Help with contacts on Nastran 8 (UG-8)

[ruedelapaix1]

Hello,

I'm trying to solve a problem of two clips, one static and the other moving.
I want to calculate how high/low each clips bends up/down.
the set is in here:

http://files.engineering.com/getfil...dc-47da-89ac-4b56840ae257&file=Sans_titre.png

How can I make the contact of the part supposed to bend possible and thus solve the set.
I tried to use the surface contact, but never worked kept on receiving errors messages.

Thank you

 

[BlasMolero]

Hello!,
Iunderstandd you run NX Advanced Simulation V8 + NX NASTRAN, ok?.
In order to be able to solve the linear contact problem using "surface-to-surface" contact (SOL101) remember you need to setup the model as 3-D, ie, you need to mesh with solid elements CETRA/CHEXA. In the picture you post I do not see if the model is 2-D or 3-D.

If the model is meshed with 2-D elements (the problem could be a typical case of PLANE STRESS, PLANE STRAIN or 2-D Axisymmetric body of revolution) then not possible to use the linear surface-to-surface contact capability, instead you will need to solve the problemnonlinearinar (SOL106) and use slide-line contact.

3-D Slide Line Contact Analysis
-------------------------------------

Slide line contact lets you model interactions between two deformable bodies. One of the deformable bodies is called the master and the other is called the slave. The modeling of interaction requires that you define contact regions in terms of slide lines. You may specify as many slide lines as you need.

A slide line contact region consists of a master line and a slave line. A master line is a list of grid points in the topological order on the master body. A slave line is a list of grid points in the topological order on the slave body. The grid points on the master line are called the master nodes, and on the slave line are called the slave nodes. A line segment joining two consecutive master nodes is called a master segment. Thus a master line, in general, consists of number of master segments. A minimum of one master segment consisting of two master nodes are required for the master line. Similar to master line, a slave line, in general, consist of a number of slave segments. However, a slave line may not have any slave segments; it may have just one slave node.

Tale a look to the NX NASTRAN HELP LIBRARY to learn more about sline line contact, or better solve the contact problem using solid elements, then you will be able to run a linear static (SOL101). But have in mind that liappliestact applyies to small displacements problems, if SLIDING exist then your linear static contact results will be meaningless ....

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[ruedelapaix1]

Hello Blas,

I'm using a 3-D model actualy, of 25.4mm in depth.
The probleme is that the option (Surface contact Mesh) seems to never work properly
How am I suppiosed to handle this to make a proper contact between the two part shown below

http://files.engineering.com/getfil...dc-47da-89ac-4b56840ae257&file=Sans_titre.png

The body is a 3-D
Thank you

 

[BlasMolero]

Hello!,
If the model is meshed with 3-D solid CTETRA elements, then the system is inestable, not possible at all to solve your model with the constraints you prescribed. Please note the part where the load is prescribed is fully unrestrained, then is free to move like a "rigid body", so you need to constraint your part properly defining any follower restraint in order to set running the "surface-to-surface", OK?.

Please note the surface-to-surface contat do not restriant the model, is simply a NO PENETRATION contact condition, then at initial of the solution not any contact stiffnes exist, causing solving errors (singular stiffness matrix issue!!), so you must take care of the boundary conditions of the model to avoit singulatities, OK?.

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[ruedelapaix1]

Hello,

I wonder how can I practicly solve my probleme, how can I make my part on which the force is acting correct.

Im new with Nastran and I'll be glad to try anything you'd suggest.

Thank you

 

[ruedelapaix1]

Hi Blas,

I finaly managed to solve the problem but the result I get I at the opposite of what I expected
I attached a screen capture of the results

The part that was supposed to bend up bends down and the one supposed to bend down finaly bends up.

I know It wont happen like this.

Do you have any idea what caused this to happen? a probleme in my contact surface parametres?

By the way I retrained the part 1 (the one on which the force is applied)as mounted on rollers. allowing movement on the axis that joins the two part

Your file's link is:

http://files.engineering.com/getfil...c-4e84-b655-dfbfabc94d0b&file=Sans_titre2.png

Thank you

 

[BlasMolero]

Dear Ruedelpais1,
Please remember this is linear static analysis where everything should follow the small displacement theory. Then check your displacement values, if not small then your analysis results aremeaninglesss, and you need to perform a nonlinear analysis activating large displacement effect. Also plot deformation using scale factor 1:1, usually the deformed shape isexaggeratedd, and gets confusing.

If linear static results are not valid, then you need to run the Advanced Nonlinear Analysis (SOL601), this is the only nonlinear solution with NX NASTRAN thsupportsrts surface-to-surface contact, where you can use "Displacement or Foce Controtechniquesues to arrive to a convergence solution, see image below:

Best regards,
Blas.

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

IBERISA
48011 BILBAO (SPAIN)
WEB:

http://www.iberisa.com

Blog de FEMAP & NX Nastran:

http://iberisa.wordpress.com/

 

[brailos]

Hello,

Did you use Surface Contact mesh from FEM with CGAP elements or did you use Surface to surface contact from Simulation? I recommend trying with Surface contact mesh and see what happens. Be careful you have to edit the Contact mesh and define the initial gap opening and the other required fields properly and set the direction of the contact.