ANSYS Workbench - Spreader - Lifting simulation (Stress)
ANSYS Workbench - Spreader - Lifting simulation (Stress)
(OP)
I have STEP model of simple spreader (I beam) with two lifting lugs for my home assigment. I want to simulate liffting of 2 ton load with my spreader. How to simulate lifting (lifting chains)in Ansys Workbench 16 only to transfer movment. What constraints to use. I don't need stress in lifting chains or lifting equipment, only in spreader and lifting lugs (When spreader is loaded with 2 ton load).
Thank You very much.
Thank You very much.





RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
Or to use cylindricat support with tangential component set to Free and apply it to internal surface of eaxh lifting lug opening ?
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
first, symmetrical half is sufficient. It also provides more stability. I would proceed as following:
1, model half of the loadspreader
2, fix the symmetry face all 6 DOF
3, Apply vertical load on the lower lug (10 kN)
4, Apply load in direction of the lifting chain (you know angle, you know the reaction force in chain)
your analysis should be in equilibrium so the fixed symmetry face should not give any significant reactions but provides stability to solution
If you use ANSYS Workbench you could use bearing load for force application as it gives proper distribution on the lugs.
Regards,
Pavel
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
here is what I have tried with skid mentioned in previous post.
I don't still know what is right approach when you want to simulate and calculate stress state in skid or spreader that is lifted in air and loaded. Maybe non of avaialble approaches are good.
How to find resultant forces in direction of fictive chains ? (I don't want to calculate them by hand because offten load is not in center of gravitiy of system - it is distributet asymmetrically and one lifting lug has bigger reaction forces then another)
Do I need to model chains ? Then are that chains elastic or rigid ? How to set them to be rigid ?
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
Any help wold be good.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
You can split the lug inner surface so that the spring is attached only to one half.
As said before, to achieve a proper stress distribution in the lugs, bearing load can be used.
Maybe you can get the value and direction of the bearing load from the first analysis (with chains modelled as springs).
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
As mentioned in previous post: if the geometry and loading are symmetrical, you can model half/quarter of the model.
I would model either a chain or a bearing force on the lug inner surface. If you choose to use bearing force, you have to calculate it by hand. You
can create a local coordinate system in direction of the chain to define the load. Remember to split the lug inner surface so that the force or chain
is not acting on the whole surface.
If your load is not evenly distributed on the platform, I think you have to model the chains. In that case there is no symmetry either.
http://files.engineering.com/getfile.aspx?folder=9...
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
If I replace chains with cicular bars that are overdimenisoned (for example 20 mm diameter) I will get reactions in them. But If I use for example cicular bars (40 mm) what effect will it have on my deformation and stress in structure. Will calculation it be valid regarding stress distribution and displacement values.
I tried to use remote displacement for this but I can not get reactions in the direction of the chain as they should be in reality. (Or x,y,z component - I don't know how to get them)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
you can only extract this resultant.
If remote displacement (one/lug) is used instead of spring element, you will get as many force reaction components as you have constrained.
If you set x=y=z=0, you will get three components. I would check that remote displacement results (deflections and stresses) correspond to spring results.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
1. The hook position should be located right above the skid weight center
2. The angle between the lifting chain and horizontal plane should be larger than 60 degree
You may need to provide lateral spring supports to the skid in the analysis model. Please note: the lateral spring support force shall be checked when the analysis is done. The analysis should be double check if there is significant forces in the spring.
Hope this help.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
what do you think about modeling lifting chains as cylindrical bars and then assigning LINK 180 element to that four cylinders - with tension only propertie and then fixing them in common intersection point.
Problem is I don't know how to write that command. I know how to add it but I don't know correct syntax :/
I am using ANSYS Workbench as GUI not "pure" ANSYS APDL.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
link: http://www.xansys.org/forum/viewtopic.php?p=93490&....
Also from Workbench help verification manual VM31. The basic procedure is to draw line bodies in
DM and then add a command object under each line body defining the element to be 180.
Can someone clarify why using link elements instead of spring elements in this case is a better option?
In my understanding, both have stiffness only in the axial direction so the results will be similar.
Using link elements requires a lot more work due to writing command objects and defining point-surface
contact to lug inner surface.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
What would be approach if I import my geometry in STEP format (Done in some 3d softvare for example). How can I then define COMBIN14 elements ? How can I draw line bodies (I will figure how to add command object). Or there is some other approach on this.
Thank You so much for information and patience. It is nice to have persons that are ready to help in this branch - very valuable infos.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
end is the inner surface (or appropriate part of it) of the lifting lug. Springs elements do not require line bodies where as link
elements do.
To draw line bodies (in DesignModeller) you have many options. Either you can draw a sketch of line and then transform it to line body or you can create a line between two points. The basic setting for is that line bodies are meshed with BEAM188 elements. This is why, if you would use link
elements, should create a command object.
I am sure you will find a tutorial how to create spring elements in WB Mechanical somewhere.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
after importing step file you can do any operations in DM.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
ET,matid,LINK 180 (part LINK ans 180 are without space but if I leve it with space forum adds link :P)
KEYOPT,matid,3,1
SECTYPE,matid,LINK
SECDATA,area
Also I have figured out how to add spring element. Now I am trying to cope with data that I need to define there :)
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
in DM even though in Mechanical it is defined again in the command object (SECDATA). If I didn't do that there was
a question mark next to the body.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
I have uese Body-Ground Scope, and placed my springs. But when I run analysis springs are not at the initial location, and model is deformed with large deformation. :( Model deforms sideways not in direction in which force is acting.
When I setup my LINK 180 try I get this error:
If one or more parts of the model are held together only by contact
verify that the contact surfaces are closed. Also make sure that
there are constraints (or friction) in the sliding direction even if
no load is applied in that direction. You can use the CNCHECK command
to check the initial contact status in the SOLUTION module.
Seams I am not constraining it well. I have created two bonded regions between lug inner surface and link 180 element and fixed link elements in
their intersection point but still this error is present.
RE: ANSYS Workbench - Spreader - Lifting simulation (Stress)
You should not see horizontal movement if both geometry and loading are symmetrical.
In case of horizontal movement, you can add a constraint to prevent it. In that case you should
check the force reaction of that boundary condition. The force reaction should be insignificant
compared to the loading.
Using LINK 180 element poses many problems. As you can see from VM31, a small initial strain
is input to give some initial stiffness. Also large deflections are activated. In order
to get the elements to work in your analysis, you might have to do the same. Also
the contact modelling might be problematic.
I suggest you to send the model to your local Ansys provider. They are usually really
resourceful when it comes to implementing command objects and new elements
to Workbench. Also the before mentioned xansys mailing list is a good resource.