ANSYS APDL Low Frequency Result in Modal Analysis

[hanxi]

Dear All:

Good day.
I've performed a Modal Analysis in ANSYS APDL simulating the Concrete Foundation Embedded in the ground (around 1.0 meter).
I made my foundation model using Solid185 and used MASS21 for machine dead loads (these dead load + the selfweight will comprise my MASS for frequency calculation). For the support condition, I used COMBIN14 for 6 cases: UX UY UZ ROTX ROTY ROTZ. I made coincident nodes (making zero-length element which will simulate spring) and at the ends of zero-length element, I've used fixed constraint.
Basically, analysis runs smooth but I'm wondering of the resulting frequencies.

The resulting 1st to 6th frequencies are within the range of 0.1~0.8Hz. But the 7th frequency it jumped to 2.1Hz and so on for the higher order frequencies.

My questions are:
1) Are the result reasonable?
2) Is my procedure of using Combin14 considering 6 Springs correct?
3) Can I ignore frequencies between 0.1~0.8Hz (f1 to f7) and make f7 as the 1st mode of my analysis?
4) Also, this is related to question #3, If I consider free-free vibration (meaning deleting all spring constraints), the first 6 modes are Rigid Body Modes which should have frequencies nearly 0Hz, does it mean f7 is the first mode of my analysis?

Thank you for your forthcoming responses.
Good day to all.

Hanxi

 

[TERIO]

1) It would be hard for anyone to say if your calculated frequency in reasonable without have some idea of mass, stiffness, geometry, and other info about your model.
2) Certainly you can use combin14 to model a spring. Probably the more interesting thing is determining the appropriate spring constants. Also, since solid elements don't have rotation degrees of freedom it is not clear to me what your rotational springs will do.
3) Why do you want to ignore them? Once you find the modes what do you intend to do with them?
4) What do the mode shapes look like?

 

[hanxi]

Good day Terio.
Thanks for the reply. Meanwhile, for clarity of the problem, let me redefine the problem:

ANSYS Model:
Block Foundation with base are dimension L=12.285m and W=8.900m (Used SOLID185)
Total Mass (Selfweight) = 10,000 kN (Used ACEL command)
Total Machine Weight = 1500 kN (Used MASS21)
Machine Rotating Speed = 6 HZ

Boundary Condition: (for the FULL MODEL)
K11 = 5.0E+06 kN/m
K22 = 6.0E+06 kN/m
K33 = 5.0E+06 kN/m
K44 = 3.0E+08 kNm/rad
K55 = 4.0E+08 kNm/rad
K66 = 3.0E+08 kNm/rad

These Spring Constants K11~K66 are obtained from a third party program.
To simplify, the notations K11, K22, K13, K44, K55, K66 pertains to Spring Translation restraint along X, Y, Z and Rotational restraints about X, Y, Z, respectively.

Summarized below are the procedures I performed:

1) Modeling of block foundation using SOLID185
2) Modeling of lumped machine weights using MASS21
3) There are a total of 150 nodes at base location (spring support location). We refer to this a SUPPORT NODES
4) Generation of 6 coincident nodes for each SUPPORT NODES (6 because I have 6 spring constants. If you noticed I've used SOLID ELEMENTS for my modelling and I'm aware that NODES of this solid element DO NOT HAVE Rotational Capability. I'm not sure if I will ignore the Rotational Springs since the Client provided me Rotational Springs. "Maybe you can comment on this method")
5) Modeling of Spring Element for coincident nodes using COMBIN14 for 6 sets (X,Y,Z,ROTX,ROTY,ROTZ)
6) Kindly take note the the VALUES of Spring Constant for each SUPPORT NODES are taken as:
Spring K for each node = Spring Value (for FULL MODEL) / 150 nodes
7) Performing ANSYS MODAL ANALYSIS using the below command line:

FINISH
/CLEAR

RESUME,'K1001-1100-MODEL','db','.'
/FILNAME,K-1001-MODAL(6.0HZ)


