# A Tutorial for Creating and Analyzing Cables?

Member

Would someone direct me to a tutorial in creating and analyzing cables? My application is analyzing crane rigging and the structural integrity of lifted assemblies. The simplest lift I would like to analyze is a simply supported beam lifted by two cables extending down from a hook. A more complex lift I would like to analyze would be to lift a steel plate by its four corners. An even more complex lift would be to lift a steel plate by its four corners with another steel plate suspended by its four corners from the first steel plate.

• Member
edited November 2018

I don't know of an existing tutorial but I can work with you on developing the models you describe above.

I understand you want to analyze the effect the cable tension has on the structure.

Can you provide a specific example for the steel plate supported at four corners. What are the dimensions of the plate: Length x Width x Thickness?

How does the cable interface to the plate? Is there a shackle to a hole in the plate or is there a loop of wire around a corner?

How high above the center of the plate is the hook?

Are you only interested in the structure or are you also interested in the cable?

Is gravity and cable forces the only loads on the structure?  What about wind?

Are you interested in the static solution just hanging or the acceleration during the lift-off?

Is the plate flat on the ground or is it resting on some stand like a pair of beams?

• Member
edited November 2018

Thank you, peteroznewman (Peter?), for your quick and inspiring response. Yes, I want to analyze the effect of cable tension on a crane lift assembly. To answer your questions:

The steel plates were idealizations of more complex structures. The first plate, connected to the crane hook via cables, represented an H-pile rigging spreader frame, depicted below. The rigging frame below consists mostly of H-piles with designation 12 x 53 manufactured by Skyline Steel out of A572 Grade 50 steel. The frame is 53 feet long and the long H-piles are 6 feet on center. H-pile flanges are welded (bonded) to H-pile webs, H-piles are welded together, thickening blocks for shackles are welded to H-piles, and for the sake of simplicity, screw pins are welded to shackle hoops, though the screw pins have frictionless contacts with H-piles. If you recommend it, I could very easily model the steel plate we talked about and add some shackles.

I chose 1-3/4-inch Crosby screw-pin shackles, which is overkill for now. I'm good with a 1-inch wire rope for now.

Let's say that the crane hook is 60 feet above the top of the H-pile rigging frame.

I'm interested first in the behavior of the rigging frame; then I'm interested in the behavior of the wire ropes.

The H-pile rigging frame would probably start off on some 7" x 9" x 8' railroad ties.

• Member
edited November 2018

I found a reference to look up what an HP12x53 I-beam looks like, and better yet, if you want to model this structure with beam elements, that section is included in the SpaceClaim profile Standard Library.

What is the correct orientation of the beams?  It's very easy to rotate the beams by 90 degrees.

A beam model is the simplest idealization of the structure, but it doesn't have any detail about the thickening blocks.

It will be necessary to have a solid model of the structure for more detailed analysis.

I put 4 springs, one from each corner to a point 60 foot above the center and turned on gravity. It successfully solved. The center of the frame sags 3.8 inches, the springs, which represent the cables, have stretched so that the corners are down 1.8 inches after gravity turns on.

Regards,
Peter

Attached is an ANSYS 19.2 archive

• Member
edited November 2018

Hi Peter.

I followed in your footsteps and generated the below H-pile rigging frame idealization in SpaceClaim. Generally speaking, I loaded the AISC_HP12X53 beam profile via "Prepare --> Profiles"; created an re-positioned points via "Design --> Point and Design --> Move --> [AXIS] --> XYZ Coordinates"; created beam elements between pairs of points via "Prepare --> Create"; and re-oriented beams via each beam's "Properties".

I'm new to ANSYS; would you please explain via what interface and how you placed springs?

I generated the above H-pile rigging frame assembly in Autodesk Inventor Professional 2019. I am interested in conducting this analysis with that model as well. May I send it to you somehow? Comparing the two model-generation methods, the SpaceClaim method allowed me to load standard geometry, define and redefine points, create and reorient beams between points, all very simply, but my point-redefinition process was very math intensive. Additionally, while the SpaceClaim model is simple, there seems to be overlap at beam junctions and no particularly easy way to eliminate overlap / selectively extrude from a shorter beam. I am grateful for learning about basic modeling in SpaceClaim though. The Inventor method allowed me to draw and dimension a cross section, extrude beam parts, make cuts, and place and constrain parts in an assembly without much math and in a very precise way. Personally, at this point, I prefer the Inventor method, but then again, I'm used to it.

