Plate boundary conditions

[Anonymous]

Hello,

I'm new with the software and i'm having trouble with a plate which is the base of a machine. I don't know how to model the boundary conditions. The plate is freely supported on the floor (no DOF restrictions just -z).

As shown in the image, it is a baler machine and the plate connects the four vertical beams (traction) with the four horizontal "U"beams (compression).

Any ideas to model the supports/constraint?

Thanks.

[sebastian.sosa]

Hello,

A couple of thoughts,
If you are running a static stress analysis then I think having just the Tz restriction on the bottom plate is not enough. You need a statically stable model in order to get meaningful results, so you shhould restrain, at minimum, translation in all directions for your model.
If your model is symmetric for both vertical planes, then you might want to take advantage of that and model just a forth of the entire model and use de cutted edges to apply symmetry boundary conditions and that way you will restrain the model for that "in plane" translation.
Finaly, you might want to check the TZ restraint you applyed. In your description you stated that the plate is prevented to move in the -Z direction, so does that implies that it is free to move in the +Z direction? If so, takinng into account that you have some loads applyed in the +z direction, restraining the TZ for that plate is not entirely accurate since it would prevent that plate to move in the +z direction. You might want to take a look of something like "gap elements"

Best regards

[John_Holtz · Accepted solution]

Hi imatiasmb,

I agree with everything that Sebastian wrote.

Assuming that the weight is larger than the upward forces (or maybe there are bolts that hold the plate to the floor) so that the model will not fly upward, then what you need to do is model the floor and create surface contact with the floor. Here are two ways to do it:

1. Add a new part to your model for the floor. Then select the floor and the plate, right-click "Contact > Surface".
2. Use the "manual" method to create the contact with the floor as described in this article "How to define a unidirectional constraint in a Simulation Mechanical linear analysis"

In addition to Sebastian's suggestion of using symmetry to provide stability in the X and Y directions, you can also use weak springs to prevent the model from "floating off into space". Please see the page in the Help > User's Guide > Perform Analyses with Gap Elements. (You need to keep in mind that the analysis is calculating the displacement in X, Y, and Z regardless of the loads, and it does this by calculating force/stiffness = displacement. When the stiffness is practically 0 in some direction because the model is not constrained, then force/practically 0 can give any result the computer wants.)

[Anonymous]

Thank you both!

Trying to clarify a point that seems to be confusing (my bad) is that the plate is lying on the floor, no bolts, no weldment, it's just put it there on the floor (like a table, or a couch). And no, the machine wouldn't fly because the upward forces that are shown in the image are reactions of the compression that the hydraulic cylinder applies to the elements to be baled. In other words, there are forces applied (downward) too on the surface of the horizontal "U" beams. It's difficult to comunicate to me at some point because im not english native speaker, sorry for that.

The thing about Gap Elements, acording to what I read here in Autodesk Community is that in order to apply the correct stiffness, you have to know the displacements before running the analysis, which I don't, so it becomes an iterative process that, to be honest, I dind't come to understand very much, because as I said, I'm new with CAD and even more so with FEM analysis.

About the creation of a new part to represent the floor, sounds logical and much simpler. I will go this road and see how it goes.

Thanks again.

[Anonymous]

And here is it.

As you told me, I created a floor part and applied Surface Contact, and it worked!. To represent the downward reactions I used 1D springs on top of the "U" beams in Z direction, apparently 100000 stiffness was too much, but will refine that.

Here's an image of the results.

Thanks!

[John_Holtz]

Hi imatiasmb,

Your English is very good -- probably better than mine.

I think we were confused about the loads in the model because we could not see the forces on the top of the channels. You do have loads applied in the -Z direction acting on the channels. Correct?

So in theory the upward force from the cylinders balances the downward forces from the cylinder. In the mathematical reality of simulation, the two loads are unlikely to balance. And even if the two loads did balance exactly, there is still the problem that the simulation is trying to calculate the displacement in the Z = sum of forces in Z / stiffness in the Z, and without some type of restraint in the Z direction, the stiffness is theoretically 0 (and mathematically close to 0). This is a potential problem.

To prevent the mathematical problem, the easiest solution is to do this:

1. Pick three random nodes on the model (such as three corners of the plate)
2. Add 3D springs to the three nodes
3. Fix the X, Y, and Z directions. (This will solve the stability problem in all directions that Sebastian was referring to)
4. Set the stiffness of these springs to a small value. (1 may be a good number.)
5. After running the analysis, look at the axial force in the 3D springs ("Results Contours > Other Results > Element Forces > Axial"). Since these springs are tying the model to the ground (just like a boundary condition, but with a specified stiffness), you do not want the result to be very large. If the axial force is a significant portion of the applied loads, then the stiffness of the 3D springs is too large.

Hopefully that makes sense. If so, there are probably three nodes that are better to use than 3 "random" nodes or 3 corner nodes, but the end result should be same regardless of which nodes have these "weak springs".