Concrete-concrete bonding

gemada

Hi Victor,
I'd like to model the shear stresses resulting form a concrete to concrete bonding slant shear test. I've tried to model it in 3d but the results are very strange...i believe it´s because of the mesh limit in the free version. I've also tried to reproduce it in 2d but the results are also strange. I'm attaching an extended abstract for you to see how this was made by a researcher in other fem software. I'm also attaching my 3d model in mecway. Can you help me?
Best regards

Victor

Hello Jacinto

I'm not sure if you're trying to model the bond strength itself as the pdf say, or the rest of the material. If the rest of the material, then the problem is that the two parts are only connected together at the corners. To see this, use View -> Open cracks. To fix it, use Mesh tools -> Merge nearby nodes and enter something small like 0.1mm. Then it'll become one single object.

Mecway doesn't have an equivalent of Abaqus's cohesive elements, so you won't be able to do that directly.

gemada

Hi Victor,
Thanks again for your support. I would like to build a graphic with the evaluation of the shear stress in the interface (like the one in the pdf). Is there a way of indirectly simulating a cohesive element in the bonding interface with Mecway?

Victor

Hi Jacinto

Here's an example showing just a linear analysis of the shear stress at the interface. I rotated the model so that the XY stress component is aligned with the interface and you can read it off directly. I also rotated the X and Y displacements constraints by the same amount. Note that the slope of the interface isn't exactly 30 degrees. Maybe about 2 degrees out.

After solving, open the Table in the solution to see the shear stresses along the line of nodes in the interface. You can copy this table to a spreadsheet or other graphing program.

gemada

Thanks once again Victor. I've done that but the shear stress distribution along the interface is completely different from the expected results(see the excel screenshot). I believe this is due to the modelling of the interface (it should be cohesive). Could it be simplified in Mecway using a thin bonded layer of a different material?

VMH

I think one of the reasons for the different could be assuming linear elastic material instead of taking into account of material nonlinearity at the bonded interface for the bonded material. In general, once the area of high stress exceeded the linear range, the stresses shred to other areas instead of continuing to increase stresses in that area (without limits) as seen in the Excel screenshot. If the stresses are too high, the solution may diverge indicating that the applied loads may be too high to obtain a converged solution.

I'm not sure how to model concrete type element for material nonlinearity. CCX option in Mecway has geometric, material and contact nonlinearities. For material nonlinearity, it's referenced to equivalent vonMises stress and equivalent plastic strain so I'm not sure of the correlations between those and concrete modeling.

Abaqus "cohesive" contact may have input for normal strength, shear strength, frictions, etc. that handle all of the nonlinearities that may exist.

VMH

I read through the referenced paper. In my opinion, the simulation section is very limited and doesn't say much on the different modeling approach for the different cases. It seems like "cohesive" bond is just a general type contact (nonlinear).

VMH

I modeled half of the block 75mmx150mmx450mm and used symmetry for the other half. I assumed linear elastic material as the PDF mentioned (assumed E=30MPa based on Mecway provided model). As for the "cohensive bonding", I used frictional contact (nonlinear) with assumed friction coeff. of 0.7 as an initial test case.

For the boundary conditions, fixed support used at the bottom block, horizontal translations restrained at the top block, frictionless support used on the side of both the top and bottom blocks to simulate symmetry, and applied inline (inward) displacement of 1mm to the top block.

I didn't use CCX option in Mecway for this run because I'm still in the process of learning CCX so I use another software. The purpose of posting the attached screenshot is not for comparison of Mecway to any other software but just to show that it may be difficult to obtain the results from the "numerical modeling" section of the provided PDF because it lacks so many info to try to replicate the results. Best wishes and hope you can replicate the PDF results.

Victor

What features of the shear stress plot concern you? It does seem to have the same general shape as the RAC-RAC curve in the pdf but the stress is scaled by some constant. I couldn't get the 70MPa you did and all my stresses were less than 0.1Mpa with displacement changed to 1mm and the geometry scaled up a bit.

If you use different Youngs modulus on each material, you get an S-shaped graph like for the other curves shown in the PDF.

I assume the cohesive contact didn't open at any point, so it might be equivalent to merging the nodes together in Mecway. Though I don't know if Abaqus's cohesive contact has some elasticity or other properties.