Nastran Output File Not Updating

[jthomas2SNH8G]

I'm running a random response analysis to analyze a sign post for its back and forth oscillation. I have everything modeled as shells. The analysis consists of around 91,873 nodes 29224 elements. 

I have rigid connector connecting the two vertical members to a point placed at the CG location and I am applying an enforced motion type load to the CG point, with PSD provided. 

The problem I am facing is, once I begin the simulation the Nastran Output stops at this line and I notice the files don't get updated or size doesn't increase. Waited for more than an hour but there wasn't any update.

What might be the issue?

@John_Holtz 

 

 

 

[jthomas2SNH8G]

@John_Holtz 

I've come across a documentation on enforced motion load type that says -

"In a frequency response or random response analysis, the number of modes (natural frequencies) calculated is based on the number of nodes with an enforced motion. The number of modes is not limited to the "Number of Modes" specified on the Modal Setup. (In addition to the time required to calculate the natural frequencies, any calculation that is based on the number of natural frequencies is affected.)"

The fact that the node at which I am applying my enforced motion is connected to a lot of nodes on either side,

Could this be the reason my analysis is super slow and it is not updating anything on the Nastran Output window and even the analysis files? If so, what can I do to work around this drawback and speed things up?

Showing image of the connector with increased visual density for clarity.

[jthomas2SNH8G]

@John_Holtz 

Why is it that it looks at the number of nodes associated with the enforced motion and calculate that number of modes? Is there a way to overrun that and restrict the number of modes (natural frequencies) calculated? 

[John_Holtz]

Hi @jthomas2SNH8G 

You have an enforced motion applied to 1 node: the center point of the rigid body. That is not the issue in your analysis.

I do not know what the issue is. Does the Windows Task Manager show (on the Details tab) that nastran.exe is still running and using CPU?

• If Yes, the analysis is still running. Letting it run is the only suggestion I have.
• If No, the analysis crashed and forgot to tell you that it had stopped.

I do not understand the rigid connectors and how the vibration of the columns is resisted by the fixed base plate.

1. Are the rigid connectors attached to 4 edges around the columns, so something that vibrates is mounted on the columns at 4 locations. Or are the rigid connectors attached to the entire face of the columns?
2. How are the columns attached to the base plate? (I assume with the offset bonded contact).
3. Regardless, how can the bottom of the columns be vibrated with the PSD while simultaneously held fixed by the base plate? That will create a lot of stress.

John

[jthomas2SNH8G]

@John_Holtz 

Yes I do see the Nastran.exe running in the Task Manager. 

I alternately tried running the analysis by having the enforce motion point connected to the sign itself, thinking it might help having relatively lesser nodes connected to the rigid connector and it ran successfully.

To answer your questions on the setup -

1. The rigid connectors are attached to the entire face as if the two columns are connected to something in the middle that is vibrating back and forth.

2. Yes the base and the columns are offset bonded contact.

3. Yes I agree and I am in the pursuit of finding that stress value.

What might be the issue then? Too many calculations required for the Eigen Values?

[jthomas2SNH8G]

@John_Holtz 

Another question related to this -

In my analysis I'm trying to simulate the back and forth vibration of the sign post.

When we give in the acceleration in the enforced motion load and provide value in  9.81m/s2,

what is the influence of + or - sign in the input? 

In the load factor table I provided (0,1) and (1,1).

[John_Holtz]

Hi @jthomas2SNH8G 

Somehow I missed in the original post, in the first sentence, that you are analyzing a sign post. Now I understand the model!

But whether you have one enforced motion applied to the sign or one enforced motion applied to the posts, it is still just 1 enforced motion. One enforced motion is not forcing the analysis to solve many extra frequencies. Surely applying the rigid connector to the posts (and making the posts rigid) is not the correct approach, especially since it is the posts that you are trying to design. I think this is how it should be setup:

1. Apply the rigid connector to the sign. Uncheck all degrees of freedom (DOF) on the rigid body except for the direction of the PSD.
2. Apply the enforced motion and constraint to the center point of the connector. Only restrain the direction in the direction of the PSD. (You want all other directions free so that the model is as free as possible to vibrate in other directions.)
3. It does not matter whether the acceleration is in the + direction or - direction. The analysis moves the model equally in both directions (during the frequency response portion of the analysis), and since the analysis is linear, the stress results are equal (and opposition in sign) regardless of whether the + direction or - direction gets "chosen" by the analysis.

