Internal forces calculations

lomo339

Hello,

I'm trying to model a steel plate supported by 5 pin reactions along each of its short edges. The dimensions of my steel plate are 2200mm x 2400mm x 12.7mm. I have a 145 kN load acting directly in the center of the plate.

I want to develop the internal forces on the reaction supports, but I can only see the reaction force in the plane of the point load. I need to develop the internal shear forces that come from the moment developed.

Is this possible on Mecway?

Thanks,

- Lemar

Victor

Could you please attach the .liml file or a screenshot showing the constraints?

At a guess, it could be that the constraints are only defined in one direction so they can't support forces in any other directions. You need 3 displacement constraints at each point for a fully 3D pinned support.

badbunny

When you say "shear forces from the moment developed" what do you mean? Do you mean shear force developed at the edge pins from the plate bending and trying to pull its edges inward? If so, then you need to enable non-linear geometry otherwise there won't be any membrane direction loading, only out of plane loading like you describe. The analysis you describe should be possible in Mecway, we just need a picture illustrating the plate boundary conditions to enable us to better advise you.

lomo339

Hello guys,

Thanks for the help everyone.

I have modeled my plate as a shell element bounded by 5 simply supported connections on two parallel sides. The simply supported connections are supposed to represent bolts that will restrain this steel plate. The others to sides are free. There is a pressure acting on a tributary area of 2m x 2m on the face of the plate. I'm trying to develop the shear forces within the bolts (or the pinned connections) to check for bolt failure modes. Essentially the force the bolts are experiencing inwards toward the plate, due to the pressure applied in the middle of the plate.

Victor: In my initial model I only had a displacement reaction in the z direction, the same direction my loading was occurring. However I have updated the displacement reaction in all directions, x, y and z, but still I cannot solve for the internal shear force.

badbunny: Yes you've got it. The shear force pulling the pins inward. I'm currently using a "Nonlinear Static 3D" Analysis method, but I'm unable to see the shear forces.

I've attached some screenshots and the .liml file for your viewings. Thanks for the continued support everyone.

Regards,

- Lemar

Victor

You can use external force in the solution to show the reaction forces on the supports. It sounds like the X components of those are the shear forces you're looking for.

Beware that these aren't simple supports, but have fixed rotations too. To make them simple supports, apply them to individual nodes, rows of nodes, or shell edges, not entire elements. The naming isn't very clear, but displacement really constrains displacement individually on each node in the selection, not for the whole selection.

lomo339

Hey Victor,

Thanks that helps a lot. I'm able to see the external forces acting on the node now. However they are pretty large forces acting on the single node and since I'm simulating a bolt to act as this node, is it acceptable to apply displacement reactions at one node alone?

To answer this question i tried refining the mesh around where the bolts would go and applied displacement constraints in x, y and z around the nodes the bolts should be placed. This helped out a bit, but I am still getting a max. force of 90 kN which seems too high to act on a single bolt with only a 100 kN applied force.

Is this happening because the constraints are not acting as one system, rather they have been modeled as many small constraints within the same vicinity. Is this acceptable? Or is there a way to correctly simulate a constraint, for ex. of a 3/4" bolt.

Thanks for the support.

Regards,

- Lemar

Victor

This is quite an effective force amplifying structure, so expect the bolt shear forces to be greater than the applied force.

In FEA, external force accurately balances the applied forces regardless of the mesh density or number of nodes constrained.

I checked by comparing external force to internal force holding the two halves of the sheet together along its central Y-oriented axis (the plane at X=1232 mm):

Internal force:
Stress = average of stress XX on top and bottom = 35 MPa
Area = 2308mm * 12.7 mm
Force = Stress * Area = 1.0×10^3 kN distributed over 5 bolts.

External force:
The model you sent also has 1.0×10^3 kN total X external force on the 5 bolts on one side. I found that total force by making an element selection where the constraint is and using Solution -> Sum to sum external force X over that element selection.

badbunny

Hi Lemar,

Victor is right about the total forces balancing, but the caveat on this is that the distribution of forces between your constraints isn't necessarily accurate. For example, if the point load causes artifically high displacement at that node (ie too flexible), then more load will go to other constraints. Also in your structure where the shear load is coming from the membrane loading, the shear flexibility at the constraint nodes might be changing the sag shape of the plate. Depending on the relative stiffness of the structure and its supports this may or may not be significant. In your case I think it might be significant.

The other thing to note with this load and BC approximation is that the plate is not really pinned at the bolts, but is supported and trying to rotate about some face/edge which is then trying to lever up the bolts (prying) as well as pull them inward, ie there is an effective moment constraint to represent at your single node constraints too (which cannot be represented at a single solid element node). The result of this is that your model will be showing the bolts are in axial compression, whereas they will actually be in prying tension. For the shear load you need to consider whether the bolts will definitely grip (if the numbers are indicating that is feasible), ie how certain are you of the friction and preload? If they do grip, then the load won't be supported by the bolts but by the friction between the plate and support. Also one final thought, is the plate and its support frame static after it is bolted down, or do you need to consider dynamic loading on the assembly?

Normally I would carry out a series of sensitivity analyses considering the significance of a simplified constraint approximation to the result of interest, and potentially move to a more elaborate bolted joint representation (or change the design to behave more simply). For example, what if the bolts grip/don't grip, what if they do/don't restrain moment, etc.

In your case with 5 pairs of bolts along opposite edges it is fairly straightforward to use quarter symmetry and explicit bolt representations for your whole assembly. Alternatively you could represent a 'half strip' of your plate, ie half of the plate width, and lengthways include half of a bolt and half of the plate width to the next bolt. This will give you much more insight into what is going on. I think there is an example in the mecway manual for bolt pretension. To be honest, although the single node support method is initially quicker, I think it will take more overall effort validating that bolt simplification than just modelling them explicitly in the first place.

Pete.

badbunny

One other complication that just crossed my mind is that the plate will sag before it is bolted down, so its initial shape isn't flat before it is bolted down and the 145kN mid load is applied. This might be beneficial, but is more complicated to represent, ie you would need to represent gravity sitdown, then increase bolt pretension, then apply mid load.

Pete.