Pressurized Inflatable structures - Frequency analysis 2

[AfonsoFerreira]

Hi everyone,

I hope that you can help me. I'm trying to do a simulation of a inflatable cylinder (100mm diameter and 500mm length).
I model the cilinder using shell elements (PSHELL). The wall has a thickness of 0.5mm and the material can be PVC or polyurethane.
My problem isn't in the modelation of the structure but the analysis. I want to do a frequency analysis to know the vibrations modes. In these analysis, I have two problems:
1º I can't especify a pressure inside the cylinder using the solver 103
2ºWhen I try to do a static analysis, it occurs always a fatal error saying that there is excessive pivot ratios in matrix kll. And I'm stuck in this step!

Can you help me?

I started to see some tutorials about a Restart analysis in NX simulation. But like I said I can't do the first part which is the static analysis without a fatal error.

https://www.youtube.com/watch?v=AYTx_jZbAcM

If you need any other information please ask :smileywink:
Thank you
Afonso Ferreira

 

[Tuw]

Hi AfonsoFerreira,

1. Yes you cant specify pressure load using Sol103, but Sol103-Response Simulation can be used instead with the aid of enforced motion location. After the first run using Sol103 RS, subsequent run is developed to perform frequency analysis based on the enforced location.

2. "excessive pivot ratios in matrix kll" means that either you did not constraint your model enough that too many possibilities where the model could displace, or maybe you did do a good job constraining it but there is a detached mesh unknowingly that does not connect to the host mesh. To solve this, you might want to re-check your constraint to make sure the model is constrained enough in all axis, or check your meshes for detached meshes, by checking the overall element's free edges, or co-incident nodes.

Good luck and regards,
Tuw

 

[AfonsoFerreira]

Hi,

Thank you for your answer.
I'm new using the Siemens NX, so I don't know many things about it. How can I use that enforced motion location?

I already check my mesh and experience another constrains and I can't solve any solution, it occurs always a fatal error. The only solution which I can obtain results is SOL 601 but with this SOL 601 I think i can't obtain vibration modes :/

Can you help me? If you need more information I can send to you the files.

Thank you,
Afonso Ferreira

 

[AfonsoFerreira]

Hi again,

I have been searching about the SOL 103 Response simulation, and I think if I can solve the static analysis it can solve my problem. But I have some questions that might you can help me.

When I chose the analysis Sol 103-Response simulation it appears 3 subcases (Dynamics, Static offset, Stress stiffness) which allows me to apply loads to the structure. These loads will be processed to calculate the vibration modes or it is two separate things? Moreover, if I apply loads in the 3 subcases he will process the 3 subcases or only one in the results? And finally, which is the best way to simulated a pressure in the cylinder and after calculate the vibration modes?

I can't understand how it works the enforced motion and how i will simulate a pressurized cylinder with it :/

Thank you,
Afonso Ferreira

 

[Tuw]

Hi AfonsoFerreira,

There are 3 subcases in a Sol103RS, the NX documentation did illustrate each of the subcase. I have tried to check the input file created when putting a load definition under each subcase, and I noticed that the main difference is the automatic keyword "STATSUB" that is input under Subcase "Stress Stiffening". In layman term, NX Sol103RS's user interface (UI) intelligently set the 3 subcases differently. Although there are 3 subcases, but you only need to use 1 of them which is appropriate/relevant. In my opinion, stress stiffness subcase might be your selection, because the pressure is applied to the structure before modes are evaluated.

You might want to read more about stress stiffening effect at link below...

http://www.eng-tips.com/viewthread.cfm?qid=62902

http://www.eng-tips.com/viewthread.cfm?qid=337439

From NX Documentation, Enforced motion location is just a location. You will need to define the actual excitation after you solve the solution.

About the fatal error, probably you can attached your model here for diagnosis...