John

[jthomas2SNH8G]

@John_Holtz 

Yes sir. I see your point of applying the rigid connectors to the post being the wrong approach.

I've changed that approach and applying to the sign itself.

So let me explain how I have it set up right now, I've numbered each component for the ease of our conversation -

Item #3 is fixed and constrained in all directions.

Item #1 and Item #2 are held to Item #3 by "Offset Bonded" contact.

Item #4 is held to Item #1 and Item #2 by "Offset Bonded" contact.

Item #5 is a external point and the Rigid Connector seen is associating all nodes of Item #4 to this point Item #5.

Enforced Motion is set on the Item #5 (point), with sub-type of "acceleration" and a value of +9.81m/s2. 

The load factor table for the Enforced Motion is (0,1)(1,1).

Questions on your suggested procedure -

1. Apply the rigid connector to the sign. Uncheck all degrees of freedom (DOF) on the rigid body except for the direction of the PSD. 
2. Apply the enforced motion and constraint to the center point of the connector. Only restrain the direction in the direction of the PSD. (You want all other directions free so that the model is as free as possible to vibrate in other directions.)

In your step 1 and step 2, the discussion of restraining the DOF are both the same and referring to the center point of the rigid connector? Also why are we locking in the direction of the PSD, won't that contradict the direction of force input we are giving the model?

As I was typing this reply the simulation I ran with my above described setup finished running and I'm attaching the result image below. It is showing really high stress value of 1070804672MPa and the contact seems to be messed up. What am I missing?

 

[John_Holtz]

In my step 1, the DOF on the rigid body connectors are related to the forces transmitted to the plate (the face where the connector is attached). The DOF are not related to the node at the center of the rigid connector. By setting the DOF to Tz only, the plate will behave like a rigid plate in Z translation only. It is not rigid in X or Y translation, so it is not quite as rigid and before.

In step 2, you are assuming the enforced motion moves the model or rigid body connector. It does not! The enforced motion moves the constraint, and the constraint moves the model. If there is no constraint at the same geometry as the enforced motion (in your case, at the center of the rigid body), then there is a 50-50 chance that the enforced motion will work.

Now that I think of it, I am not sure what the rigid body connectors will do if the plate end only transmits Z direction forces and if the center node is only constrained in Tz. Will the rigid connectors be unstable? If that happens, you can fully fixed the constraint at the center node to prevent the rigid body from "flying around". Since the DOF of the rigid body is Tz only, only reaction forces in the Z direction will be transmitted to the plate, so the "fixed constraint" does nothing to the analysis (other than provide stability, if needed).

John

[jthomas2SNH8G]

@John_Holtz 

OK. I understand what you mean by your first point and I applied that in my setup, by setting the DOF of the rigid connector to be Tz (direction of my PSD). I unchecked the rest of the DOFs.

I'm confused by the "constraint" you are referring to in your second point. Especially when you say "If there is no constraint at the same geometry as the enforced motion (in your case, at the center of the rigid body)"- Are you saying I must create a constraint for that center point of my rigid connectors and constrain the PSD direction i.e. Tz? (Tz is the back and forth direction, the mode I am analysis via. my PSD input)

In my head I'm thinking if I constrain that node in the direction of my PSD Input how will it transmit the input force to the sign? Doesn't it have to move to work?

Just to show you more clearly how my rigid connector is modeled, the center point of the rigid connectors is outside the sign itself, a point I modeled in.

 

Assuming that in your second point you mean I must create a constraint for the center point of my rigid connector and must constrain the PSD direction (Tz), I ran the analysis but it looks like nothing is happening and so I get zero stress i.e. I restrained the DOF of the rigid connectors and the constrained the center point of the rigid connector, but seem to be doing something wrong. Can you elaborate a little bit about how enhanced motion works? 

 

[John_Holtz]

Can you attach your model? Compress the assembly file(s) (.iam) and part file(s) (.ipt) at attach the .zip/.rar/.7z file to the forum post. There are enough strange things going on (long time to run, sign bonded to posts but not staying bonded, enforced motion not working) that we need to have the actual model to help.

Also, indicate which version of Inventor Nastran you are using. That way, other readers will know if they can open the model or not.

John

[jthomas2SNH8G]

@John_Holtz 

I've attached the files.

I am using Inventor 2020.

