asdeasoft.net

Dear Sir/Madam
I would like to simulate a diagonal tension test of masonry assemblage as shown in attached figure. There are two metal shoes, respectively, at top and bottom with a bearing length of about 200 mm along the edges. To model the BCs, I fixed the Ux and Uy at all nodes along the 200 mm shoe length at the bottom, and applied EDOF Uy and Fixed Ux at all the nodes of the top 200 mm shoe length. Specimen is 1.2 m x 1.2 m, Unit dimension is 190x90x90 mm3 and mortar thickness is 10mm. I followed DamageTC3D material and assigned appropriate properties for unit and mortar. I want to monitor and top Uy vs ReactionForce at the restrained nodes from the bottom. I used LoadControlled sp to impose displacement Uy=-1 mm at top node to apply the vertical load. The problem that I face now is that there is convergence issue! Can you please help me to figure out the solution for it? Thank you

P.S: Also attached is the STKO's model here

The reason for non-convergence is related to an issue in your model.
Some of the faces have a normal vector pointing in the negative Z direction. This is not allowed in 2D analyses, because a negative normal vector will result in a negative area (the Jacobian determinant will be negative) in the 2D finite element.
If you build your model directly in the X-Y plane STKO takes care of making the faces points into the +Z direction. Probably you did some rotation or other CAD commands that made the face point into different directions.
However, in these cases, you can use the Reverse command (to change the normal vector of faces or the tangent vector of lines).
In this case, I used the "Make Coherent" option, to make all faces point into the [0,0,1] vector (+Z).
Keep in mind that now, if you move or change your geometry, you need to repeat this step!
Look at the dark faces in this image, they have a normal vector in the wrong direction:
I also changed some other minor issues:

• You don't need a node force, since you are applying a displacement. The force will be the reaction to that displacement. You cannot apply both.
• Your applied displacement was 0.003, I changed it to 1[mm]
• You don't need a EDOF(Y) on top. In fact if you apply the Uy displacement to all nodes of the metal sheet, they will already move of the same amount.

Here is the modified file and the output:

Dear Sir/Madam
Thank you so much for the response. I sincerely appreciate your customer support by providing clear and succinct answers.

Glad we could help!

Dear Team,

I tried to model the diagonal compression test as given in above reply, but I am getting an error attached below. Any suggestions would be appreciated.

Regards,
Zeeshan Bhat

Some of the faces have a normal vector pointing in the negative Z direction. This is not allowed in 2D analyses, because a negative normal vector will result in a negative area (the Jacobian determinant will be negative) in the 2D finite element.
If you build your model directly in the X-Y plane STKO takes care of making the faces points into the +Z direction. Probably you did some rotation or other CAD commands that made the face point into different directions.
However, in these cases, you can use the Reverse command (to change the normal vector of faces or the tangent vector of lines).
In this case, I used the "Make Coherent" option, to make all faces point into the [0,0,1] vector (+Z).

You have the same problem, some faces are pointing downward, so use the Reverse command, select all the faces, and choose "make coherent" with vector 0,0,1. This will make all the faces point towards the global Z direction

Thank you so much. it is now working.

Regards,

Zeeshan

Great! Happy modeling

Dear Team,

I modelled the diagonal compression using shell element, But I am not getting any damage in my results section in postprocessor. However If I change it to plane stress quad element , then I am getting damage in postprocessor. Any Suggestions will be appreciated.

Regards,

Zeeshan

Dear Mr. Zeeshan
According to my knowledge, you should have selected section.fiber.damage in setting up parameters in MPCO recorder. Additionally, if you want to see strain and stress, you should also select section.fiber.strain and section.fiber.stress. It is because the 3D material is converted accordingly to the shell definition, so, we need to go ahead with section.fiber to record such responses. Thanks