Hello.
I am simulating the transmission line structure by ANSYS 19.2 workbench. I use link 180 element and the initial shape of the transmission line is a parabola. Its connection between the transmission tower and line is assumed pin-pin connection. But I cannot realize the form finding part of transmission line. It always shows like this: The value of UZ at node 399 is 4.033743309E+13. It is greater than the current limit of 1000000 (which can be reset on the NCNV command). This generally indicates rigid body motion as a result of an unconstrained model. Verify that your model is properly constrained.
What should i check next? Thank you.
peteroznewmanpeteroznewman Posts: 11,376Member February 2019 edited February 2019
The shape of a cable hanging from towers is a catenary, not a parabola.
JackieXJackieX Posts: 21Member February 2019 edited February 2019
Hi. Thank you so much for your reply. I may not express clear.
Before ANSYS finding the transmission line's catenary shape of the transmission line, I use this equation to get its initial form: z=q/(2H)*x*(l-x)+c/l*x, H=q*l*l/8/f. Here q is the line load of transmission tower, H is the initial horizontal force, l is the span between two transmission towers, c is the height difference between two ends of the transmission line, f is the midspan sag. So I can get a set of coordinates of the initial shape of the transmission line. I use workbench 3D curve to generate this line. After this, I plan to find the catenary form of the transmission line by ANSYS. I use a method I found online: I first give small Young's modulus of transmission line and a initial strain about 1. After that, I adjusted the Young's modulus to the normal value of the transmission line and give about 0.0001 initial strain. But this method does not work. It shows the error like I showed on the previous question. so I do not know how to build the transmission line properly by ANSYS.
peteroznewmanpeteroznewman Posts: 11,376Member February 2019 edited February 2019
You wrote, "I first give small Young's modulus of transmission line and a initial strain about 1. After that, I adjusted the Young's modulus to the normal value of the transmission line and give about 0.0001 initial strain."
This is not a good strategy for converging on the true shape. The small Young's modulus allows large deflections that later need to be retracted. I see no advantage in this strategy.
JackieXJackieX Posts: 21Member February 2019 edited February 2019
Thank you so much for the quick reply.
So what should I do to find the catenary shape of the transmission line? I use link 180 element, I set it tension only. I use the end release connection to realize the pin-pin connection between the tower and line. But it does not work when I add load on it.
peteroznewmanpeteroznewman Posts: 11,376Member February 2019 edited February 2019
What is the purpose of your analysis?
If you start with the equation of a catenary you could mesh that with link180 elements. See the Elastic catenary section if the Wiki article, because that is what a collection of link180 elements would be.
Did you apply a gravity load to your model?
Do you have Large Deflection turned on?
Do you have Auto Time Stepping turned on?
Do you have Initial Substeps set to 100 (or 1000)?
JackieXJackieX Posts: 21Member February 2019 edited February 2019
I plan to simulate dynamic wind load on the transmission tower-line structure.
I have done all your questions: gravity load, large deflection on, auto time stepping on and inital substeps 1000. It shows this now: There is at least 1 small equation solver pivot term (e.g., at the UZ degree of freedom of node 398). Please check for an insufficiently constrained model.
What should i check next?
peteroznewmanpeteroznewman Posts: 11,376Member February 2019 edited February 2019
Set the Solver Type to Direct.
JackieXJackieX Posts: 21Member February 2019 edited February 2019
The node 398 is on the transmission line. It is a node created because of meshing.
jj77jj77 Posts: 843Member February 2019 edited February 2019
OK,
truss models, representing cables are very difficult to get to converge. Normally software have inbuilt cable element with a catenary formulation, and other features.
Now using truss elements one will calculate how the cable hangs/drops, and place the elements on that shape. That is the start.
The link180 is a truss element, and a chain of them is very unstable. Normally one uses displacement scaling sub steps to built up lateral stiffness (via geom. non-linearity). Before you apply gravity or any lateral loads, you need to built the nonlinear lateral stiffness via initial strains or stresses (tensile). So first initial strain, and then activate other loads.
