Contact between solids & natural frequency extraction 1

[ADmek]

Dear ABAQUS users,

I am currently trying to see the behaviour of the contact interaction when running a natural frequency extraction analysis, and I having a trouble with the contact behaviour...Here is how I processed:

1- I first ran the natural frequency extraction of a thin-wall steel extruction, without any bounday conditions, in order to extract the first modes.

Here is how the first mode looks like:

http://files.engineering.com/getfil...-6c37d65769db&file=PlaqueSeule_0fix_mode1.png

2- I ran the same analysis, but with one end of the thin-wall extrusion considered clamped.

Here is how the first mode looks like. It's indeed not far from the previous one:

http://files.engineering.com/getfil...-087f5f15859a&file=PlaqueSeule_2fix_mode1.png

3- This time I considered that the thin-walled extrusion is now clamped at one end on a steel base, on which the extrusion is lying. A contact pair was defined between the two parts with the defaults properties. The master surface is an element set from the steel base, and the slave surface is a node set from the extrusion area in contact with the base.

Here are the results:

3.1 - Clearance=0.001
-- mode 1:

http://files.engineering.com/getfil...3-b24608333dda&file=AssComplet_2fix_mode1.png

-- mode 2:

http://files.engineering.com/getfil...6-329f5b12e5ce&file=AssComplet_2fix_mode2.png

3.2 - Clearance = OFF
-- mode 1:

http://files.engineering.com/getfil...46e&file=AssComplet_2fix_gravite_clearOFF.png

-- mode 2:

http://files.engineering.com/getfil...91b98&file=AssComplet_2fix_mode2_clearOFF.png

Here is the problem: according to the behaviour observed in the cases 1 & 2, the non-restained end of the extrusion should bend upward in the first mode, and "twist" around it's longitudinal axis in the second mode. This is nearly achieved when the *CLEARANCE is set off (case 3.2), but the contact between the two parts is not respected, as both of them are colliding. On the other hand when the *CLEARANCE option is set to 0.001 (case 3.1), the contact is respected but the non-restained end of the extrusion only slides over the base, and the first and second modes are completely differents.

For the case 3, here is how the analyses are run:

Step 1 (static): application of the gravity over the entire model
Step 2 (Nat.freq.extraction)

Would you consider another way to modelize the contact, or is it basically impossible to consider the contact during a frequency analysis?

Any help is welcome

 

[amubashar]

Hi,

Just an observation regarding the first point where you are extracting the natural frequency without any boundary conditions. Since there are no boundary conditions, the first six modes would correspond to the six rigid body motions and the first natural frequency will be given by mode 7. The picture attached with point 1 is showing Mode I with zero frequency corresponding to rigid body motion. You might be knowing that already.

Regards

Aamir

 

[ADmek]

Hello Aamir,

thank for notifying me that...I lost my pecision. the first natural frequency (mode 7 can be found here):

http://files.engineering.com/getfil...-f005edc0aec6&file=PlaqueSeule_0fix_mode7.png

 

[Noirom84]

As I've understood you want to combain natural frequency extraction with contact analysis? In my opinion that is impossiblem. You can't combine typical modal analysis with non-linear (quasi static) analysis.

Regards

 

[guru64]

Noirom84 is right.

Freuquency extraction is a Linear Petrubation Step. So by defintion it cant accomodate the non-linearities like Contacts. The Frequency Extraction considers the intial state at which the step starts and maintains that. That means, if a contact is closed at the begining of this step, it remains closed and if it is open, it will be open and will not see the contact.

Guru

http://www.abaqusguru.blogspot.com