Learning Forum

[Aslinn]

Hi,

I am working on a pushover analysis on a 5-storey masonry building in Ansys workbench, but I think I'm doing something wrong because my displacement keeps growing...basically I don't see any non-linearity in my results. Could someone please give me some hints? My questions are:

1. How do I extract base shear from the results? I am currently using the support reaction. Is this correct?

2. How do I define the load multiplier? I am defining incremental loads using load steps. Is this correct?

I am using the default concrete NL material for now, so I think it's not the material properties issue. I have attached some images showing key setting. 

Figure 1 Analysis setting

Figure 2 Applied loads

Figure 3 Capacity curve (obviously wrong)

I would really appreciate it if someone could give me some help.

Best Regards,

Aslinn

[Wenlong]

Hi Aslinn,

 

Before attempting to address your question, I would like to ask for some clarifications:

1. What is the x and y axes meaning of Figure 3?

2. What are your boundary conditions?

3. Can you please provide a screenshot of the concrete material model? I am guessing that the only effective part of the material model is the Elastic modulus, and that could be the reason for your elastic response. 

If you can provide more details maybe I can provide more of my thoughts. Now regarding your questions:

1. Yes, I would use the reaction force to obtain the shear force at the support. 

2. Yes, I would use load steps to define incremental loads to avoid sudden change of load amplitude.

 

Regards,

Wenlong

[Aslinn]

Hi Wenlong,

Thank you for your quick reply. To answer your questions:

1. In figure 3, x-axis is the total deformation, y-axis is the force reaction, both directly extracted from Ansys results

2. The models are fixed at the bottom, as shown in figure 2, the only applied loads are gravity loads and horizontal force at each floor level

3. The material property is shown below. I didn't change anything from the default...maybe I should?

I hope this information is helpful. Please let me know if you need more information.

Best Regards,

Aslinn

[Wenlong]

Hi Aslinn,

Ah, so the material you defined is an isotropic elastic material since you only defined Young's modulus and Poisson's ratio, and in this case, your model will only behavior linearly. 

So to solve the issue you will need to find the correct material properties, maybe adding some damage or as least hardening to the material (these are just suggestions based on my initial impression). I would recommend referring to the test data or literature to determine the best material properties to use. 

Regards,

Wenlong

[Aslinn]

Hi Wenlong,

Thank you for pointing that out. I have tried to add the multilinear isotropic hardening curve into the material model and saw the expected capacity curve shape in the result. However, I am using a concrete model for now, because I have some difficulties defining the masonry:

1. Masonry has different stress-strain relationship for compression and shear, how should I include that in my material property? Or would we assume that shear is more important so we only include shear?

2. After yield, the capacity of masonry drops as shown below, and it seems Ansys does not allow such behaviour. Is there anyway to include it in the material model?

 

Best Regards,

Aslinn

[Wenlong]

Hi Aslinn,

1. So for geomechanical materials like concrete or masonry, you can check the options available like Druker-Prager, Mohr-Columbs, and so on. Please refer to https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_mat/mat_geomechanics.html for more information. If you have trouble accessing the ANSYS Help, please refer to this post: /forum/forums/topic/how-to-access-the-ansys-online-help/

However, I would suggest you work with simple material models and figure out the softening behavior first before you move to more complex geomechanical materials. 

2. Softening behavior can also be defined with geomechanical materials like Druker-Prager material. However, you will definitely have convergence challenges when softening behavior happens. In that case, you can try either the "stabilization" or "Arc-length" method. Please refer to this page for more information: https://ansyshelp.ansys.com/account/secured?returnurl=/Views/Secured/corp/v201/en/ans_str/Hlp_G_STRUNST.html

Regards,

Wenlong

[Aslinn]

Hi Wenlong,

That's really helpful and I didn't know I could bypass the portal login before LOL. Thank you very much.

Best Regards,

Aslinn

[Wenlong]

Hi Aslinn,

Good to know it is helpful. If you think this solves your problem, please click "is solution" button so that we know the issue is solved. 

Thanks!

Regards,

Wenlong