How to constrain some nodes immovable in one direction(only negative)?

[alin09]

I analyze a structure which consist a beam on the ground. I would like to constrain the beam in that way that it can be movable in positive Z direction but immovable in negative Z direction. (Z is vertical to the ground) How do I do that?

From Patran displacment constraint, I can only make it zero.

Thanks for any input!

 

[GregLocock]

You need to use a non linear solver. What you are describing can be achieved with contact, or a very non linear spring.

Cheers

Greg Locock

I rarely exceed 1.79 x 10^12 furlongs per fortnight

 

[alin09]

Greg, thank you for the reply.

As you said, I need to create some nonlinear spring connected with nodes of beams and then use nonlinear analysis. I don't know if nonlinear solver will generate some error.

 

[ThomasH]

Hi

If you use Patran I guess you use Nastran. Then you can get the effect you want from a gap element and, of course, a nonlinear solution.

Good Luck

Thomas

 

[Onda]

You can use linear gap elements. refer to this post

http://www.eng-tips.com/viewthread.cfm?qid=260080&page=1

Onda

 

[GregLocock]

This might help

http://www.nastran.jp/ne_pdf/01_TUTAddingGapElementsModel.pdf

Cheers

Greg Locock

I rarely exceed 1.79 x 10^12 furlongs per fortnight

 

[alin09]

Thomas,Onda, and Greg,
Thank you very much! These are helpful, and I'll try it later.

 

[trainguy]

Alin09,

I have, in the past, done this kind of analysis for a beam on an elastic foundation using springs at various nodes, then checking where the spring reactions were tensile, then removing them and iterating until all the assumed spring supports are in compression.

Of course, at that time, I did not have access to NL solvers and gap elements.

tg

 

[alin09]

Thanks, trainguy,
I can try spring element later. I might give large stiffness to the springs to simulate ground support effect.

Anyone use 1D linear gap element before?
I can create CGAP PROPERTY of Patran 2008. But I am not sure how to apply CGAP property in the model. It sounds like I can only apply this property to elements or curves. Thus, I can either
1. Apply this property to curves;
2. Create 1D elements to connect nodes at the gap, and apply this property to the elements;
I could not find examples of CGAP in NASTRAN manual and two linear contact problems in the manual use MPC, SPOINT conditions.

Another question is
How to restrain 3D solid for FE analysis? Since 3D elements don’t have rotational DOF, I need to fix three rotational DOF of all the nodes? There is singularity of DOF 456 shown in f06 output file.

 

[Onda]

You can look @ this thread for example to how to apply Linear gap.

http://www.eng-tips.com/viewthread.cfm?qid=243224&page=1

Pay attention that CGap and Linear Gap are two different things.
To use CGap you shoud run a non linear analysis.
To use linear gap you should re-iterate a linear analysis. parameter CDITER.
Linear gap should be done using the Patran utility :
Utilities->Applications->Linear Gaps.
The only way to do linear gaps is between two grid points. The grid points could be coincident or not coincident.

Linear gaps haven't any property they are just open or close.
If they are open no load could pass through the linear gap. If they are close full load pass through them.

To constrain grid points of a 3D model you could use AUTOSPC, YES or much better constrain the grid points with a SPC1 Card.
You could make a first run and ask for AUTOSPC (PUNCH),YES in case control section.
the open the file *.pch and you will find all the cards you need to constrain the grid points of your model.
You could just rename the *.pch to *_xxx.bdf and include the file with an INCLUDE '*_xxx.bdf' statement.
Just add in the main bdf the SPCADD statement with the code needed.
Onda

 

[alin09]

Onda,

Thank you for the helpful post.
In order to test 3D modeling, I tried an example of a simple 3D cantilever beam. The picture is attached, and the beam is fixed at one end and forces are applied on the top surface. (My Patran has problem of generating jpg file and I can get bmp file, not sure why). Element type Hex8 is used.

