Spring Connector Floating Body Issue

[Anonymous]

Hi,

I'm trying to perform a mass spring system on Nastran in CAD but I keep getting failures.

I have applied 3 points on one of the faces of the concrete block and another 3 points on the opposing face of the concrete block. I then applied 6 point perpecdicular to those points on a sketch I created on an offset plane. I then applied rigid connections in all direction between 4 points and their corresponding edges and 2 points and the faces they sat on. I then applied a fixed constraint to all the points on the sketched plane. I then made a spring connection between each two corresponding point and applied a gravitational load.

I keep getting errors regarding this analysis with these constraints. Is there a better practice of doing this problem?

Thanks,

Akshay

[John_Holtz]

Hi Akshay,

I have a couple of questions regarding your analysis.

1. What error are you receiving?
2. What prevents your model from moving in the X and Z direction? Is looks like you only have support (the springs) in the Y direction. You need to prevent the model from moving in the X and Z directions, too.

______________________________________________________________

If my post answers your question, please click the "Accept as Solution" button. This helps everyone find answers more quickly!

[Anonymous]

Hi John, thanks for the reply.

1. The error I am receiving is T2044.

2.The T shaped concrete block is meant to move in all directions, I want to see how it acts with the supported springs on the points I have chosen. Those springs are actually seismic isolators that sit underneath concrete blocks to absorb vibrations. They are just models as springs for simplicity.

[John_Holtz]

According to this article, the T2044 error occurs because you have multiple rigid connectors that are attached to the same nodes. (Error: "Fatal error T2044" in Nastran)

The article suggests using beam elements instead. In your case, I would suggest that you split the surface of the CAD model so that you can apply the rigid connectors  to areas that do not touch each other. In other words, each rigid connector will use a different set of nodes.

The static analysis will not work properly if any portion of the model is free to move in X, Y, or Z translation, or rotate about X, Y, Z. Something in real life is preventing the structure from moving freely in the X and Z directions, so that is what you should try to duplicate. (My guess is the isolation pads have stiffness in the horizontal directions, or friction, so the easiest thing for you to do in your model is to add X and Z stiffness to the springs.)

[Anonymous]

Do you mean a split like in the image attached, and then have the spring connector attach to one of the vertices?

Even in reality the model is free to move in all directions, but of course there will be more resistance in certain direction than others due to the rubber padding on the isolators and stuff. I will try with the stiffness value in all translational directions first and see what happens

[John_Holtz]

I do not fully understand the images of your model. Based on your description of the 3 connectors and 3 springs per side, I thought that it was something like this:

Figure 1: Original faces. The connectors 1 and 2 share the same nodes along the common edge (green arrows).

To avoid sharing the nodes, you need to split the surface so that there is a gap between the connectors, like this:

Figure 2. Gap between the faces used for the connectors.

[Anonymous]

So do you mean creating three parts, and then adding a surface contact between all three parts so that they act as one model?

[John_Holtz]

A simpler way is to create a sketch that is the outline of the face. In the modeling environment, use the "3D Model > Modify > Split" command to create the surfaces. (I think you need to do this when editing the part. I think you cannot split faces on a part when working on the assembly.)

This methods keeps the model as one part; it just has additional faces/surfaces.

P.S. You also use the Split command to create a smaller face when you want to apply a load or constraint to a smaller region of a face.

[Anonymous]

John,

After inputting values for stiffness on the x and z lateral directions and having a split faced model, I have gotten a new error, E5001. which means that a negative term has been detected at the stiffness matrix. It could also mean that the model is running with too few constraints, but like I stated earlier, the block itself is essentially floating. It is only dependent on the springs being attached to the ground.

Any ideas?

Thanks,

Akshay

[John_Holtz]

Hi,

My only thought is that the workpoints used for the rigid connectors, springs, and constraints are somehow different.

In order for everything to be connected together, the rigid connector needs to be connected to "workpoint 1", the spring needs to be from "workpoint 1" to "workpoint 2", and the constraint applied to "workpoint 2". I have seen some cases where there are multiple points at the same coordinate, so one of the three items (connector, spring, or constraint) gets applied to the wrong CAD geometry. For example, the constraint is applied to "workpoint 3" instead of "workpoint 2", so the spring is free to move as a rigid body.

If you are still having problems, feel free to attach your part file to the forum. Someone will be able to track down the problem.

[Anonymous]

Hi John,

Yes I have checked my work point configurations for the springs, rigid connections and constraints. I will attach my work file for you or anyone on Autodesk to look at.

