asdeasoft.net

Dear Sir/Madam
I have been trying to model the elemental shear test on the mortar bed joint as per the details in the research article "Micro-scale continuous and discrete numerical models for nonlinear analysis of masonry shear walls" by Dr. Massimo. To simulate the uniform shear stress across the element, I used single triangular element (tri31) with one Gauss point. However, I could not reproduce the same results found in the paper. I hereby attach my model for your perusal. I kindly request your help to simulate it. Thank you.

There is something wrong with your test.

Your model is a unit cell (1 mm per side).
The results on the paper are for a 15-mm mortar joint.

So you need to divide the total applied Us (shear displacement) by 15, to obtain the shear distorsion(for a unit cell).
In the same way, the Gt and Gc in the reference are real fracture energies. Your model has the AutomatcRegularization, but your triangle has a characteristic length = 1. So you need to scale those energies by 15 (Gt = Gt(paper) / 15, same for G)
The applied force should be the vertical stress you want to apply, divided by 2, because the top side has only 1 node (while with a quad you would have 2 nodes).
Here is the model:
Your second option is you scale your model so that the sides of the triangle are exactly 15 mm.
In this case you just need to scale the applyed load = sigma_y * 15 / 2.
Here is the model:
Note 1:
In both models, I used the monitor function, to obtain the graphs you need in real-time. Note the scaling I used with both of them. See the differences.

To obtain the Us and Un from the 1mm model, I need to scale the abscissa x 15.
To obtain the stress I need to scale the reaction x 2.

In the 15mm model instead, the displacements are not scaled,
while to obtain the stress I need to scale the reaction force by 1.0/(15/2)

Note 2

:
You will see some differences from the paper because this test is a pure shear test. However, in the paper, the quad was embedded in other quad elements for the total length of the mortar joint (in fact in reality they are confined).
Probably you will obtain closer results if you fix Ux also at the bottom right node.
IN this way you are also confining the Exx strain.

Note 3

:
You can do the same without creating any mode, just use the material tester:

Dear Sir/Madam
Thank you for providing me such a detailed answers. Sincerely appreciate your timely responses. I just explored a little further based on your suggestions. For the models with right-bottom node Ux fixed, the results improved; actually, out of those two models (1mm and 15mm), 1mm model performed better than 15mm in every aspects. I also explored the material tester. It is a really valuable suggestion to quick idea. Yes, eps_11 of about of 0.0004 to 0.0006 (negative) gives nice results! I observed that for increasing confining pressure in Y direction, I had to also increase the confining strain in X direction.

I have one more question. We usually obtain the compressive stress-strain curves from conducting tests on a brick unit (size varies) and a mortar cube (50 mm size). Actually, the fracture energies to be input in the STKO's material section are Gc and Gt. Suppose the "auto-regularization" box is checked-in, is it correct that the Gc and Gt values should directly be worked out from those stress-strain curves?. I mean that if I have mortar cube tested with 50 mm side and obtained stress-strain curve, and now, if I want to do the above triangular model with unit cell, what Gc should I input into STKO's section when "auto-regularization" is checked-in?

Moreover, I was little bit confused that, if we notice, the brick unit sizes are different for different construction purposes, and we test them directly placing in UTM, so the Gc and Gt would vary according to the sizes, like half-size/full-size bricks, right?. At least, for mortar, it is somewhat standard as the size is kept constant. Thank you.

The concept of fracture energy is quite hard to understand at the beginning.

This is what you should do in general (I'm not referring to any specific material, mortar brick, or even concrete).

• Get the stress-strain (or stress-displacement) curve from your test.
  If the abscissa of your experimental data are strains, you need to multiply it by the size of the specimen orthogonal to crack direction, to obtain a stress-displacement curve. Then, the area underneath this curve will be your Gt (or Gc)
• Input that fracture energy as it is in the DamageTC3D material, if you check the autoRegularization.
• Keep in mind that the autoRegularization only makes sense during the analsysis, when you assign it to a mesh with a finite size. Instead, during material test, it does nothing, because there is no real mesh size.
  So just for the testing, you could manually divide the Gt and Gc by the size of your specimen.
  Once you are done with your material tester, put the real Gt and Gc and run the analysis

Dear Sir/Madam
Thank you so much. It is clear now.

Great. Good luck with your model