FREQ = 6.0 !HZ
/SOL

ANTYPE,2
EQSLV,SPAR
MXPAND,100, , ,0
MODOPT,LANB,100,0,1.5*FREQ, ,OFF

/output,outputfile,out
SOLVE

FINISH
/output

After the MODAL ANALYSIS, I got the following from output:

*** FREQUENCIES FROM BLOCK LANCZOS ITERATION ***
MODE FREQUENCY (HERTZ)
FREQUENCY RANGE REQUESTED= 0.00000 8.85000
1 0.3065373168673
2 0.3513237790095
3 0.3913485982358
4 0.9157331996164
5 1.030886553010
6 1.083972906072
7 1.866312791262
8 2.258646677570
9 2.481456086583
10 2.489518386723
11 2.554872007164
12 2.676282048282
13 2.817612645348
14 2.841658783466
15 2.976208364247
16 3.099926114316
17 3.353721411111
18 3.463519243771
19 3.602616190552
20 3.656991353921

From these result, I just wanted to verify if my procedures and the resulting frequencies is reasonable because the same model above were model and analyzed using two (2) other FEM Software and both software has resulting frequency around 4.0 HZ for the 1st mode (for both software).
I wonder if there's something strange in my modeling in ANSYS that lead me to a LOW FREQUENCY in 1st Mode.
Any thoughts folks?
Thanks.

 

[hanxi]

Dear All:

Also, If I used basic Mechanics formula for Single DOF, we have frequency = sgrt(stiffness/mass).
Applying this to my problem, we have:

1st frequency = sqrt {[5.0e6kN / 9810kg-m/s^2] / [(11500kN / 9810kg-m/s^2]}
This yields f= 21 rad/s or approximate 3.3Hz... This value is somewhat far from Ansys f1 = 0.3Hz...

 

[hanxi]

Errata for my previous post:

1st frequency = sqrt {[5.0e6kN/m x [(9810kg-m/s^2)/kN]} / [(11500kN / (9810kg/kN)]

 

[TERIO]

I think you have the units wrong in both checks above. 1 N = 1 kg-m/s^2 or 1 kN = 1000 kg-m/s^2. You should probably also go through and double check that your units are consistent in the ANSYS model as well.

 

[hanxi]

Good day Terio:

Thank you for your response.
Meanwhile about equivalence of N and Kg, my understanding is like this:
1 kg x 9.81m/s^2 = 9.81kg-m/s^2, hence 1kg = 9.81 kg-m/s^2 or simply 9.81N....

If this is wrong, did I overlooked something?
Thanks

 

[TERIO]

Yes. W = mg (as you show), or m = W/g = 11500 kN / 9.8 m/s^2 = 11500 kN * (1000 kg-m/s^2/1 kN) / 9.8 m/s^2 = 1.17e6 kg

If you are already working with weight a quick way to do the natural frequency calculation is omega=sqrt(k/m)=sqrt(k/(W/g))=sqrt(k*g/W)=sqrt(5e6 kN/m * 9.8 m/s^2 / 11500 kN) ~ 65 rad/s or ~ 10 Hz.

Exactly what units have you used in the ANSYS model for mass (Mg?), density (Mg/m^3?), length (m?), force (kN?), pressure/stress/elastic moduli (kN/m^2 = kPa ?), time (s)? ANSYS doesn't know what units you are using so they must be consistent.

Also based on the weight you provide and the two dimension I get that your foundation is close to 4 meters thick. Is this correct?

 

[hanxi]

Dear Terio:

Thank you for your response.
For ANSYS model, I've used the following units:
Loads/Weight = N
Length = mm
Density = kg/mm^3 (for material property)--- Is this correct? or do I need to use N/mm^?
Mass21 Loading = kg --- Is this correct also? or do I need to use N?

Regards.

 

[TERIO]

No, that is not ok. I've given a lot of hints but short of doing it for you (which I won't do), I can't provide much help by one or two sentence exchanges every couple days. It would be beneficial for you to find somebody local (in your office?) to teach you.