Thanks,

Akshay

[John_Holtz]

Hi,

It looks like there are two problems.

• The springs need a small rotational stiffness in K4, K5, and K6 to prevent it from rotating (like a shaft in two bearing)
• There is something else going wrong; I think it is related to connecting the spring to the rigid connectors, but I am not sure why it is a problem. You may be able to change the rigid connectors to Interpolating type (I did not try that), or eliminate the rigid connector entirely and create the model like the figure below.

That is, connect the spring directly to the model. Either move the spring to the corner of the model, or do this to keep it at the current location:

1. replace the work point in contact with the surface of the model with a sketch point.
2. In In-CAD, add a Mesh Control.
3. Activate the Vertex Data selection box on the mesh control dialog, and click the 6 sketch points.
4. Remesh the model. This will create a node at each of the sketch points.
5. Define the springs from the sketch point on the model to the work point on the ground.

Of course, with a slab that weights 115000 lbf, you should use a spring with a higher stiffness than 11 lbf/in. Otherwise, you should make sure that your toes are not underneath the slab when you "let it go".

[Anonymous]

Hi John,

I have made the revisions you suggested and got the model to run, however it looks like from the animation the springs are not connected to the body. Before I have seen the springs move along with the body, does that mean the rigid connectors do not have any effect? I cannot run the model without the connectors as it will cause a singularity, And I am using the weird stiffness values, just to see the motion, which does look correct.

Thanks for the advice and I hope to hear from you soon,

Akshay Abraham

[John_Holtz]

Hi Akshay,

What I am seeing is that the rigid connectors are not moving with the model. Since the springs are attached to the rigid connectors, it looks as if the springs are not moving. Is this what you are seeing? (Sometimes the rigid connectors move with the model, and sometimes they do not. This is a known issue.)

The other problem that I am seeing is that some corners of the model displace upward. How can that happen when the gravity load is downward? It cannot happen (especially when you are trying to support 115000 lbf with 6 springs of 11 lbf/inch spring constant). In my opinion, these wrong results are an issue due to connecting the springs to the rigid connectors. I do not know why it happens. Maybe it is a numerical issue when the model includes something weak (the springs) and something stiff (the rigid connectors). I tried converting the rigid connectors to bar elements (using the parameter RIGIDELEMTYPE and KRIGIDELEM) but that did not work. I tried using the PSS solver, but that did not work.

I think these are the options:

• As you have already tried, connect the springs directly to the model and ignore the high stress that occurs at that point.
• A new option: Create beam elements in place of the rigid elements. Create a sketch with 4 lines in the "X" pattern to connect the corners of each split face to the corresponding workpoint. Define these 4 lines and the 4 edges of each split face on the solid as beam elements. Then you can connect the spring to the "centerpoint" of the beams, just like you are doing with the rigid connectors.
• A new option: Instead of using beam elements, create 6 solid parts that are a "pad" in contact with the split face on the model. These can be thin, and given properties to make them "rigid". Then connect the springs directly to these new pads (similar to what you tried before). When viewing the results, you can hide the pads to ignore the hot spots.

[John_Holtz]

Hi Akshay,

FORGET EVERYTHING THAT I WROTE!

It looks like the model was not remeshed after the surfaces were split. So although the rigid connectors were defined on the new surfaces, there were no nodes associated with those surfaces. Therefore, most of the connectors were not created in the actual analysis file, and the model was unstable.

Please remesh the model, and the analysis should run properly.

[Anonymous]

Hi John,

I generated the mesh again, but the issue still stands, the rigid connectors dont move with the body. Is there a certain way I should mesh the model, ie linear or continuous?

Thanks,

Akshay

[John_Holtz]

Hi. Rigid connectors and springs are just dumb glyphs (a graphical symbols) and are not related to what is included in the analysis. They are just like the force arrows. If you change the density of the display, you see more arrows, but that does not mean that there are more forces in the analysis. (In other words, force arrows, constraints, connectors, and so on are just symbols that are shown on the model. What gets translated to the NASTRAN file is what is important.)

Sometimes the rigid connectors move with the model, and sometimes they do not. This is a known issue. They probably should never move! Forces and constraints never move; they are always shown on the undeformed model, not on the deformed model.

If the motion of the connectors is the only "problem" that you are seeing and the results are correct, there is nothing to worry about. If the results (displacement, forces in the springs, etc.) are wrong, then please clarify specifically what result is wrong.

[Anonymous]

I see, its just that I had another model where the springs and connectors moved so I was confused why they werent doing it now. But the results are showing right differences.

Thank you for all the help John!