Tranmission tower cable simulation in ANSYS Workbench

  • 155 Views
  • Last Post 05 May 2019
  • Topic Is Solved
saranshdikshit posted this 01 April 2019

Hi everyone, I have been trying to model a 200 ft long cable in ANSYS. I have 42 elements along the length of the cable. Each element serves as an element for each line. I read through a lot of posts about cables. I have turned on large deflections and added the lines in the APDL command to convert beam elements to link elements. Also, I have added a bit of initial strain to the link elements. I have made the two ends of the cable as pin supports and applied a point load ( static load) in the center of the cable in the downwards direction. I have been trying to solve the model but I have been getting the solver pivot error and the internal solution magnitude exceeded error. Right now I am just doing static analysis. Later on I would like to do transient analysis. I would be grateful if someone could help me debug this issue. I have spent a lot of time on this and anyone's help will be greatly appreciated.

Order By: Standard | Newest | Votes
jj77 posted this 02 April 2019

Hard to say (pivot error can mean often that it is not really restrained well), but I would try to used fixed restrain at the two ends, alternatively remote displacement with all 6 dof fixed (that will be still be pinned since it is a 3 dof truss/link element). Also see some post for more details.

https://studentcommunity.ansys.com/thread/transmission-line-simulation/

 

 

Otherwise attach your model here and I will have a look,

saranshdikshit posted this 02 April 2019

I have attached my model with this reply. I even did the modal analysis of the cable. No part seemed to be flying off. The cable doesnt show rigid body motion. My main issue is with the static structural and transient analysis of the same cable. I would be really grateful if you could look at the model and let me know on how I can correct my mistakes. 

Attached Files

saranshdikshit posted this 02 April 2019

I went through the post that you recommended. I followed all the steps. Still I think I am missing a vital piece of info. Please share your insight about the model that I created. 

jj77 posted this 02 April 2019

First change the commands (take away the seccontrol):

 

*get,myarea,SECP,matid,PROP,AREA ! gets the area and  assigns it to myarea

ET,matid,LINK180 ! define link element

SECTYPE,matid,LINK ! assign link

SECDATA,myarea ! assign area

MP,EX,matid,,5.5E10 ! SI units

MP,DENS,matid,,8900 ! SI units

INIS,SET,CSYS,-2    

INIS,SET,DTYP,EPEL

INIS,DEFINE,,,,,1.5E-5 ! strain, unit less

 

One does not need to specify tension only (seccontrol) since this chain link can only be in tension(compression makes it unstable), hence remove that command.

 

Most importantly also before the force add gravity (first step), and then apply the load (second step).

(Two  steps are needed for this)

 

Change also the model units to SI (m,kg,..), and then in analysis data management settings set the solver units to manual and choose mks units system.

saranshdikshit posted this 02 April 2019

Thank you so much for your insight into this problem. What you are suggesting is that I need to create two load steps. In the first load step, only gravity (acceleration is present). In the second load step, both the acceleration and the force are present. In terms of the boundary conditions of the model, do they look ok? Also, what should I do with the analysis settings? In terms of auto time stepping, solver type, weak springs and inertia relief? If I can make my static analysis work, my next step would be to do a transient analysis. Would any of the options in the analysis settings change? For the transient analysis, could I again create two load steps? The first load step would just be gravity (acceleration) and the second load would contain numerous substeps with the loading values and the added acceleration due to gravity.  

saranshdikshit posted this 02 April 2019

Also, I had a question about the nonlinear controls present under the analysis settings. Should I tinker with the nonlinear controls for my static and transient study? 

jj77 posted this 02 April 2019

BC are OK (simply). You have understood the load steps also (step 1 gravity is only active,step 2 gravity + force are active).

 

Autotime stepping is OK, you need only say 10 10 20 in the settings (not 1000), to let the stiffness develop gradually. Also setting auto time stepping to programme controlled is fine here. 

 

Inertia relief does not work in large deflection analysis, and is used sometimes in free "floating" structures (e.g.. for ships, air planes) - weak springs are not necessary here.

