Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in

Contact in frequency response analysis 2

Status
Not open for further replies.
isponmo

isponmo

Aerospace
Jul 20, 2012
39
0
0
NL
Dear All,

I have a FE model in which two of the parts touch each other but do not remain in contact all the time. The aim of the model is to estimate the stresses caused by an event defined in the frequency domain.

As a first step, I did a normal modes analysis ignoring the contact between the parts (there is an alternative loadpath via screws, which is the critical path). However, after checking some modal survey test results, it turned out that the modes were quite different to the predicted ones, so I performed several changes to improve the model. At the end, it turned out that considering a permanent contact between the two parts improved the results.

Now, the problem is that if I consider permanent contact, I am creating an additional loadpath and part of the stresses are diverted from the main loadpath (screws). Consequently, I have the feeling that such approach is not conservative from the strength point of view and I have the following dilemma:

a) Using the permanent contact -> Risk of underestimating the stresses in the main loadpath.
b) Ignoring the contact -> Excitement of nonexistent modes during the frequency response simulation, which can also lead to erroneous results.

How could I deal with this? What is the best approach for parts that touch each other in frequency response analysis and normal modes analysis?

Thank you very much.

Best regards,

I. Pons
 
Replies continue below

Recommended for you

Sort by date Sort by votes
Dear GregLocock and spongebob007,

Thank you for your answers.

I agree tata using non-linear transient analysis is the most accurate approach, but sometimes it seems impractical. For example, for a random vibration analysis it is not possible (as far as I know) to convert the load, described in the frequency domain as ASD vs freq. to an equivalent transient load. In addition, some times the size of the model is too large to carry out non-linear transient of many cases.

How should we proceed in such cases? And what are "realistic loads" equivalent to contacts when contacts and non-linear solutions cannot be used?

Best regards and thanks again!
 
Upvote 0 Downvote
You can synthesize loads from an asd back to a time history. I personally wouldn't trust the result. If your excitation spectrum is supposed to represent random noise then it should work, but real operating loads usually have some harmonic structure with some non random phase structure.

So you either get a time history of the loads, or you take a punt.



Cheers

Greg Locock


New here? Try reading these, they might help FAQ731-376
 
Upvote 0 Downvote
Dear GregLocock,

Thank you very much for your fast answer! :)

Do you know a good source where I could find further information about synthesizing ASD back to time applied to FEM? Is this process a common practice? Why wouldn't you trust the results?

I imagine that if we convert a ASD load into time domain, we will get a set of sines combined in a particular manner (with a particular phase for each one), and that the load will not be totally random. If all sines were in phase, the response would be much higher than if they are not in phase. How can we make sure that such load is statistically representative? Assuming a gaussian distribution, could that synthesized signal be considered as a 1-sigma? How could we then define a 3-sigma case?

Best regards.
 
Upvote 0 Downvote
Dear I. Pons,
NX Nastran provides a contact capability for SOL 101 linear static analysis, and also in consecutive dynamic solutions 103, 105, 111 and 112.
In fact, a contact condition can be included in a normal mode solution (SOL 103), and in an optional dynamic response calculation (SOLs 111 and 112). In the normal mode solution, contact stiffness result is added from the end of the converged linear statics contact solution. The contact stiffness values in the normal mode solution represents the final contact condition of the structure around the contact interface. Thus, it will appear that the resulting contact edges or surfaces are attached during the normal mode analysis. Since the calculated normal modes include the final contact interface conditions, the response calculation (SOLs 111 and 112) which use these normal modes automatically include the same conditions.

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

Take a look to my blog where I explain how to use it:

mode1_contacto_sf2sf.gif


Best regards,
Blas.


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

IBERISA
48004 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Dear Blas,

Thank you for your reply.

If I understood it correctly, what the software does is defining open and close contacts during the static analysis, and applying the resulting contact states to the subsequent analyses. Consequently, the contacts that are closed, remain like that during the following analyses, and the ones that are open, never close.

If that is the case, it does not solve my problem: In my problem, different parts in contact are expected to separate and touch during the vibration, so the contacts do not keep their open/close condition.

Cheers,

Israel
 
Upvote 0 Downvote
Dear Israel,
With FEMAP & NX Nastran Modal Frequency Response (SOL111) Dynamic Analysis is based in the calculated normal modes computed previously using the contact interface condition, mode by mode, then the response calculation (SOL111 and SOL112) which use these normal modes automatically include the same conditions. This is only valid for modal methods, not for direct ones (SOL108 and SOL109).
Best regards,
Blas.

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

IBERISA
48004 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Dear Blas,

Thank you very much again.

How is the contact condition defined mode by mode? How does the software define which interfaces are to stay open and which ones are to stay close?

And still, even if for each mode the contact conditions are defined independently, I don't see how does that solve the problem: for a particular frequency in the spectrum, the contacts cannot open and close, they have to stay either open or close.
 
Upvote 0 Downvote
Dear Israel,
When contact conditions are included in a modal solution, the NX NASTRAN solver will search and detect when element faces come into contact. The software then creates contact elements, thus preventing the faces from penetrating and allowing finite sliding with optional friction effects.
Best regards,
Blas.

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

IBERISA
48004 BILBAO (SPAIN)
WEB: Blog de FEMAP & NX Nastran:
 
Upvote 0 Downvote
Dear Blas,

I am not able to totally understand:

The sliding condition with friction is kept during the frequency response analysis? Or are the contacts frozen as I suspect? And can separation happen once the parts have been in contact, for the same frequency in a frequency response analysis?

Cheers,

Israel
 
Upvote 0 Downvote
Blas,

Yes, NX Nastran does have the capability to augment structural stiffness with contact stiffness for a normal modes analysis. However, this is not done on a mode-by-mode basis and is not appropriate for the type of model/analysis that the Isponmo is describing ("two of the parts touch each other but do not remain in contact all the time").

The NX Nastran process is to solve a linear static subcase containing contact. Once this contact solution converges, the final contact stiffness (as well as the differential stiffness) is used to augment the structural stiffness in the subsequent normal modes analysis. The effect of the contact stiffness is similar to glue - the two faces are tied together at fixed locations and the contact does not re-open or close further in the subsequent modal or response analyis phases of the solution.

This approach is a sufficient simplification for analyses where the contact condition is not expected to change significantly as a function of the response. A typical example would be bolting two large, chunky solids together - i.e. a cylinder head to an engine block. The static subcase can solve for the bolt preload and the contact pressure between the head and the block. In a subsequent frequency response analysis, the structural stiffness and joint stiffness are high enough that the two components respond as a single entity(the cylinder head is not separating from the block in the frequency range of interest).

Regards,
Jim
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

MrRogers1987
  • Locked
  • Question
Contact Conductance in Riveted Joint
Replies
8
Views
16
geesaman.d
geesaman.d
Saleh abbasi
  • Locked
  • Question
Small contact region in COMSOL
Replies
1
Views
11
FEA way
FEA way
Bayram2014
  • Locked
  • Question
XY data report : Contact output duplicated
Replies
3
Views
10
Bayram2014
Bayram2014
mohamed hassan 2014
  • Locked
  • Question
Nonlinear analysis using HyperMesh with OptiStruct
Replies
0
Views
15
mohamed hassan 2014
mohamed hassan 2014
NASAJPL
  • Locked
  • Question
(Linear) Contact Force, but No Contact Pressure
Replies
2
Views
15
BlasMolero
BlasMolero
Back
Top