For more detail. Please refer following papers.

https://www.researchgate.net/profile/Ghanshyam_Tejani/publications

http://www.sciencedirect.com/science/article/pii/S2288430016300653

http://www.tandfonline.com/doi/full/10.1080/0305215X.2016.1150468

http://www.tandfonline.com/doi/full/10.1080/15397734.2015.1124023

http://www.sciencedirect.com/science/article/pii/S2288430015300439

Let me define this problem ones again. This problem belong to simultaneous size, shape and topology optimization of 24-bar truss structure with static and dynamic constraints. That, I already optimized using 30 algorithms.

Now, I need to validate the best results using ANSYS APDL. I have already solved this problem for static constraints. However, I failed to search frequency constraints. Therefore, it requires modal analysis to find its natural frequencies.

Final data is as follow:

Nodal coordinates (in m)

Node number(x,y):

1(0,2.5)

2(2.5,3.25)

3(5,4)

4(7.5,2.5)

5(2.5,0)

6(5,0)

7(1.792,0) (Fixed)

8(7.186189,0) (Fixed)

Element Number, node end1, node end2, Area in m2

7, 2, 7, 0.0013 (Remaining elements are removed, After topology optimization it has only 8-bars)

8, 2, 5, 0.0003

12, 2, 3, 0.0003

13, 3, 7, 0.0021

15, 3, 6, 0.0004

16, 3, 8, 0.0024

22, 7, 5, 0.0001

24, 6, 8, 0.0001

Modules of elasticity E = 6.9e10 N

density = 2740 kg /m3

lumped mass 500 kg at node 3.

I need its natural frequencies in ANSYS APDL.

As per Matlab results I got following natural frequencies:

f1 30.3936 f2 46.7040 f3 156.4569 f4 219.4590 f5 292.6373 f6 325.4761 f7 518.0560 f8 538.0699

That I need to validate using ANSYS APDL.

If you need more details please ask.

My cell number is +919824899801

You model looks fine but you have not yet added the lumped mass.  This is done by declaring a mass element with the appropriate mass/inertial properties and then creating point mass elements where they are required.  Hope that is helpful.

Dear Dr. Ramsay,

Thanks for valuable suggestion. The attached code is showing an error.

Dear Dr. Ramsay,

I would be glad if you please show steps of ANSYS APDL of How to assign lumped mass?

Now the code is giving exact answer in ANSYS APDL without Lumped mass. I request please educate me to assign lumped mass. 

Thanks

with

Best regards

Following code is working. However I need to define lumped mass at a node.

/NOPR ! Suppress printing of UNDO process

/PMACRO ! Echo following commands to log

FINISH ! Make sure we are at BEGIN level

/CLEAR,NOSTART ! Clear model since no SAVE found

! WE SUGGEST YOU REMOVE THIS LINE AND THE FOLLOWING STARTUP LINES

!*

/prep7

! Node 1 is located

n,1,0,4.820523

n,2,2,3.695932

n,3,4,4.399216

n,4,4,2

n,5,2,2

n,6,0,2

n,7,4,-0.800993

n,8,2,0.791178

n,9,0,-0.381448

et, 1, link1 ! Element type; no.1 is link1

r,1,0.0021,,

r,2,0.0004,,

r,3,0.003,,

r,4,0.001,,

r,5,0.0002,,

r,6,0.0007,,

r,7,0.0024,,

r,8,0.003,,

!First Material

mp, ex, 1, 69e9 ! Material Property, Elastic modulus no. 1

mp, prxy, 1, 0.3

mp,dens,1,2740

! 'Real Constant' (Cross sectional area)

real, 1

en,1,1,2

real, 2

en,4,5,4

real, 3

en,5,9,8

real, 4

en,8,2,5

real, 5

en,11,5,8

real, 6

en,13,1,5

real, 7

en,15,2,4

real, 8

en,20,4,8 Element connectivity

FINISH

/SOL

!*

ANTYPE,2

!*

!*

MODOPT,SUBSP,8

EQSLV,FRONT

MXPAND,8, , ,0

LUMPM,0

PSTRES,0

!*

MODOPT,SUBSP,8,0,0, ,OFF

RIGID,

SUBOPT,8,4,12,0,0,ALL

!*

!*

FLST,2,2,1,ORDE,2

FITEM,2,1

FITEM,2,9

!*

/GO

D,P51X, , , , , ,UX,UY, , , ,

/STATUS,SOLU

SOLVE

FINISH

/POST1

SET,LIST

)/GOP ! Resume printing after UNDO process

)! We suggest a save at this point

Hi,

this is a purely technical problem. I hope you have already solved it. However, I modified a little your last code and placed below. See comments in the code for the added mass element. It works (assuming ANSYS version 11 or later). Although the results of frequencies are not matching the values you reported. Maybe the element properties and real constants should be rechecked to be sure that it matches the ones used in Matlab code.

Regards,

Ev.

FINISH

/CLEAR

!*

/prep7

! Node 1 is located

n,1,0,4.820523

n,2,2,3.695932

n,3,4,4.399216

n,4,4,2

n,5,2,2

n,6,0,2

n,7,4,-0.800993

n,8,2,0.791178

n,9,0,-0.381448

et, 1, link1 ! Element type; no.1 is link1

ET,2,MASS21 !* Element type mass21

! r - 'Real Constants' (element properties e.g. Cross sectional area, etc.)

r,1,0.0021,,

r,2,0.0004,,

r,3,0.003,,

r,4,0.001,,

r,5,0.0002,,

r,6,0.0007,,

r,7,0.0024,,

r,8,0.003,,

R,9,500,500, , , , ,!* 'real constant' of mass21

!***                          (500 kg in X and Y directions since link1 is a 2D link).

!First Material

mp, ex, 1, 69e9 ! Material Property, Elastic modulus no. 1

mp, prxy, 1, 0.3

mp,dens,1,2740

!

real, 1  ! real - 'Real Constant' used when creating a following element

en,1,1,2

real, 2

en,4,5,4

real, 3

en,5,9,8

real, 4

en,8,2,5

real, 5

en,11,5,8

real, 6

en,13,1,5

real, 7

en,15,2,4

real, 8

en,20,4,8

REAL, 9 ! real constant used for element # 100

TYPE, 2 ! element type used when creating an element # 100 (default is 1)

EN, 100, 4 ! element # 100 (mass21) on node 4

FINISH

/SOLU

!*

ANTYPE,2

!*

MODOPT, LANPCG, 8 ! PCG Lanczos eigensolver

MXPAND,8

!*

FLST,2,2,1,ORDE,2

FITEM,2,1

FITEM,2,9

!*

/GO

D,P51X, , , , , ,UX,UY, , , ,

!

SOLVE

FINISH

/POST1

SAVE

SET, LIST

Dear Sir,

Thank you very much for your time and effort. I really appreciate your support. Yes, you are correct I have solved this problem and it gives perfect answer. 

Thanks ones again for your continuous support

with

Warm regards