I run this file and NASTRAN shows that there are singularity of DOF456 of many nodes. I tried AUTOSPC, YES and it is still the same. I didn't use PATRAN/NASTRAN to model 3D before. For other software I used before, I don't need to apply the constraint of rotational DOF. Is there anything wrong with this 3D modeling?

 

[BlasMolero]

Dear Alin09,
With current version of NX Nastran 7.0 you can achieve the desired behavior using a node-to-node CGAP compression-only element "linear contact constraint", and no need to run a nonlinear analysis, simply linear static SESTATIC (SOL 101) analysis is OK. The basic properties you must enter to define the CGAP element in the preprocessor are compression stiffness, gap allowable displacement (if zero or bigger than zero, then compression-only gap), gap friction, and gap orientation (also you can enter shear stiffness, and traction stiffness).

In order to activate the contact algorithm you will have to add BCSET=1 in the case control section, then the solver will iterate to get a contact converged solution. I have just solved a simply GAP problem and the output is similar to the following (solution monitor will also show the XY Plot of contact convergence progress):

^^^
^^^BEGIN CONTACT ITERATIONS FOR SUBCASE NUMBER 1
^^^
^^^
^^^CONTACT ITERATION NUMBER 1
^^^
^^^NUMBER OF INACTIVE CONTACTS: 0
^^^NUMBER OF ACTIVE OPEN CONTACTS: 2
^^^NUMBER OF STICKING CONTACTS: 0
^^^NUMBER OF SLIDING CONTACTS: 0
^^^BEGIN CONTACT FORCE ITERATION
^^^
^^^
^^^CONTACT ITERATION NUMBER 2
^^^
^^^NUMBER OF CONTACT STATUS CHANGES: 2 (NCHG: 0)
^^^NUMBER OF INACTIVE CONTACTS: 1
^^^NUMBER OF STICKING CONTACTS: 0
^^^NUMBER OF SLIDING CONTACTS: 1
^^^BEGIN CONTACT FORCE ITERATION
^^^CONTACT FORCE CONVERGENCE RATIO: 2.464475E-09 (CTOL: 0.000000E+00)
^^^
^^^
^^^FINAL CONTACT STATUS AT CONVERGENCE
^^^
^^^NUMBER OF CONTACT STATUS CHANGES: 0 (NCHG: 0)
^^^NUMBER OF INACTIVE CONTACTS: 1
^^^NUMBER OF STICKING CONTACTS: 0
^^^NUMBER OF SLIDING CONTACTS: 1
^^^
^^^CONTACT ITERATION CONVERGED
^^^
Best regards,
Blas.

 

[GregLocock]

So how do you do a modal analysis on a 'linear' model that has "linear contact constraints"?

Cheers

Greg Locock

I rarely exceed 1.79 x 10^12 furlongs per fortnight

 

[BlasMolero]

Dear Greg,
This is a very powerful feature found in NX NASTRAN since Release 5.0, it is perfectly possible to perform "linear contact in a normal mode solution (SOL 103)" including the contact stiffness from a converged line-to-line or surface to surface contact solution. With this feature you can perform a normal modes analysis on an assembly of parts connected, for example, via pre-loaded bolted joints and considering contacts between components.

I will show you how it runs: in the normal mode solution SEMODES (SOL 103), NX Nastran adds the differential stiffness calculated from the bolt preload analysis of a linear statics SESTATIC (SOL 101) of the assembly, plus the contact stiffness resulting from the converged linear static contact solution to the structural stiffness.

The contact stiffness values in the normal mode solution represent the final contact condition of the structure around the contact interface. Thus, it will appear that the resulting contact surfaces are attached during the normal mode analysis.

The inputs for the normal mode solution are consistent with differential stiffness solutions which require a linear static subcase. The difference is that the linear static subcase should include the BCSET case control command. When defining the normal modes subcase, a STATSUB bulk entry must be included to reference the subcase id containing the contact definition. The contact solution in the linear static subcase must fully converge before moving to the normal mode portion of the run.

