USER FATAL MESSAGE 9137 1

[kammieorama]

I am running a SOL101 analysis and here is an error which I am getting

GRID POINT ID DEGREE OF FREEDOM MATRIX/FACTOR DIAGONAL RATIO MATRIX DIAGONAL

30 R1 -1.83702E+09 2.69117E+09
30 R2 -6.46914E+08 7.67864E+09
21:11:06 100:02 1025.3G 101.0 5969.5 0.1 SEKRRS 143 DCMP END
^^^ USER FATAL [highlight #EF2929]MESSAGE 9137 (SEKRRS[/highlight])
^^^ RUN [highlight #EF2929]TERMINATED DUE TO EXCESSIVE PIVOT RATIOS IN MATRIX KLL[/highlight].
^^^ USER ACTION: CONSTRAIN MECHANISMS WITH SPCI OR SUPORTI ENTRIES OR SPECIFY PARAM,BAILOUT,-1 TO
^^^ CONTINUE THE RUN WITH MECHANISMS.

in the header file i have specified max ratio as
first with PARAM,MAXRATIO,1.0E+15
and then with PARAM,MAXRATIO,1.0E+25

but in both cases I did not get the same error.


kindly help....

best regards
kammieo

 

[BlasMolero]

Dear Kammieo,
Your stiffness matrix is singular because you have a rigid mody motion. Run a modal eigenvalue analysis (SOL103) and you will see the mechanism in your model. To learn more take a look to my blog in the following address:

http://iberisa.wordpress.com/2011/0...run-terminated-due-to-excessive-pivot-ratios/

Best regards,
Blas.



~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[kammieorama]

Dear Blas,

i have run the modal SOL103 analysis.

Is there anything specific that i should see in it?

In this model which i am simulating, I am also applying an force.
So , i wanted to see the stresses developed.

[highlight #FCE94F]is there a way that we can see stresses in result from a SOL103 analysis?[/highlight]

I had used [highlight #FCE94F]STRESS(PLOT)=ALL[/highlight] to get stresses in SOL103 run.
But when i tried viewing in a postprocessor(hyperview) it gave an error that results were not attached.


Kindly suggest what to do.

Best regards

 

[kammieorama]

Dear Blas,

Also kindly explain as to what you mean by "Your stiffness matrix is singular because [highlight blue]you have a rigid mody motion[/highlight]"

 

[BlasMolero]

Dear Kammieo,
If you run a modal eigenvalue analysis (SOL103) then you can animate the rigid body motions present in your model, i.e., modes with frequency zero (NX NASTRAN modal solver allows you to solve structures nor properly constrained), this way you will see where your model is not constrained properly, ie, where the mechanism exist, OK?. Animate MODE#1, you will see probably a component go to fly, the same to MODE#2, etc.. This type of analysis is a "trick" to debug finite element models to locate where the error in constraints exist.

Running a modal eigenvalue analysis (SOL103) do not provide stresses, not loadings are applied, this is simply eigenvalues and mode shape that will allow you to understand houw stiffness & mass is distributed in your FE mode. Please do not get confused with displacements results, these are meaningless, is simply a way to represent the model shape, displacements are normalized result, remember: not any loading exist!!.

The usual first step in performing a dynamic analysis is determining the natural frequencies and mode shapes of the structure with damping neglected. These results characterize the basic dynamic behavior of the structure and are an indication of how the structure will respond to dynamic loading. To obtain dynamic responses ans stresses an advanced dynamic analysis should be performed using NX NASTRAN, for instance, modal frequency dynamic response (SOL111) or modal transient dynamic response (SOL112).

For you to know, the natural frequencies of a structure are the frequencies at which the structure naturally tends to vibrate if it is subjected to a disturbance. For example, the strings of a piano are each tuned to vibrate at a specific frequency. Some alternate terms for the natural frequency are characteristic frequency, fundamental frequency, resonance frequency, and normal frequency.

Best regards,
Blas.


~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[kammieorama]

Dear Mr Blas,

Thank you for the response.

I checked your blog just now, but unfortunately the posts are in a different language.

however your reply here was very helpful.

My doubts are still not cleared.

I am simulating a crankshaft to which I want to propose some desigbn changes.
To simualte the rotating i have used RFORCE on it.
Now i expect some stresses to produced because of this rotation awhich will cause the centrifugal force due to connecting rod journals and the counterweights.

I also need the rigid body modes for MKS simulation in ADAMS.

Now is there a way that I can see both the stresses and modes in the same analysis or do i need to do two different analysis?

