Steady State Dynamics - noise in plot

[TB2000]

I constructed a simple SDOF model, using a cube mass (C3D8) , SPRINGA and DASHPOTA elements. The spring and dashpot were in parallel and shared same nodes. A vertical CLOAD force was applied to cube. All DOF were restrained so the model only moved in Z-dir.

The plot of the displacement of the cube looks right but noisy. Is this to be expected as i cant see where i went wrong?

*NODE
1,0,0,1
2,0.7071067811865,0,1.707106781187
3,0.2071067811865,0.7071067811865,2.207106781187
4,-0.5,0.7071067811865,1.5
5,-0.5,-0.7071067811865,1.5
6,0.2071067811865,-0.7071067811865,2.207106781187
7,-0.2928932188135,8.659274570719E-17,2.707106781187
8,-1,8.659274570719E-17,2
9,0,0,0
*ELEMENT,TYPE=C3D8
1,1,2,3,4,5,6,7,8
*ELEMENT,TYPE=SPRINGA
2,9,1
*ELEMENT,TYPE=DASHPOTA
3,9,1
*ELSET,ELSET=Element_Selection
1
2
*ELSET,ELSET=MASS
1
*ELSET,ELSET=SPRING
2
*ELSET,ELSET=Damper
3
*MATERIAL,NAME=Material
*ELASTIC,TYPE=ISOTROPIC
210000000000,0.3
*DENSITY
7850
*SOLID SECTION,ELSET=MASS,MATERIAL=Material
*SPRING,ELSET=SPRING

3.600000000000E+007
*DASHPOT,ELSET=Damper

6000
*BOUNDARY
1,2,0
1,1,0
2,2,0
2,1,0
3,2,0
3,1,0
4,2,0
4,1,0
5,2,0
5,1,0
6,2,0
6,1,0
7,2,0
7,1,0
8,2,0
8,1,0
9,1,0
9,2,0
9,3,0

*STEP
*FREQUENCY,STORAGE=YES
1
*END STEP

*STEP
*STEADY STATE DYNAMICS, HARMONIC = YES
10,12,300
*CLOAD
1,3,100000

*NODE FILE
U
*END STEP

[jbr]

@TB2000

The plot of the displacement of the cube looks right but noisy. Is this to be expected as i cant see where i went wrong?

What is your expectation of the graph? You are requesting a single mode extracted and then doing a steady state dynamics from 10 to 12 Hz with 300 points, what are you expecting to see?

[TB2000]

Thanks for taking a look.
I was trying to plot the resonant displacement response curve for the SDOF model between 10-12Hz. The resonant freq is 10.78Hz. So if looking at absolute values i should have got a curve similar to this amplification curve (fn=10.78, Z=0.0056).

The flip is due to the phase change at resonance.

[Disla]

Could you show displacements on the other two components?

[jbr]

@TB2000

The resonant freq is 10.78Hz

Did you get that from the output file? Check the *.dat file for the values. Those should match. Looking at the nodes, maybe something is wrong with how you set it up. Looking at your values for stiffness and density, it doesn’t add up to 10.78Hz, can you check that too?

[vicmw]

The constraints in *BOUNDARY are wrong and not being enforced, which you can see from the other displacement components being non-zero. Change
1,2,0
to
1,2,,0
etc. The extra comma indicates an omitted parameter (last DOF).

However, Discourse corrupts text by removing extra commas so your original file is probably fine. Better to use code formatting for .inp files like I did above to prevent that.

[jbr]

Try to request the magnitude of U3 instead of just the value of U3. I got a similar curve to the one you showed.

[JuanP74]

you have forgotten that this model is not a point mass plus a spring but there are at leat 2 springs 1: the springa and the stiffness from the solid cube, probably with very different eigenfrequencies and furthermore a point element attached at a corner of a solid element may create mathematical distortions. And you have cut the model response to the first mode only. So I am not sure that the response you expected is the one of the model you created.

[TB2000]

How are you graphing the ABS(complex displacement) ? What command should i use ?

i make a set for a node (NODESET)
then
graph NODESET time DISP D3.