Regards,
Tuw

 

[AfonsoFerreira]

Hi Tuw,

Thanks for the information it was very helpful. I already obtain some results with the SOL 103 Response Simulation. But I have some strange warnings.

Some of the links you gave to me in the last comment, they speak about SOL 106 and they refer to do a Restart analysis. I can't do this because the fatal errors in my simulations.

I just attached my models and simulations attempts. If you could look to them and discover what I'm doing wrong I will be much appreciated.

In the zip attached file I put two folders:
[ul]
[li]In the First Folder (InflatableCylinder) there is the model and my simulation attempts with only one material in the entire structure. This gave me a lot of errors in the simulations so I tried another approach which is the second folder.[/li]
[/ul]
[ul]
[li]In the second folder (InflatableCylinder2Materials) there is the same model but with 2 materials. The top and the base of the cylinder are in steel with 5mm thickness and the cylinder body are in PVC with 0.3mm [/li]
[/ul]

I hope you can help me to solve the static analysis.

Thank you,
Afonso Ferreira

 

[AfonsoFerreira]

Here goes the first folder.

Thanks

 

[AfonsoFerreira]

Here goes the second folder file

Thanks

 

[Tuw]

Hi AfonsoFerreira,

Please find attached file for your reference.

There is a bit tricky in applying constraint for a structure such as pressure vessel (your model seems like one). Some article suggested to used Sol106 with Large Displacement option.

Anyway, I have tried 2 methods to constraint it:
1. Involves splitting the structure model into its symmetry lines, and apply user defined constraints based on cylindrical coordinate system, some with cartesan coordinate system. This method involves more workflow but more systematic.

2. No need to define constraint. Check Inertia relief option in the solution. This option is located in the Edit solution dialog box.

I have compared the results obtained from both method and seems similar.

Regards,
Tuw

 

[AfonsoFerreira]

Hi Tuw,

Thanks for your answer and your work in my model. It helped me to understand some things in NX. I liked the way you split the model into its symmetry lines and how you applied the constrains. How did you do that? I think I don't have inertia relief option in SOL106

I don't understand the deformation that you obtain, in my opinion, the deformation should be uniform in the entire cylinder body in such a way that the cylinder will expand the same in all directions and not only in the top and the base. This is one of the reasons that I went to model my cylinder with two different materials like in the second folder which I attached before. I will attached an image of the deformation results that I obtained with the advanced nonlinear solution of this model to show to you how I think the cylinder should deform. Could you have a look in my second folder? And how I should obtain my vibration modes?

What do you think it's the best way to model my problem, using SOL106 with Restart Analysis or using SOL103Response Simulation with stress stiffness subcase?

Thank you very much for your help so far! It was splendid. Sorry for give so much trouble with this problem.

Regards,
Afonso

 

[Tuw]

Hi Afonso,

Why the deformation is not as your expectation is very much depending on what you have input. I have shown you the correct way to do the constraint based on the first folder, and you should try to do it on the second folder yourselves. Please do your homework to study the UI with the help of NX Help Documentation.
Until now, I dont understand what are you trying to achieve by doing a frequency analysis. You do not need to do a frequency analysis to find the vibration mode, a simple Sol103 will do.. Please elaborate more on your analysis objective.

Regards,
Tuw

 

[Tuw]

Hi Afonso,

I have just created a video about stress stiffening effect in Sol103. Actually we can apply loading condition in Sol103..

https://www.youtube.com/watch?v=OvJk0vTG_bk&feature=youtu.be

Regards,
Tuw

 

[AfonsoFerreira]

Hi Tuw,

Thank you very much for the help! The video is very good. I had some troubles last week so I couldn't work on this project. I will try to do my inflatable structure with your tips and help that you gave me before

I will after publish here my feedback and my questions

Thank you,
Afonso

 

[Tuw]

Hi Afonso Ferreira,

I have tested the 3 subcases in Sol103 Response Simulation.
1. Subcase - Static Offset
By inserting a load definition in it, with the given boundary condition, this subcase will return the equivalent result of a linear static solution. In simple word, this is to obtain a linear static result.

