## Ansys Workbench Commands (Cable type elements)

I am doing a nonlinear analysis in, Ansys Workbench, of a fuel tank tied down in an aircraft using cargo straps. I need to know how to insert a command function in Ansys workbench 11 that creates compression only elements (in order to model cargo straps). Based upon what have been reading I need to use a link10 element but I have no idea how write the command function to convert workbench pre-set elements (springs, beams, whatever..) into link10 elements. Any help would be much appreciated.

 PhysOrg.com science news on PhysOrg.com >> Heat-related deaths in Manhattan projected to rise>> Dire outlook despite global warming 'pause': study>> Sea level influenced tropical climate during the last ice age
 Recognitions: Science Advisor This would be much easier to do in Classic (now known as Mechanical APDL). Anyways, without the software at hand, let me give it a go. Let's assume for the moment that your tank is a simple cylinder that you're going to model with solid elements. Open DesignModeler and either create your cylinder or import your geometry. You'll then need to either hand draw the straps, or being them in along with the geometry. They need to be lines, not surfaces or volumes. Typically at this point in MAPDL you would simply define your LINK10 elements and section properties and LMESH that line, however it's much more of a pain in the *** to do in Workbench. Open mechanical. You should have 4 bodies: the cylinder, two straight lines and a curved one on top of the tank. Right click on the analysis type (e.g. Structural Analysis) and click Commands. This will put a commands line in with your loads/boundary conditions. Ansys allows you to insert APDL commands using this command feature, however some commands are limited in Workbench; there is much you cannot do in Workbench. OK, at this point, you need to redefine the elements. Ansys counts each body as gives it its own element type. The top listed body is ET,1. The next is ET,2, etc, etc. So, if the tank is the first listed body, then you'll need to: Code: /PREP7 ET,2,10 ET,3,10 ET,4,10 At that point, you'll need to redefine the real constants for those elements as well. I think those include masses and things like that. I also think there is a keyopt which needs to be set to say tension/compression only. Now, this is assuming that this will all work in Workbench. I've recently had some LINK10 experience that I'll share and hopefully it will help. My analysis was a cantilevered fuel tube that was supported with safety wire. I was doing modal analysis on it. My analysis did not work with simply meshing the line. Each wire had to be one element. If it was meshed with multiple elements, then the slack sides would really jacked up. You may have to specify a meshing control in that code snippet as well to try and get one element. If that doesn't work, I've heard of people using beam elements and then inserting one single small link element at the endpoint. Anyways, hope this helped, good luck. p.s. You'd do yourself a lot of good to switch to Classic. Upgrade to v12 and use it as a frontend for managing your analyses (new module-based approach) and importing CFD BCs, but export each to an APDL.
 minger Very cool, I used your method and was able to get a working model. I tweeked a few things but for the most part it worked. Also I discovered that if my KEYOPT(3) is set to zero I can mesh the beams representing the straps with multiple elements and have little trouble in regards to erronous deflections. Thanks again for the help. Another way I was shown this was to write a program that converted beam188 elements to link10 elements. See bleow, the original program converted spring14 elements in workbench to link10, but I fudged the program a bit to convert beam188. fini /prep7 *get,t_max,etyp,,num,max /com,before etlist elist *do,jj,1,t_max-1 /gopr *get,type_jj,etyp,jj,attr,enam *if,type_jj,eq,188,then et,jj,10 mp,ex,jj,10e6 ! ex of the link10 elements r,jj,20 ! cross sectional area *endif *enddo /com,after etlist elist fini /solu

Recognitions:

## Ansys Workbench Commands (Cable type elements)

BEAM188 have a tension/compression only keyopt?

OK, without the "actual" reference in front of me, I was able to find a copy of the BEAM188 reference. It doesn't show a KEYOPT,3 (only 2,5,6-9). Are you sure you're getting what you think you're getting?

 Oh my bad I guess I was talking about 2 different things. I used your program with my model and set my keyopt(3) to 0 for a slack cable. The mention of the beam188 was in regards to the other program that I posted, which converts the beam188 elements in workbench to link10 elements. I am still experimenting with my results to make sure things are behaving as expected. Hope all is well.
 Recognitions: Science Advisor Can I ask how your modeling the contact between the tank and the straps?
 I created a hybrid part using design modler so that coinicdent nodes were auto generated at the cable/box interface.

 Quote by BlkHwkEng I created a hybrid part using design modler so that coinicdent nodes were auto generated at the cable/box interface.
Also as I have gone deeper into the rabbit hole of this analysis I had to turn on the Beta options tool/options menu so I could create beam contacts. The stress around the contact seems to be garbage but I am really not interested in this anyhow.

 Recognitions: Science Advisor I've tried the beam contact beta option as well without much luck. What kind of loads do you have? I would assume some sort of lateral ACEL load?

 Tags analysis, ansys, compression, link10, workbench