 

Also for the transient use the two steps again.

 

Now for the transient (with inertia effects, thus mass matrix is assembled) the time steps used (capture dynamics) are based on the smallest period of the structure,thus time step = T_smallest/10. For impact, timestep = Impact_duration/20 or so.

saranshdikshit posted this 02 April 2019

Thank you for your insight. I did what you asked me to do. I added two load steps. Still I get the convergence error. I have attached the modified model for your perusal. Please have a look at the model and guide me whats going wrong. What happens if the load applied to the cable has a very high magnitude? Would I need more substeps? 

Also, in case of transient analysis, the time step would be governed based on the modal analysis and the frequencies I want to capture right?

Attached Files

saranshdikshit posted this 02 April 2019

 The only difference in number of substeps equal to 20 and 1000 is the time ANSYS takes to solve the problem right? With 1000, it would solve for 1000 increments of the load and vice versa. How does one decide the number of substeps to for a problem like the nonlinear case of cables?

jj77 posted this 02 April 2019

First thing, Set UNITS to SI (Metric). This is important since we get the section area and we want that to be in SI units (m2).

Second thing, do not apply acceleration (delete that) we said apply inertial standard earth gravity instead.

Finally set autotimestepping to programme controlled (no need for so many substeps, if needed solver will decide if it should substep - for more info : http://www.padtinc.com/blog/the-focus/you-dont-wanna-step-to-this-breaking-down-loadsteps-and-substeps-in-ansys-mechanical)

 

Late here now, take care for now 

 

PS: Yes for dynamics you need an idea of the modes/natural freq. Thus the time step is Period_small/10 where Period_small corresponds to the mode with the highest freq. of interest,

saranshdikshit posted this 02 April 2019

Thank you so much for your guidance. I will post on how my progress goes. Thanks again for your help!

jj77 posted this 02 April 2019

No worries. The acceleration that was applied forced the cable in the other direction opposite to gravity direction hence it goes into  compression and can not solve, thus to act in the grav. dir. we need to have it as +9.8 m/s2 thus opposite to the grav. dir. (a bit funny but that is how it works). Thus it is easier to always use gravity for a gravity load. see the help manual for more info on acceleration.

 

Talk to you soon

saranshdikshit posted this 07 April 2019

I was able to make the cable work. I was modelling a transmission tower with a set of beam and link elements. Would I need to add the commands for the link elements as the ones you have mentioned for all the elements as well?

zw123456 posted this 05 May 2019

 

Dear jj77 and Peter,

 

How are you? Could you please have a look?

 

1. The result of SMISC1 is 3.4165E5, is it too large for tension force? 

 

2. the result is not sensitive for lateral force only along Z axis?

 

3. The equation for calculation for initial strain, unit less  Y is young's modulus, F is pretension, A is section area?

 

 

 

 thanks for help!

 

 two cables are connected with beam (truss) for transmission line simulation.

 

 ====================================================================

 

 *get,myarea,SECP,matid,PROP,AREA ! gets the area and  assigns it to myarea

 

 ET,matid,LINK180 ! define link element

 

 SECTYPE,matid,LINK ! assign link

 

 SECDATA,myarea ! assign area

 

 MP,EX,matid,,5.2E10 ! SI units

 

 MP,DENS,matid,,1828.57 ! SI units

 

 INIS,SET,CSYS,-2   

 

 INIS,SET,DTYP,EPEL

 

 INIS,DEFINE,,,,,5.53E-4 ! strain, unit less

 

 =======================================

 

 Boundary condition:

 

 Vortex 1,5, 6: no displacement

 

 Vortex 4: displacement in x and z axis

 

 Vortex 2,3: displacement in z axis

 

 Element:

 

 Cable: link180

 

 Beam: beam188 (truss)

 

 Force 1: (0,0,-4N/m), Force 2: (0,0,-1N/m), applied to line body edge

 

line body: 3D curve in DM

 

beam radius=0.03m, cable radius=0.015m

 

zw123456 posted this 05 May 2019

Close