Thank you in advance..!!

best regards
Kammieo

 

[BlasMolero]

Dear Kammieo,
All the above explained is basic in FEA, in order to run FEM/FEA with success for engineering not any doubt should exist in basic things, then I suggest to contact with your FEA reseller to ask training.

If you want to run a linear static (SOL101) of a crankshaft, you need to make constraints asumptions in order to eliminate rigid body motions and make possible so solve equations by the FEA solver (this is not a problem of Nastran, the same error will happens not matter the solver used).

In the image below the movement in the horizontal plane -left image- is removed using a pinned constraint at the left end -right image-. In the case of working in 3-D (not in the plane) please note that still a rigid motion exist, rotation around the longitudinal axis of the beam, this degree of freedom (DOF) should be also removed in order to run with success a 3-D linear static analysis.

In the case of your crankshaft you need to identify the existing rigid body motions and proceed properly. Please note FEA do not solve mechanism (this is not Multibody Dynamic Analysis), we solve structures & assemblies of componets properly constrained.

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[kammieorama]

Dear Blas,

I would like to repeat if i understood clearly.

Kindly correct me if i am wrong.

1. Applying Rotating force (RFORCE) will not cause any change in the natural modes of the crankshaft.

2. When we run SOL103 no stresses will be calculated. (Since I will use the op2 generated for fatigue)
(which will consequentially mean that for fatigue analysis i will have to apply loads in FEMFAT)

3. To calculate stresses using SOL101 caused due to rotating force i should constrain by crankshaft.
(now since the rotating force is about X axis so it will work if i constraint only 4DOF )

Thank so much for sharing your knowledge and helping me..!!

Best Regards
Kammieo

 

[kammieorama]

Dear Blas,

If its not too much for you then can you please do me a favour.

Can you please suggest which SOL will be best for obtaining both the natural modes and stress values with a rotating force. I

I tried reading the NASTRAN manual but i was unable to decide the best one.

thanks a lot in advance

best regards
Kammieo

 

[BlasMolero]

Dear Kammieo,
To study seriously a rotating crankshaft you need to run rotor dynamics module, here you are a video explaining the process:

http://youtu.be/9HzgtTFrAac

FEMAP with NX Nastran includes a rotor dynamics capability that lets you predict the dynamic behavior of rotating systems. Rotating systems are subject to additional forces not present in non-rotating systems. These additional forces are a function of rotational speed and result in system modal frequencies that vary with the speed of rotation.

In a rotor dynamics analysis, the system‟s critical speed is particularly important. The critical speed corresponds to a rotation speed that is equal to the modal frequency. Because the critical speed is the speed at which the system can become unstable, engineers must be able to accurately predict those speeds as well as detect possible resonance problems in an analysis.

With frequency response analyses, the user can predict the steady-state response for different rotor speeds. Asynchronous analysis can be done by keeping the rotor speed constant and varying the excitation frequency. In the synchronous option, the excitation frequency is equal to, or a multiple of the rotor speed. Grid point displacement, velocity and acceleration, element forces and stresses can be recovered as function of rotor speed or excitation frequency.

In NX Nastran, you can perform rotor dynamics analyses on structures with one or more spinning rotors using either direct or modal solutions. You perform a rotor dynamics analysis in NX Nastran using solution sequence 107 or 110 (Complex eigenvalue analysis). To compute the response of a rotating system in frequency domain, solution sequence 108 or 111 (Frequency response analysis) can be used. For transient analysis in the time domain solution sequence 109 or 112 (Transient response analysis) can be used. For maneuver load analysis, solution sequence 101 (Linear static analysis) can be used.

The following picture shows a Sketch of FE model details at one of the support of a rotor:

Best regards,
Blas.

~~~~~~~~~~~~~~~~~~~~~~
Blas Molero Hidalgo
Ingeniero Industrial
Director

IBERISA
48004 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[kammieorama]

Dear Mr Blas,

Thank you very much for your help.

I was reading the NxNastran Manual.

I was unable to understand the difference between [highlight ]Direct Complex Eigen Values(SOL107)[/highlight], [highlight #E9B96E]Direct Frequency Response (SOL108[/highlight]), [highlight #8AE234]direct Transient Response(SOL109[/highlight]), [highlight #729FCF]Modal Complex Eigenvalues (SOL110[/highlight]), [highlight #F57900]Modal Frequency Response (SOL111)[/highlight] and [highlight #4E9A06]Modal Transient Response (SOL112).[/highlight].

From my understanding transient will give time depoendent response. but what is difference between direct and modal ? difference between complex and frequency?

Is there any literature that u have on this apart from the Nastran Manual which i did not find very helpful

Maybe i din know where to look for it in the manual.

Can u please provide some help on this.

best regards
Kammieo