigenvalue analysis like frequency and participating mass. How did you obtain the period value you were talking about?

I suggest you read this whole thread I answered a few days ago.
viewtopic.php?f=33&t=1823

It's called "Time history error" but if you read forward, especially at this post viewtopic.php?f=33&t=1823#p2886 you will find a through explanation of all the possible ways to run an eigenvalue analysis correctly in STKO.
Also check out this webinar for more information on the new functionalities available in STKO version 2.0
https://www.youtube.com/watch?v=vUXKVm5 ... e=youtu.be

I didn't have time to go through your properties and calculation. But my suggestion is to first set up your analysis the best way possible, so you are sure you are obtaining in fact the right result, and once you know that's not the problem retrace your step and check the rest.

Hope this helps.
Enjoy your modeling
Francesca

[STKO Team]

Your mass is wrong by a factor of 1.0E+3!
Keep in mind that when you assume a mass of 2200 kg/m^3, you were assuming the SI unit system with N and m. So g = 9.81 m/s^2.
It is not sufficient for you to divide your 2200 by 1.0E9 (1/m^3 -> 1/mm^3),
because in N - mm, g becomes 9810 mm/s^2!

A small matlab script that can be useful for you to check your unit system, I see this error very often!

Finally you will see that your rho_shell (mass density times the thickness of the shell) is : 7.70E-07 <N*s^2/mm^4>


N = 1;
mm = 1;
kN = 1000.0;
m = 1000.0;
s = 1;

w = 21.582*kN/m^3
g = 9.81*m/s^2
rho = w/g
thickness = 350.0;
rho_shell = rho*thickness

[alokbhatta]

Hi Francesca and STKO team,
Thanks for all the help. Also, leading from the previous question regarding face mass, what would be the units for edge mass assigned to linear elements? In my case, the wood weight density is 7000 N/m^3. So, what would be the value of edge mass applied at the wood truss? My calculations were as follows: =7000*10^-9 to change it to N/mm^3; divide it by g= 9810; and multiply it by width*height (180*90), to get 1.2e-05 N*s^2/mm^3 (per unit length). Please correct me here as I am not confident about the units again for edge mass.
After the above roof edge mass was applied with along with the face mass, I am still getting a time period of 1.2 seconds. So, could you please check my model (attached) that should be loading correctly now. I apologize for the previous model for being incomplete.
After the eigen value analysis, I will go forward with gravity analysis and transient analysis. I was told by Dr.Petracca to remove the roof trusses to simplify my model. However, I wanted to see if I could work with keeping it as a offset and creating a interaction. However, I am not sure what constraints should I be using in the interactions. Right now I am fixing all DOFs. I will appreciate any improvement suggestions to my model as I begin with IDA pretty soon after this.
Really grateful for all the guidance!
Thanks,
Alok

[STKO Team]

In my case, the wood weight density is 7000 N/m^3. So, what would be the value of edge mass applied at the wood truss? My calculations were as follows: =7000*10^-9 to change it to N/mm^3; divide it by g= 9810; and multiply it by width*height (180*90), to get 1.2e-05 N*s^2/mm^3 (per unit length). Please correct me here as I am not confident about the units again for edge mass.

That's correct.

The reason for your strange periods is that your model geometry is messed up:

• Your walls have many unconnected faces (look at the free edges in this image)

  

  freededges.png (270.21 KiB) Viewed 5240 times

• Also the interaction with the roof are wrong. You should select the roof as master, and the wall-tops as slave.
• Finally you should create a fake (0-step) analysis before the eigen command, because otherwise OpenSees will use the transformation and it will not handle correctly all those constraints.

With the fixed model I obtained a period of 0.05 seconds.
However the first modes are all related to the roof beams, and they excite a very small amount of mass.

Probably you can consider, removing the edge mass from the roof beams, and lump it onto the wall tops using proper tributary area. In this way, only the wall geometries will have masses. So you can exclude the vibration modes of the roof beam that are not interesting for you

Here is the fixed model.
Try to move the roof mass from the beams to the top-walls and see what happens.

masonry11.zip

(6.94 MiB) Downloaded 222 times

One more note.
In the attached mode, I used the modalProperties command that we introduced in STKO v 2.0.0 (instead of the custom script).
To use it, you can download the STKO v 2.0, and the new OpenSees-Solvers from prof. Tarque's website.
Let me know

[alokbhatta]

Hello,

Thanks a ton for the revised model and all the advice regarding edge mass. When I assigned the roof mass into the walls itself, the time period came around 0.17 which is good.
Moving on now to the dynamic analysis,
The attached model and some image screenshots of the output:

output 0.4g.PNG (150.05 KiB) Viewed 5228 times

I have cut the analysis short to 15 secs of the ground motion and expecting to see damages in both adjacent walls as ground motions are applied in both x-dir and y-dir. I am using Volume Color Map and the magnitude of displacement to check corresponding displacement magnitude:

outputparameter.PNG (7.76 KiB) Viewed 5228 times

. I am not sure about the drastic out-of-plane deformations I am getting early in the analysis, before I can correctly observe hairline cracks and all.
However, using the fiber heat map, I did see that the stress concentration was first focused at the gable walls and then the in-plane mail walls, as the gable toppling comes under one of the first damage state criteria for fragility curves, which was positive.
I saw on Dr. Petracca's paper that other parameters like d+ and d- and strain was checked. Also, I am aware that a control node could be set at the top or middle of the wall, using monitor function. Actually, I am not sure about my analysis as the damage is seen to be very localized and drastic. Can you please lead me towards a better output parameter and also check that the model is behaving well? I cannot post the whole output file. But, it would not take long as the time series is just 15 sec.

masonry_alok.zip

(7.49 MiB) Downloaded 222 times

Appreciate all the help!