Best to use the local element system when defining the pre-strains (strain causing tension is positive), this is done as shown below
INISTATE,SET,CSYS,-2 ! LOCAL ELEMENT SYSTEM FOR PRE-STRAINS
INISTATE,SET,DTYP,EPEL ! STRAIN
INISTATE,DEFINE,,,,,1E-7 ! STRAIN VALUE
If you are having troubles, attach the model and I will have a look (not sure If I can make it converge, in Strand7 I would, since this is the software I know and work with).
Also see verification VM31, where cables are modelled with LINK180 el.
JackieXJackieX Posts: 21Member February 2019 edited February 2019
Thank you so much!
I add the pre-strain based on your suggestion. It works now!
jj77jj77 Posts: 843Member February 2019 edited February 2019
You do not need to do any form-finding, unless it is part of your student work.
You can use Strand7 demo, run a cable element with gravity, and that will give you the catenary shape of the cable under gravity.
You can then write down (text file) all of the point/nodes along the cable and add them to a text file, which can be imported to design modeler as a point cloud, and then define lines along these points to get the correct cable. Unfortunate one can not copy paste the points on the cable from the Strand7 demo GUI (only possible in normal version).
JackieXJackieX Posts: 21Member March 2019 edited March 2019
Hi. Can I ask one more question about add load on the transmission line?
I imported the points of transmission tower from txt by design modeler 3D curve. In this way, there is no point for me to add load on the transmission line in Static Structure. Would you please give me some suggestions? Thank you so much!
jj77jj77 Posts: 843Member March 2019 edited March 2019
I used the Strand7 approach which gives me the nodes on the cable and they were imported as points in DM. Then trusses are defined based on these. In that way it is easy to apply vertex force or line force on these trusses.
If you do not have that (which I doubt, you must have many vertices and line bodies), then one can apply loads via commands, say the nsel,all and then f,all,fz,1, applies 1 N fz force on all nodes.
See the command reference in the ansys help for more information.
Might be another way which I can not think of now.
JackieXJackieX Posts: 21Member March 2019 edited March 2019
so you link your nodes from Strand7 approach by line in design modeler or 3D curve? I import my points by 3D curve in design modeler and I cannot add load on the transmission line.
jj77jj77 Posts: 843Member March 2019 edited March 2019
Correct, from the points, I use create line from points in DM to generate the line bodies that will later be the beam or truss elements.
JackieXJackieX Posts: 21Member March 2019 edited March 2019
Yeah, I just tried. I think line from points works. If I use 3D curve, there is no point on the transmission line for me to add load.
JackieXJackieX Posts: 21Member March 2019 edited March 2019
Hello, when I model tower by beam 188 and model transmission line by link 180, do I need to end release at their connection point?
saranshdikshitsaranshdikshit Posts: 14Member March 2019 edited March 2019
Hey! Could you share your ANSYS model? I have been trying to model link element as well for a cable and would be grateful if you could share a working model.
sdebodesdebode Posts: 7Member March 4
Hi, can anyone tell me if it would be possible to couple a link180 to a shell element? I am trying to model a structural membrane coupled to a link. But I cannot run it due to the error "link element references section 1(membrane) which is not a link section"?
Help would be appreciated!
ekostsonekostson Posts: 219Ansys Employee March 4 edited March 4
It seems like the section you reference for the link is the section for a membrane. So you need to have a separate section for the link element.
So say we have section for link, and section for shell, then it should be:
ET,1,180
ET,2,181
SECTYPE,1,LINK, ,
SECDATA,0.1,
SECCONTROL,0,0
SECTYPE,2,shell,,
secdata, 0.005,1,0.0,3
Thus when we define a link, we need:
secn,1
type,1
E,node1,node2
and for shell
secn,2
type,2
E,...
More info about these commands can be found in the help manual , apdl section.
All the best
Erik