[John_Holtz]

Hi @jthomas2SNH8G 

Perhaps there are other highway engineers reading this post that can provide some insight to the design process.

Here are a few things that I see:

1. The range of the PSD is 7.967 to 12.91 Hz. All you know is what the vibration load is when the model vibrates between 7.967 and 12.91 Hz. The lowest natural frequency of the model is 98 Hz. Since this is much higher than the PSD, vibration should not be a problem. You do not need to run an analysis.
2. Even if you do decide to run an analysis, you should ask yourself what load value is used from the PSD (the input table) when the exciting frequency is outside the range of the PSD? For example, what value of PSD is used for an excitation frequency of 1 Hz? 23.39653 Hz? You should extend the PSD to use values that you want to use. I suspect the analysis extrapolates the PSD which means that at a forcing frequency of 500 Hz, you may be getting garbage. (I have to think about this: what is extrapolation in a log-log plot. Maybe it just approaches 0 the further you get from 8 and 12.9 Hz. Regardless of that answer, is it giving the value that you want?)
3. You should not include gravity in the analysis. Gravity is not multiplied by the PSD in real life, but all loads are multiplied by the PSD in the analysis.

Even with the above changes, the results are outrageously high. Are you sure the provided PSD is in g^2/Hz measured at the sign?

John

[jthomas2SNH8G]

@John_Holtz 

The actual case I am analyzing is not a sign post but a mast on a vehicle. I can't share the actual images of what I'm working on due to proprietary reasons I'm sure you understand. But I've been using that model I shared with you for our discussion and trying out figure out how stuff plays out on there before I try it on my actual model as it is relatively a big file and takes almost an hour and half to finish run.

To answer your question about the PSD Data, Let me give you a better picture of what I'm doing without making anyone mad - 

So what we did was place an accelerometer on top of a Mast that is part of a fork-lift type vehicle. We got the time history data and did an FFT and produced the PSD curves. (Attached one test run's plot below)

From the PSD Curve I took the distinct top 4 data peaks and decided to use that as input I understand by your point about the PSD extrapolation. Are you suggesting I put the whole data points I have regarding the PSD into the Inventor File? Won't that delay the analysis time?

Now what I'm trying to do in my simulation is to understand what is the Max. Stress I would see on the Mast and eventually would like to run a vibration fatigue analysis to get a life cycle estimation.

 

[jthomas2SNH8G]

@John_Holtz Any ideas sir? 

[jthomas2SNH8G]

@John_Holtz  Any thoughts?

[John_Holtz]

I think we need someone familiar with testing equipment and applying the PSD in a model. Unfortunately, I do not have any experience in this regards.

Here are some thoughts that come to mind:

1. Since you were measuring the acceleration, is the PSD in g^2/Hz, or is it in (m/s^2)^2/Hz or some other unit? If the PSD is in (m/s^2)^2/Hz, then the applied load should be 1 m/s^2 acceleration. If the PSD is in g^2/Hz, then the load of 9.81 m/s^2 (= 1 G) is correct.
2. Although the acceleration is measured at the top and it makes sense to apply the load at the top, I wonder if the load should be applied at the base since that is the source of the vibration. It may need to be scaled up or down so that the calculated acceleration at the top equals the measured valued.
3. Or perhaps the load should be applied to a small area of the sign so that the stiffness of rigid connector does not have an adverse effect on the stiffness of the structure. (I was trying to minimize that by only setting the Tz on the rigid body connector. Of course, the Z direction is the most important direction!)

John

[jthomas2SNH8G]

@John_Holtz 

What confuses me is -  where this extra stiffness is being induced that is causing these enormous stress values.

In my case I select all the nodes of the top surface on which the accelerometer was placed. Using a RBE2 connector I constraint all those top nodes to a single independent node. Selecting the Tz  (my PSD Data) direction to be the one controlled by the Rigid Connector. And I constraint that Rigid Connector's Central Node in the Tz direction.

Still end up getting very high stress values.

Secondly, for sure it would be very useful if we could understand how the PSD curve is extrapolated for the points not provided by the user? To just check if the multiplication factor is what is causing the stress results to be this amplified and ultimately not sensible. Is there some kind of Autodesk developer or someone from their team who could guide us on what the software is doing for the region of the PSD not provided by the User?

I would really like to figure this out to get a closure to this effort of understanding the Frequency Response and Random Response Analysis in Nastran.