Best
Alok

[Clarabella]

Dear Alok,
I made few changes in the model, I suggest:
1) Use ASDshell, the performance is much better than MITC4 (see our validation manual)
2) Reduce the step. The model is IMPLEX, so explicit at material level and it requires smaller time steps. I used 1/10 of the your dt =0.01
3) I would add the lintels to the model.
4) Show the damage as shown in the pictures, I suggest using "hot" colors. It is clear that the building is failing out of plane, vertical cracks and horizontal cracks in the picture
5) There are several Engineering Demand Parameters for continuum models to evaluate the damage. The problem is quite complex. We are preparing a document to explain how to make a 3D continuum model efficiently for students and researchers.
6) I also suggest to make two separate models: 1) for the eigenvalues 2) for the TH. For the TH use 10 processors if you have the possibility.
Regards

[alokbhatta]

Hi Ciarabella,

Thank you for all that you shared. I am ready to try all that you suggested in my model. But I wanted to clarify a few things first.
1) I am slightly worried about having to increase my time increment to 0.001s as you suggested, since I am already struggling with trying to minimize the computational time and output file size with 0.01s. For around 40s ground motion, it would take me a lot of time (around 2 days, presumably), so can you suggest me some ways to reduce file size as well? I understand what you said regarding the model being IMPLEX though.
2) I am planning to add in lintel beams just at the top of the window level. Presumably, I will add a force beam element with reinforcements assigned right? Wouldn't the meshing in the wall system get affected due to introduction of this lintel beam in the middle of the wall?
3) I see that the outputs are shown quite clearly using d+/d- EDP. However, how will I measure the displacement of walls through this EDP? I intend to draw out fragility curve.

I am looking forward to reading through the document that is being prepared. Please let me know around when would it be available.
Best Regards
Alok

[STKO Team]

1) I am slightly worried about having to increase my time increment to 0.001s as you suggested, since I am already struggling with trying to minimize the computational time and output file size with 0.01s. For around 40s ground motion, it would take me a lot of time (around 2 days, presumably), so can you suggest me some ways to reduce file size as well?

In the MPCO recorder, you can specify the output frequency. By default, it records at every time step. You can reduce it by setting the output frequency to "every dt" = 0.01. So it will record every 0.01 seconds. (or even larger if you want to save space).

2) I am planning to add in lintel beams just at the top of the window level. Presumably, I will add a force beam element with reinforcements assigned right? Wouldn't the meshing in the wall system get affected due to introduction of this lintel beam in the middle of the wall?

It will not affect the meshing, because you don't have to draw a new geometry. You can just go in sub-selection mode (select only edges), and select the edges of the shells (for example the top edges of the window holes) and assign a Physical Property and an Element Property to them. When they have an Element Property assigned, STKO will automatically create an OpenSees element for them.
And since they are the boundary of the faces, beams and shells will share the same nodes.

3) I see that the outputs are shown quite clearly using d+/d- EDP. However, how will I measure the displacement of walls through this EDP? I intend to draw out fragility curve.

I don't think you can use the Damage as a measure for the wall displacement. You can just measure the wall displacement at some significant point

[Clarabella]

Hi Alok,
1) I am slightly worried about having to increase my time increment to 0.001s as you suggested, since I am already struggling with trying to minimize the computational time and output file size with 0.01s. For around 40s ground motion, it would take me a lot of time (around 2 days, presumably), so can you suggest me some ways to reduce file size as well? I understand what you said regarding the model being IMPLEX though.
I understand your concerns. You can try with 0.005, but I would do some calibration to ensure you get the correct results, otherwise you can change the material to work in implicit, try it! I suggest to reduce the duration of the ground motion to 25 seconds (most of the standards require 10 seconds + 15 seconds)

2) I am planning to add in lintel beams just at the top of the window level. Presumably, I will add a force beam element with reinforcements assigned right? Wouldn't the meshing in the wall system get affected due to introduction of this lintel beam in the middle of the wall?
Use a displacement beam element, it can be also elastic, it carries only the vertical load. Tip: Make sure to model the beam allowing slip between the beam and the masonry

3) I see that the outputs are shown quite clearly using d+/d- EDP. However, how will I measure the displacement of walls through this EDP? I intend to draw out fragility curve.
Using the new python interface you can write a simple code to measure the panel drifts during the NLTH. The new interface was created exactly for this type of problems. You can measure instaneous, average, maximum, whatever you like. Follow our next webinars