9050 Fatal error in simulation of lifting of a Jackup barge

[visheshsaxena]

I have modeled a Jackup barge with 32m tall legs for lifting it. I am running SOL 101. I am again and again getting 9050 error for some or other node. I have checked the model for any free element but there are none. I have run SOL 103 which shows some movement for legs otherwise its fine. I have attached the deck file. Please help ASAP.

 

[visheshsaxena]

I have modeled strings as GAP elements with closed stiffness as 1. Please check if this is correct to model a sling which becomes slack in compression. I am using GAP elements for first time so need guidance.

 

[Naffoussi]

you forgot to attach the file

Seif Eddine Naffoussi, Stress Engineer

http://www.Innovamech.com

33650 Martillac û France

 

[nlgyro]

Quoting:

> I am again and again getting 9050 error for some or other node

This has been covered many number of times on this forum. Check out the following thread, for example:

thread825-340948

 

[visheshsaxena]

Please find the attache file. Please have a look. I think its due to "closed stiffness=1" assigned in gap elements.

That link is no use to me as this problem is different. Have a look and then advise me.

http://files.engineering.com/getfil...c-3c69-4d23-a58d-f1282d81150d&file=Jackup.zip

 

[BlasMolero]

Hello!,
You need to mesh each string with only ONE CGAP element, not with hundered. And also you need to define the CGAP properties correctly: for compression-only gaps use a value of compression stiffness = 1e6 N/mm, run the same way for tension-only GAPs, enter a tension stiffness = 1e6 N/mm.

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/

 

[visheshsaxena]

GAP element properties has option for "Closed Stiffness" & "Open stiffness". WHat value should I put in them to model a compression only or tension only element.

Also, What will be the difference if I model ONE GAP element or hundred GAP element? Please elaborate.

 

[BlasMolero]

Hello!,
I told you before: if your GAP is working in tension-only, then enter a value for tension stiffness. But if your CGAP element is working in compression-only, then enter a value for compression-stiffness. I don't understand the physical problem you are running, then I can not give you more help.

Regarding meshing with one or more CGAPs elements, this is clear: the CGAP is a contact element, NOT A BEAM, don't have initial stiffness, the NX NASTRAN solver has to perform contact iterations to know if the gap is working in tension or compression, then depending the GAP properties the solver will close or open (no stiffness) the gap. If you mesh with more than ONE CGAP element, then you have a chain, and the problem will be singular, you have a MECHANISM!!.

To simplify things please consider to mesh the ropes using CROD elements, this way the stability of the model is more easily achived: play with length, cross section area and Young module to achive the stiffness desired (K = AE/L).

To understand to detect singularities take a look to this post:

http://www.iberisa.com/soporte/femap/excessive_pivot_ratios_nxnastran_error.htm

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/