2. Subcase - Stress Stiffening
By inserting a load definition in it, this subcase will give the modes result (under subcase Dynamics) with the stress stiffening effect.

3. Subcase - Dynamics
By inserting a load definition in it, this subcase will give the modes result (obviously no stress stiffening effect unless the load definition is inserted in subcase 2), plus a "Distributed attachment mode". This distributed attachment mode is only useful for subsequent Response Simulation Analysis. For example, let's say I am interested to know what will happen if the load definition is excited (rather than stagnant/static) within a certain frequency range (for example from 20Hz to 200Hz). Response simulation is an add-on process to the existing Solution (Sol103 RS), that is capable to perform various type of response, such as transient, frequency, random, etc..

In general, if you are comparing Sol103 and Sol103 - RS, both will give you the same result because the keyword defined and the nastran solver is the same. The main difference between these 2 is that Sol103 - RS involves a further add-on process for further analysis, such as transient, frequency and random response analysis.

Regards,
Tuw

 

[AfonsoFerreira]

Hi Tuw,
During this week I have been working on this project. I couldn't view the NX help, I had a problem in the NX installation and I solved it. With the documentation of the NX, your comments and your videos I managed to have a solution (in response simulation) without fatal errors.
However my solution have some warnings which I can't solved them and I think it is influencing my results in a bad way.

I have 4 warnings of this type:
NASTRAN Msg: *** USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX KLL .
NASTRAN Msg: ^^^ USER WARNING MESSAGE 9136 (SEKRRS)
^^^ ENCOUNTERED EXCESSIVE PIVOT RATIOS IN MATRIX KLL.
NASTRAN Msg: *** USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX KYL .
NASTRAN Msg: *** USER WARNING MESSAGE 4698 (DCMPD)
STATISTICS FOR DECOMPOSITION OF MATRIX (NONE) .

I think this error is about the static response of the model which I couldn't managed to obtain a solution without errors. The solution which gives better results about the deformation is the SOl 601 Advance Nonlinear Simulation. But, with this I can't obtain the frequency modes :/.

In this Solution (advance nonlinear simulation) it occurs only one warning, which is:
NASTRAN Msg: ***WARNING: THE FOLLOWING LIST SHOWS UNSUPPORTED FIELDS FOR CERTAIN
BULK DATA
ENTRIES PROCESSED IN THIS INPUT FILE. YOUR MODEL MAY BE
AFFECTED


What I want to obtain is a relation between the pressure inside the cylinder and the frequency of the vibration modes. So, like you explain before, the right way to do it I think is using the Sol103 Response Simulation with the Subcase - Stress Stiffening.

I did some analysis with the response simulation and the stress stiffness. I varied the pressure inside the cylinder to be able to compare the frequency of the vibration modes. With higher pressure I obtain higher frequency in the vibration modes until I reach 0.5bar. After that the frequency modes start decreasing. I think it’s because of the warnings.
To check the results I did a Response simulation analysis with static offset. The results obtained was similar to the Sol 601 Advance Simulation. The static offset is irregular only in one point of the mesh (right in the middle of the cylinder) and doesn't make sense that deformation in that place.

How can I solve that warnings? What I'm doing wrong to have this 4 warnings?
I read that some materials in NX library aren't totally defined. Do you think it's because of that?

I attached the model and the analysis if you want to have a look.
Thank you,
Afonso

 

[Tuw]

Hello Afonso,

As for warning messages, usually we can ignore it, but not 'fatal' errors..
I have roughly checked your work files. The modes change is insignificant (for the first bending mode) as compared to each solution, when the pressure is varied. However, the modes begins to become different between each solution at mode no.5 (shown in figure below).