Or do i have to use *node print and then write a script to get ABS or real+complex component at each frequency.

[TB2000]

I would have thought if i request using mode 1 only it should be ok as the higher modes would be excluded. Also i did try the model with a mass on the node instead of the cube. It kept failing as it said i didn’t have an elastic restraint condition for the mass. I gave up and used the cube.

[Disla]

I’m getting a clean curve.
I had to fix the Boundary card adding an extra coma. There was displacements into x and y components.

@TB2000

It kept failing as it said i didn’t have an elastic restraint condition for the mass

I have experience this before and solved it by accident. Check this post. Solution seems to be adding a solid dummy element.

DAMPING should be preceded by a *MATERIAL card

Thanks to both of you, I was preparing the proposal of the cube at the tip and …surprise. If a dumb cube is added to the system the matrix is assembled and the problem is solved with the springs. I am referring to a loose cube. I have yet to see if the result makes sense but it is surprising isn’t it?:joy: [imagen]

EDITED: I suspect eigensolver can’t solve a problem with just one mode.

[JuanP74]

@Disla

I suspect eigensolver can’t solve a problem with just one mode.

I thought this was fixed in V2.21

[Disla]

Hi Juan and Happy Christmas,

That’s true, 2.21 now can end up the analysis with that old
( no elastic constants were assigned to material MASS in a (thermo)mechanical calculation) error…… but,
one can’t request to extract the same number of modes that the system has.
One Spring, one dashpot and one mass element all constrained but one z, is a system with a unique mode. The eigen solver can’t extract it.
If I add a second dummy element or spring (with a higher mode !!!) to rise the number of modes of the system , then it works. Of course, the steady state solution for the second element is empty.

*NODE
1,0,0,1
2,0,-1,1
3,0,0,0
4,0,-1,0
*ELEMENT,TYPE=DASHPOTA
1,4,2
3,3,1
*ELEMENT,TYPE=SPRINGA
2,3,1
4,4,2
*ELEMENT,TYPE=MASS
5,1
6,2
*NSET,NSET=N_LOAD
1
2
*ELSET,ELSET=ELEMENT_SELECTION
2
4
*ELSET,ELSET=SPRING
2
4
*ELSET,ELSET=DAMPER
1
3
*ELSET,ELSET=SPRING2
4
*ELSET,ELSET=SPRING1
2
*ELSET,ELSET=Mass_1
5
*ELSET,ELSET=Mass_2
6
*DASHPOT,ELSET=DAMPER

6000
*SPRING,ELSET=SPRING2

4.600000000000E+007
*SPRING,ELSET=SPRING1

3.600000000000E+007
*BOUNDARY
1,1,,0
1,2,,0
2,1,,0
2,2,,0
3,1,,0
3,2,,0
3,3,,0
4,1,,0
4,2,,0
4,3,,0
*MASS,ELSET=Mass_1
7850
*MASS,ELSET=Mass_2
7850
*STEP
*FREQUENCY,STORAGE=YES
1
*END STEP

*STEP
*STEADY STATE DYNAMICS, HARMONIC = YES
0,20,20,3

*CLOAD
N_LOAD,3,100000

*NODE FILE
U
*END STEP

[JuanP74]

you were right, it was due to a particularity in the CGX commands to generate the plot, the manual is somewhat cryptic in this respect, the proper sequence for a postprocessing .fbd file is:

read steadydyn.frd
seta node5 n 5
ds 1 3 eh 3
graph node5 time

otherwise in the .out file you see couples of numbers for each frequency corresponding to real and imaginary parts.

[JuanP74]

Merry Xmas to you as well and many thanks for a year of challenging discussions!

[TB2000]

Thank you all for a nudge in the right direction. Merry Xmas

[Calc_em]

I have an example of SSD analysis of SDOF system here: https://www.youtube.com/watch?v=dLkmF7UesgE

In Abaqus, I would use mass, spring and dashpot elements but here I was limited by the capabilities of PrePoMax and CalculiX so I only used a discrete spring element.