Questions about Units, Self-weight, and UP elements

[Charon]

Dear STKO Team，
Hi，I tried to model a centrifuge test of group pile-soil interaction with a sine wave input . PDMY was used for the soil material and brickUP was used for the soil elements. the materials and elements used for the piles and cap are detailed in my attachment. Phased construction is used.

Now I have a few questions:

1. How are the units standardized?

I have seen your "Getting started with STKO" video tutorial and I learned that if I use 'm' as the unit of length, then the uniform units should be: Length: m, Time: s, Mass: kg, Force: N, Velocity: m/s, Density: kg/m³, Stress: Pa.

But, as I was browsing through the postings in the forum, I noticed that, again, using meters as the unit of length for modeling, people use at least two different uniform units when assigning values to PDMY material properties. Some are rho: kg/m³, refShearModul, refBulkModul, refPress, liquefac1: Pa. Others are: rho: ton, refShearModul, refBulkModul, refPress, liquefac1: kPa.

Which of these two is correct? I used kg/m³ and Pa in my model.

Another example is that the material I used for the cap is ElasticIsotropic, and in the properties of this material there is also the option of rho. Suppose my material density is 2800kg/m³, so here, should I fill 2800 with kg/m³ or should I fill 2.8 with ton?

2. How should the self-weight of soil, pile and cap be applied?

After browsing some posts in the forum, this is my current understanding, please correct me:

In my model, I can fill in rho in the material property of PDMY and bz in the element property of brickUP, after I fill in these two numbers, will they apply self-weight to the soil immediately after executing "add soil" in the analysis step? So I don't need to use VolumeForce and apply a LoadPatterns to apply the self-weight?

Similarly, the ElasticIsotropic material properties of the cap have rho, but if I don't fill in b3 in the properties of the elements of the bearing SSPbrick, they won't apply self-weight after the "add pile and cap" step in the analysis step? So I need to create a VolumeForce and then apply the self-weight to the table with a LoadPattern in the analysis step?

Honestly, I think my understanding of this may be completely wrong, and I have never had a thorough understanding of the self-weight issue. But I believe many STKO newbies will have the same confusion as me.

3. Is the element with UP very special, such as brickUP?

I have learned that elements with UP may have inertial effects when analyzed, for example, static cannot be used in gravity analysis, and the transient analysis option is needed, which also requires a particularly large duration (e.g. 1e+06s).

Also if the ramp is too short (e.g. 1s) when loading an element with UP, inertial effects can occur, right?

Is there anything else special about elements with UP that you can summarize for us, so that people can come to this thread to read these in the future?

4. A suggestion: the STKO team could regularly summarize the commonly encountered problems described by users in the forum. Really! Many very useful solutions usually require searching many posts to find them.


This is a very long post, and I hope that STKO team members who are at work and see it will not be intimidated, and that my questions and your answers will be helpful to future users learning STKO.

Best wishes，
Charon

[STKO Team]

1. How are the units standardized?

There are no units in STKO and OpenSees so you have to be consistent

If I use 'm' as the unit of length, then the uniform units should be Length: m, Time: s, Mass: kg, Force: N, Velocity: m/s, Density: kg/m³, Stress: Pa.

This is not completely true.
The rule is this:
Pick a unit for LENGTH and a unit for FORCE. The unit for MASS will not be arbitrary because FORCE and MASS are related to each other.
For example:
if you choose LENGTH=m, FORCE=N, MASS must be kg
if you choose LENGTH=m, FORCE=kN, MASS must be Mg
if you choose LENGTH=mm, the acceleration of gravity cannot be 9.8 (m/s^2) but 9.8E3 (mm/s^2)
etc...

Which of these two is correct? I used kg/m³ and Pa in my model.

It's fine, but just keep in mind the above rule

2. How should the self-weight of soil, pile and cap be applied?

Either using the body force in your Element Property (if the element gives you this option), or using VolumeForce which is an STKO automation to emulate distributed loads with equivalent nodal loads in load Patterns

In my model, I can fill in rho in the material property of PDMY and bz in the element property of brickUP, after I fill in these two numbers, will they apply self-weight to the soil immediately after executing "add soil" in the analysis step? So I don't need to use VolumeForce and apply a LoadPatterns to apply the self-weight?

Correct.
Just pay attention to what bz means in your Element Property.
For example in a stdBrick bz = body force (i.e. mass density times gravity acceleration component in Z)
In BrickUP instead it's only gravity acceleration component in Z, which is internally multiplied by the provided mass density to create the body force

3. Is the element with UP very special, such as brickUP?

UP elements are used to model fully coupled soil-fluid porous media.

I have learned that elements with UP may have inertial effects when analyzed, for example, static cannot be used in gravity analysis, and the transient analysis option is needed, which also requires a particularly large duration (e.g. 1e+06s).
Also if the ramp is too short (e.g. 1s) when loading an element with UP, inertial effects can occur, right?

Correct. This is due to how the fluid part has been implemented.

Is there anything else special about elements with UP that you can summarize for us, so that people can come to this thread to read these in the future?

Here you have some references:
https://opensees.berkeley.edu/wiki/inde ... References

[Charon]

Thanks for your thorough reply!

Now I finished calculating the model, however, when I compared the calculated to superporous water pressure with the results of the shake table test, I couldn't reach a result that matched the test. The point chosen is at a depth of 11m. I tried different permeability coefficients (from 2e-7 to 2e-4), and the best result is probably when the permeability coefficient is 2e-4 or 2e-5, but then the super-pore water pressure is only more than half of the test result, which is far from the level of liquefaction. Can you help me to check what is wrong?

I will attach the model with the diagram below.

The calculations may be time consuming , so if you need the database of the completed calculations, please let me know and I can try to upload it to Google Cloud Drive.

[Charon]

Dear STKO Team，
Hi，
A new development: I added 2% Rayleigh damping to the soil, and now the ultra-pore water pressure time curve in the deep part of the soil is in better agreement with the test results, but the ultra-pore water pressure in the shallow part (around 3m) can only reach about half of the test.
At the same time a new problem has emerged: the acceleration time curve in the lower and middle part of the soil has a huge oscillation in the second half of the loading (as shown in the figure), and the oscillation gets bigger the closer to the bottom.
Do you know how I should solve these two problems?

Best wishes，
Charon

[STKO Team]

Probably you can remove those oscillation using numerical damping.
Try The Damped Newmark (i.e. Newmark with gamma = 0.6, beta = 0.3025)

[Charon]

Probably you can remove those oscillation using numerical damping.
Try The Damped Newmark (i.e. Newmark with gamma = 0.6, beta = 0.3025)

Dear STKO Team，
Thanks for your reply！I used a Newmark factor of 0.6, 0.3025 numerical damping and 2% Rayleigh damping, and it worked really well, the oscillation was gone.
However, when analyzing the results, the acceleration amplitude of the soil obtained from the numerical simulation is particularly small at shallow locations and particularly large at deeper locations compared to the test results. Only at the points in the middle of the soil, the amplitude of the simulated and tested acceleration is more consistent. Do you know what causes this? How can I solve this problem?
I have attached my latest model file below.

Best wishes，
Charon

[STKO Team]

It's hard to reproduce experimental tests. You have to pay attention to boundary conditions, material properties etc...
This is not something we can do on this forum.

Other then this, you have to make sure the numerical simulation is correct from a numerical point of view (numerical damping for example, maximum mesh size as function of the shear wave velocity, time step, etc...)