Thanks,

Tom Lever

• Member
edited November 2018

Hi Tom,

A beam model is probably too simplistic for your needs, but it is proof of concept for more advanced models that are built from the solid models that come from Inventor. SpaceClaim may be able to open an Inventor file directly, but if not, you can export an ACIS file from Inventor and open that in SpaceClaim.

The only math I used in the tutorial below was to divide 53 by 2.

Here is the bending moment that I added later.

Regards,
Peter

• Member
edited November 2018

Hi Peter,

I ran the analysis you presented in your video above. Thank you. I now know how to perform a simple static structural analysis of 1D beams in a 3D arrangement sharing endpoints subject to gravity supported by 1D springs. The only issue I had was that I needed to collapse the view of the idealized beams down to lines so that I could select intersection points as connection points for the springs.

I also performed a static structural analysis involving my Inventor geometry subject to gravity supported by 1D springs. Unfortunately, I had to eliminate shackles to I believe bring my ANSYS part number down to 13, because with shackles the part number was 21, even when I tried to transform the Inventor assembly into a single derived part. Any suggestions here? That being said, my 1D springs only attach to single points on the H-piles at the edges of the holes for the shackle pins, and apparently do so via idealized beams, though I can't seem to see them. I assume the first warning below is related to the spring attachments? Any suggestion on further constraining the model to address Warning 2?

The below solution is total deformation. It ranges from 0.36 inches downward at the corners of the rigging frame to 1.0 inch downward at the center of the rigging frame. I suppose this is reasonable. The equivalent stress ranges from 8.7 psi pretty much everywhere to 1.0 x 10^5 psi somewhere. Where is the maximum equivalent stress? I'm not sure how to create a section plane on the Inventor geometry, even after clicking the Section Plane button on the standard toolbar...

I found Young's modulus for 8 x 19 wire rope with fiber core to be 9 x 10^6 pounds per square inch per http://www.hanessupply.com/content/pdfs/wireRope101.pdf, and computed the axial stiffness of the springs to be (1-inch-diameter wire rope cross-sectional area) * (Young's modulus) / (initial length of spring) per https://ccrma.stanford.edu/~jos/pasp/Young_s_Modulus_Spring_Constant.html. The value for the axial stiffness came out to be 9,060 pounds per inch, which was in accord with your 10,000 pounds per inch guess.

Tom

• Member
edited November 2018

Hi Tom,

Well done getting your solid model version running!

Are you using the free Student license?  It has a limit of 50 bodies and 300 faces in the Geometry editors, so that may have been why you were unable to bring in more geometry.

The first warning is telling you that the software automatically did something very helpful. The vertex at the end of the line body actually has the entire cross-sectional area of the profile to hold on to, so the stress is the force/area.  When you pick a vertex of a solid body, the stress would be infinite because the area is zero. ANSYS knows this and so automatically creates a spider web of hidden elements from that vertex to nearby nodes to create an area and have a finite stress.  If it didn't do that, the solution might fail.  You can manually do this to have more control by using what is called Remote Point, and picking the face you want to spread the load over, while generating a single point to attach a spring. With a Remote Point you can move the point to different coordinates.  Or you could just attach the spring to a face instead of a vertex, but then the spring will be at the center of that face and you can't move it.

The second warning is acceptable because you know that you have drawn all the springs to come from a single point. That means the structure is free to pivot about that point with no resistance. That means there is no solution to the matrix inversion. The weak springs that stop the model from twisting around that point allow the matrix to be solved. That is fine because you aren't interested in it spinning.  You could avoid that warning if you separated the four springs and terminated them at four points below the hook instead of terminating them at a single common point, but then you would have to do some math to calculate those four points. Just let the weak springs fix the matrix for you.

You have a plot of Equivalent Stress, there is a flag on the toolbar called Max that if you click it will show where on the part the maximum value is.  If there are multiple parts, the Details window says which part has the maximum values.