Note that since the calculated normal modes include the final contact interface conditions, the modal transient response solutions (SOLs 111 and 112) which use these normal modes automatically include the same conditions.

This is a great feature to consider contacts pre-loaded modes in dynamic analysis. When time allowed I will write an example to show you step-by-step how to perform the analysis with a simply assembly.
Best regards,
Blas.

 

[johnhors]

The contact solution in the linear static subcase must fully converge....

There appears to be some misunderstanding of the use of the term "linear".

My understanding is that a static linear analysis involves just a single pass through the solver to solve for X in F=K.X

For a solution to "fully converge" it must be iterating, thus making multiple passes through the solver with a changed problem definition each time. This is a "non-linear" analysis!

http://www.Roshaz.com

 

[BlasMolero]

Not at all, this is linear contact analysis, the solver iterates till contact convergence achieved, this is a feature (linear contact analysis using CGAP node-to-node and modern surface-to-surface contact) that you have in many FEA packages of today times, not only in NX Nastran. In fact, the quality of the solution should be take with care: this is linear static analysis, then whe should remain in the field of small displacements and small strains, if you have large displacements, intermitent contacts, situations where the structure buckle or experience stress stiffening effects, etc.. this is nonlinear analysis, and then you must solve the problem using the nonlinear modules available in you FEA code.
You can perform a linear static analysis and arrive to a solution, yes, but the accuracy of results is nothing compared with real life, not sense at all.

The initial question was how to define "constraints" on Z-only", the answer is using CGAP compression-only node-to-node contact elements (or surface-to-surface, the procedure is the same), and if the problem is linear & static it can be solved using SESTATIC (SOL101) with FEMAP & NX NASTRAN.

Please note FEA is a tool in the hands of the engineer, is the engineer who has the control of the tool, and it should be used correctly.

Best regards,
Blas.

 

[johnhors]

You could solve this in Abaqus but NOT as what Abaqus calls with a "Linear Perturbation" analysis.

You could solve it in Lusas under what they term "Non-Linear Control".

Neither of these, or other solvers I know of would term this a linear analysis.

In a static linear analysis the results (displacements, nodal forces and stresses) are directly proportional to the applied loads (including load reversals) with the load path and stress flow directions remaining constant.

In a contact analysis this relationship no longer holds true, where the level of loading can determine the amount of contact, which then subsequently determines the loading path (imagine the extreme case with the loading reversed! pin in a lug for example)

http://www.Roshaz.com

 

[BlasMolero]

Dear Johnhors,
This is a nastran forum, if in other FEA codes this feature is not possible I am very sorry.
Best regards,
Blas.

 

[BlasMolero]

Oh!, sorry, we are in the "general engineering programs" discussion forum. In any case, I remember doing exactly the same say more than 15 years ago using old COSMOS/M GEOSTAR code, if COSMOS/M or NX NASTRAN can solve a linear static analysis with GAP elements, I am sure Abaqus will be the same.
Best regards,
Blas.

 

[johnhors]

The “linear gap” technology introduced in. MSC/NASTRAN V70.5 linear static solution (SOL 101)

http://www.mscsoftware.com/support/library/conf/auc99/p05799.pdf

Linear gaps are implemented in SOL 101 by using explicit Multi-Point Constraints (MPCs) to define the gaps. Because MPCs are used, there is no gap stiffness; adjacent grids are either “welded” or ‘free” in the user specified degrees of freedom. The linear gaps provide for contact, or compressive, forces only. Because of the implementation, friction is not available, but a large class of problems can be solved efficiently. The MPCs are satisfied by an iterative technique that is built into SOL 101. The solution converges when there is no penetration of MPCs (i.e. gap deflection >=0.0) and there are no tensile forces.


Despite what MSC say an "iterative technique" is not a linear solution!

http://www.Roshaz.com