Reply To: Too high stress in a plate

[peteroznewman]

Hi Max,

Let me check my understanding.

• You have 12 mm diameter glass-filled plastic pins that will have concrete molded around them.


• The concrete panel is 3 cm thick and the pins can be embedded to some depth where the concrete will bond to them.


• The depth of the pins can be between 0 and 3 cm into the concrete.


• There will be a pressure load on the face of the panel and you are interested in the stress in the concrete.

Given that, I expect the peak compressive stress to be where the pin and concrete meet on the back of the panel, but the peak tensile stress may be on the front face of the panel. Therefore, you must build a 3D solid of the panel, with blind holes with a 12 mm diameter where the pins exist, and pins that fill those holes. The easy way to make the holes is to use the pins in a Boolean subtract. For a first model, you can put the all parts (9 pins and panel) into a single part in DesignModeler (Form New Part). That way, the mesher will create shared nodes at the coincident faces and that will "bond" the pins to the concrete without using contact in Mechanical. I would cut off the pins at the plane where they emerge from the support block and hold those faces fixed. Don't even model the support block. Add pressure load on the front of the panel.

You must ensure that there are at least two layers of solid elements in the thickness of concrete that matches the depth of the holes, and two layers of elements in the pin that is in the hole. These conditions will avoid "pivot" errors from the solver. An easy way to ensure the two layer minimum is to create a plane at the bottom of the hole and slice the concrete at that plane. You can then sweep that body in meshing and specify the number of elements. You might want an lot more than two elements to resolve the peak stress.  Do the same with the pin by creating a plane on the back face of the panel, and use that to slice all the pins.

Since it is concrete, I expect the compressive strength is much higher than the tensile strength. You might consider how you will calculate a failure metric that accounts for this difference in strength. Also, what about gravity? Doesn't the weight of the panel deform the pins in a vertical orientation of a panel? Finally, I do think there is a singularity in the model I described, since there is a sharp interior corner at a point of high stress.

Best regards,

Peter