After you click the Section Plane button just sketch a line through the model to section it. There are tools to move that line around using the Edit Section Plane button in the Section Plane window. That is the quick way to see the stress distribution inside the part. A more controlled way is to RMB on Model and Insert Construction Geometry. Then RMB on Construction Geometry and Insert Plane.  Define the plane, then you can create a Stress result scoped to that plane.

Regards,
Peter

You can show your appreciation by clicking Like below the posts that are helpful.

• Member
edited November 2018

Hi Peter.

I am using the student version of Workbench. How much would a individual or corporate license be, to the nearest hundred dollars?

I don't seem to be able to add shackles at all given my license restrictions. Given the simplified configuration, the equivalent stresses at the spring / pile junctions seem unresolvably greater than the yield stress of steel. That being said, ANSYS automatically distributing forces at spring / pile junctions across the related pile cross sections seems more charitable to the model than asking ANSYS to distribute forces over the hole faces using a Remote Point, so I won't use the Remote-Point option right now.

I will also accept ANSYS's introduction of weak springs to keep the system from rotating about the crane hook.

The maximum equivalent stress indeed does seem to be exactly where a spring meets an H-pile. Section-Plane-ing might be interesting if I can get the plane to be precisely through the cross section containing the spring / pile junction point, but I think I'm good for now.

I feel like I've reached a conclusion point regarding my static structural analysis of a lifted H-pile rigging frame in a student version of ANSYS. Except, how would you apply a static, uniformly distributed wind load? Another question: In real life, do wire ropes behave in a dynamic situation as very stiff springs?

• Member
edited November 2018

Hi Tom,

Contact the ANSYS Sales department to get a quote. There are also special offers for small businesses through the ANSYS Startup program. The commercial licenses start with Mechanical Professional and you will want to add a SpaceClaim (or DesignModeler) license to that. You can do Modal analysis in Mechanical Professional but it won't do Transient Dynamics, which is included in the Mechanical Premium (which comes with a premium price tag!).

You can go a little further in the Student license by creating a "Breakout" model, sometimes called a "Detail" model.   Your overall system model using beams solved for the tension in the cable.  In Inventor, use two planes to cut through the solid model beams 3 feet back from one corner where the shackle attaches at the corner. Hide all the rest of the solids and bring that one corner into SpaceClaim and into Mechanical. On the short beam, the 3 foot cut is at the center plane, so create a Symmetry Region on that, which means zero displacement normal to the plane. On the long beam cut face, create a Remote Point on that face, and relocate the Remote point 23.5 feet back and hold that remote point fixed.  Now you can select the faces the shackle contacts and apply a force along the line of the cable, with the magnitude of tension in the cable.  The corner will flex up much like the beam model did, but you will be able to evaluate detailed stresses in the welded joint between the beams, with any reinforcements welded in.

To the question of uniformly distributed wind load, that would be to select all the faces that face the wind and apply a force.

In real life, wire ropes behave exactly like very stiff springs.

Regards,
Peter

• Member
edited July 2019

Hi Peter,

Why did you choose Body-Ground inside Spring configuration?

When you include the 4 'springs cables', ansys understand that the model is supported in the point where the connections touch each other (point 3, 60, 26.5)? That is the reason you didn't include any support in the analysis?

If based on this analysis I would like to size the cables, how can I get the force acting on that? Do I need to have an user define function or some Spring Probe?

Regards.

• Member
edited July 2019

Body Ground means that the spring comes from a point on the corner of the body to a point that is fixed (ground) at coordinates above the frame. The purpose for the analysis was to compute the deformations in the object being lifted. There was no interest in the supporting structure, so no need to model that.

You use a Probe to extract the force in the spring.

• Member
edited July 2019

Peter, thank you for your clarification!

One last question. Taking as an example the lifting structure of the tutorial, if I took off 2 slings (the ones in the diagonal) and substitute them for 2 remote forces pointing to the same link point [3, 60, 26.5], how is it possible to do it?

I'm asking you this because when I try to define the direction of the force, I just have the point in the structure, but don't have the physical point [3,60,26.5].