Surface to surface contact condition and Normal mode calculation


Hi everyone


I am studying how to calculate normal mode with Surface to Surface Contact condition applied.


0.Contact_test_Model.PNG1. Model configuration(Spaced 1mm aprt)1.Mode shape Without Contact.PNG2.Normal mode(with out STS Conditions , The Edege of the large Plate are all clamped)2.Mode shape With Contact(without Gravity).PNG3.Normal mode(with STS Conditions but not gavity applied)3.Mode shape With Contact(with Gravity).PNG4.Normal mode(with STS Conditions with gavity )4.Contact Pressure without gravity.PNG5. Contact Pressure(No gravity)5.Contact Pressure with gravity.PNG6. Contact Pressure(with gravity)


My model has two flat plates connected by spot welding as shown in the Figure 1 .

If there is no  STS Contact condition, the first natural frequency is 25.8 Hz.(Figure 2)


If there is  STS Contact condition But the gravity is not applied, the first natural frequency is 34.8 Hz.(Figure 3)


If STS Contact and gravity are applied, the first natural frequency is 120.3 Hz.(Figure 4)


if Gravity is not applied , the distribution of the contact pressure is very strange.(Figure 5)


My question is as below...


1. Why do I have so many different natural frequencies with and without gravity?


2. Assuming that applying gravity is a better condition, the natural frequency is  too high when applying STS Contact conditions.(This results is not realistic...)

How can i get more realistic results?....


3.If the STS Contact condition is applied , the plates are attached and moves together like Glue condition..


How do I get the same mode shape that Blas Molero (https://iberisa.wordpress.com/2011/11/07/analisis-de-frecuencias-sol103-de-un-ensamblaje-con-contact...) did?

(i.e. No penetration but not attached during mode shape animation)


Is it possible with Sol103?


I attached fem and sim file and please let me know if i had imposed an inappropriate conditions.


Any answers will be very helpful.









Re: Surface to surface contact condition and Normal mode calculation

Siemens Phenom Siemens Phenom
Siemens Phenom

The animations on the web page you reference are deceiving because the video only shows 0 to max displacement (a Linear animation in Simcenter terminology). To see the full mode shape, the author should have used a Modal animation (-max to max). This is why you are not seeing penetration in the Mode#3 = 2377.522 Hz animation.


Here is the linear animation:

(view in My Videos)


And here is the corresponding modal animation:

(view in My Videos)



A couple of issues particular to your model:

  • Without the gravity load, there is no load on the model, so the contact forces go to 0.0 and there is no contact stiffness generated to transfer to the modal subcase
  • With the gravity load, contact forces (an corresponding contact stiffness) are generated. This is transferred to the modal subcase and essentially behaves as glue in this subcase.


Re: Surface to surface contact condition and Normal mode calculation

First of all thank you for your valuable answers.
I have additional questions about your answers.
1. Do I need to load(or Gravity) to get Contact Stiffness?
first of all, to generate contact element.. Normal vectors of Source region and Target region must intersect and distance between source region and Target region must be less than Max Search Distance in BCTSET CARD.
after Contact element generated.. Contact element Stiffness is calculated as follower(From NX nastran User's Guide)
(When PENTYP=1 Defult) K=e * E * dA ( e= PENN or PENT , E=Elastic modulus , dA= area)
In my opinion, contact element Stiffness do not need "external load" ...  so Do i need to apply gravity in my model?..
2. If Surface to Surface Contact condition is given and the Two Plates move together
What is the difference between a contact condition and a Glue condition?
Best regards.

Re: Surface to surface contact condition and Normal mode calculation

Siemens Phenom Siemens Phenom
Siemens Phenom

The equation shown shows how the initial contact condition is created. During the solution, the solver iterations will deactivate contact elements that have separated or have no normal force in them. So, even though contact is initially set up as you describe, at the end of the static subcase, most or all of the contact elements will be inactive if there is no load or interference in the model.