I just recall that you cannot use symmetry constraint representation in your case. A reason symmetry constraint cannot be applied for modal analysis (Sol103) is because some modes are not symmetrical, and setting those constraint will eliminate those important modes, thus you will be missing some of the results. For your case, I would suggest you model the neighboring components of the model that serves as the mounting component as well. For example, the vessel is bolt-jointed to a mounting bracket and the mounting bracket is fixed to the ground. Thus, you will need to mesh the mounting bracket, and fixed the bracket hole instead of the vessel directly. By doing this way, you would reduce the possibility of over-constraining your vessel.

As for your expectation that by increasing the pressure load within the vessel should increase the mode, while your results seems to show otherwise, currently I am unable to solve it. My guess is probably by incorporating geometric nonlinearity into an eigenvalue solution (Sol103) would give the desired outcome.

Below is what I found on how to perform a Modal analysis (Sol103) on nonlinear model from Sol106..
______________________________________________________________________________________________________
The following information in SOL 106 the NX Nastran Basic Nonlinear Analysis
User's Guide Ch 5.5(NX Nastran 4) or Ch 5.4(NX Nastran 5.1) states the
following:

5.4 Nonlinear Modal Analysis

You can request prestressed normal modes at the end of each subcase in SOL 106
by adding the following items to the input file.

Add METHOD=SIDin the subcase of interest. A prestressed normal mode analysis
will then be performed at the end of this subcase. The METHOD command points
to an EIGRL or EIGR Bulk Data entry which then selects an eigenvalue method.

For multiple normal mode analyses in SOL 106, the METHOD command may appear
in more than one subcase or above all subcases. In the latter case, a normal
mode analysis is performed at the end of each subcase. The stiffness used for
modal analysis corresponds to the last step of the subcase. Modal analysis
cannot be performed at intermediate solution step.

A PARAM,NMLOOP,loopid command must appear in the Case Control or Bulk Data
Section to request a normal mode analysis at the end of those subcases with a
METHOD command. The actual value of loopid is unimportant as long as it is a
positive integer. This alleviates the cumbersome task of figuring out the exact
loopid.

Add the appropriate EIGRL or EIGR entry in the Bulk Data Section of the NX
Nastran Quick Reference Guide.

____________________________________________________________________________________

Regards,
Tuw

 

[Tuw]

Hello Afonso,

Just realize you are using Quad8 elements, please change to Quad4 which would have better convergence.

Regards,
Tuw

 

[AfonsoFerreira]

Hi Tuw,

Thank you for your 2 last comments! They helped me a lot. Changing the element from Quad8 to Quad4 made the errors and the warnings in the Response simulation analysis disapear. And, like I thought, the frequency of the vibration modes increases with the pressure inside.

However I still have a strange deformation in the cylinder. The static offset is irregular only in one point of the mesh (right in the middle of the cylinder). This deformation doesn’t make sense :/ . Do you know why this happen? (I attached an image of the strange deformation).

In the advance nonlinear simulation the strange deformation is exactly the same and this error continues to appear:
NASTRAN Msg: ***WARNING: THE FOLLOWING LIST SHOWS UNSUPPORTED FIELDS FOR CERTAIN
BULK DATA
ENTRIES PROCESSED IN THIS INPUT FILE. YOUR MODEL MAY BE
AFFECTED

Do you have any idea how to solve this or why this happen?

Thank you,
Afonso

 

[Tuw]

Hi Afonso,

The unusual deformation is at the location of the Mesh Point.

If we look closer at the mesh point, noticed that the mesh point causes that mesh to sink, thus the mesh is relatively inaccurate.

In other words, the mesh created and the polygon bodies has a small difference. The mesh node might be slightly deviate from the geometry. I think this scenario would happen more in Quad8 elements condition. For Quad4 meshing, usually I didnt encounter such significant effect.

For your case, by removing the mesh point and using Quad4 elements might help.

Regards,
Tuw

 

[AfonsoFerreira]

Thank you Tuw.

It solve my problem. I can do my analysis now

Regards,
Afonso