Contact problem 1

[Alakin]

Hi I'm trying to do a very simple thermoelastic analysis,
there are two concentric rings of different material to whom I impose a costant nodal temperature. I put the two rings in contact but it doesn't seem to work perfectly. It looks like the contact is respected only on one half of the two rings as shown in the figure

The bdf is attached it's very little.
I'd be glad if someone could explain me what I did wrong

Thanks a lot and sorry for my english

 

[Alakin]

here 's the figure

 

[BlasMolero]

Dear Alakin,
The key here is to define correctly the bounday conditions is order to stabilize the FE model to solve using surface-to-surface contacts of "no penetration": if you study 1/4 of model and prescribe the corresponding symmetric boundary conditions then the linear static contact analysis will be performed with a few contact iterations, very fast. I have read your nastran input in FEMAP, re-defined BCs, prescribed the source & contact regions, define a CONTACT property with the following options:

And solved the model using NX NASTRAN and here you are th results, simply fast & reliable:

If you want to learn more in my web site & blog you have plenty of post & videos dealing with contact, linear & nonlinear.
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/

 

[Alakin]

So the problem was the BCs? beacuse when I ran the sol 101 analysis without the contact nastran solved it c

http://www.eng-tips.com/viewthread.cfm?qid=336068orrectly

(the two rings of course where overlapping but the structure didn't have mechanisms). I know that what you did was correct and smarter (analyze only 1/4 of the structure) but why couldn't it analyze the whole structure?
Thanks a lot for your help
I'll look into your blog and site it seems very well done

 

[BlasMolero]

Dear Alakin,
You can solve the FULL MODEL if you like, here you are the solution of thermal displacements using linear static analysis with FEMAP & NX NASTRAN (SOL101), you see that full or 1/8 model arrives to exactly th same result but at a cost 1/8 smaller, and in contact or nonlinear analysis this is VERY important. Please note you have symmetry in the three planes XY, YZ & ZX, then the "trick" is to prescribe the above boundary conditions in the full model. Sometimes for "marketing" reasons we are forced to solve the full model, no problem, you can do it, simply prescribe the BCs in the full model and you are done, 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/

 

[Alakin]

ok so it was the BCs, I thought that limiting the theta displacement in the cylindrical system leaving only the radial displacement was enough. In my view it should have forced the axysimmetry of the structure.
Thanks a lot for your help, you've been very helpful

 

[BlasMolero]

Dear Alakin,
Please note this is a true solid body of revolution model, ie, a 2-D Solid AXI-SYMMETRIC problem, then you can solve a simply 2-D axisymmetric model to account for 3-D solid displacements & stresses.

Beginning with FEMAP V11 and NX Nastran 8.5, solution 101 and consecutive solutions 103, 105, 111, and 112 supports edge-to-edge contact between the edges of axisymmetric, plane stress, and plane strain elements in the XZ or XY plane. Edge-to-edge contact is supported for the following elements:
• Axisymmetric elements CTRAX3, CQUADX4, CTRAX6, CQUADX8.
• Plane stress elements CPLSTS3, CPLSTS4, CPLSTS6, CPLSTS8.
• Plane strain elements CPLSTN3, CPLSTN4, CPLSTN6, CPLSTN8.

Then, here you have your model solved as 2-D solid axisymmetric with edge-to-edge contact, solution time is faster, and final results are exactly the same, not matter you solve your FULL model, 1/8 model or a simply 2-D axisymmetric slide, but at a fraction of cost -- impressing!!.

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/

 

[Walterke]

Please translate your website in English. It looks very informative

NX 7.5.5.4 with Teamcenter 8 on win7 64
Intel Xeon @3.2GHz
8GB RAM
Nvidia Quadro 2000

 

[sswatzell]

Blas...I'm running a somewhat similar problem and having issues...I've had decent results in the past using the linear surface contact and SOL 101...but this time I'm having trouble and I think it might be related to the fact that I have a small space between surfaces when the solution begins (see attachment)...I can seem to find any info as to whether this is an issue or not...Basically the solution seems to (for the most part) ignore the contact surfaces....So the the part just pass through one another...Any suggestions/comments would be great...thanks, scott

 

[BlasMolero]

Dear Scott,
Please note this is LINEAR contact, then the small displacements assumtion should be in effect. If you have a GAP, investigate the reason: this is due to manufacturing reasons, or assembly reasons, etc.. This is Finite Element, not CAD, the position of every body should be at the moment of working starting, if both parts should be in contact at the moment of working, then do not let the job of moving parts to the solver NX NASTRAN, the contact position should be your model, because this is LINEAR analysis (SOL101), where we support only very small displacements, if not this should be treated as NONLINEAR ANALYSIS (SOL601) taking in consideration large displacements effects apart of other nonlinearities like contact or material.

In summary, make both diameters to have the same value, and you are done. Or use OFFSET with one of the Contact regions, this is equivalent way, take a look to my blog here:

http://iberisa.wordpress.com/2012/0...-lineales-de-zunchado-con-femap-y-nx-nastran/

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/

 

[sswatzell]

Blas...thanks for all that info....very helpful...regarding the use of the offset...will that need to be declared on the slave and master or just the slave or just the master surface?

thx,
scott

 

[sswatzell]

also, is there anything specific (or special) that needs to be done to the connection properties?

 

[BlasMolero]

Dear Scott,
There are two contact region parameters which can be used in linear solutions, the SURF and OFFSET fields.
• SURF is used to define the contact side of shell element regions, not of interest in this case.
• OFFSET field allows to account for a rigid layer which might occur between two faces coming into contact. For example, a model which has two metal surfaces coming into contact, and one of these has a ceramic coating. If the ceramic material stiffness is not significant enough to be included in the analysis, it may not have been specifically modeled, but the thickness it adds to the face of the metal may be important when considering the contact problem.

You can also use the OFFSET field to analyze an interference fit problem if unconnected elements are modeled coincident. The offset value in this example can represent the theoretical interference of these faces.

Apply the OFFSET in the SOURCE region.

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/

 

[sswatzell]

Blas...are you aware of anything regarding mesh density between target and source?...I have been told by others that this is important when dealing with SOL 400 (MSC Nastran)...Just curious if you are aware of anything similar for NX SOL 101....

thx,
scott

 

[BlasMolero]

Dear Scott,
The best advice is "use the same mesh density for both SOURCE & TARGET contact regions", and you are done!.

In general, of the two contact regions you use for the pair, choose the one with the finer mesh for the source region. When the source and target regions have different mesh densities, more elements on the source region will mean that more contact elements are created, which will produce a more accurate solution.

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/

 

[sswatzell]

Blas...thanks for all the great info...One other question regarding the interference condition...So if I am analyzing for a pressfit condition, the 'offset' would be defined at the difference in diameters, correct?...Not the actual deformation between the two parts (per Shigley, etc.)...thanks again, scott