Sling Tension - lifting analysis

[johnster100]

Hi,

I've currently running a lifting analysis on a large steel structure. The model has 4 lifting eyes and these are linked to the crane hook point using rigid connectors (all DoF free except the vertical direction).

The model creates displacements which look realistic but I would like to check the tension in slings to see that it matches with those which I have calculated.

Is there a way to extract this value from the model or the Nastran output file?

I've attached a simple model which shows the model setup:

thanks,

John

[johnster100]

Hi,

I've currently running a lifting analysis on a large steel structure. The model has 4 lifting eyes and these are linked to the crane hook point using rigid connectors (all DoF free except the vertical direction).

The model creates displacements which look realistic but I would like to check the tension in slings to see that it matches with those which I have calculated.

Is there a way to extract this value from the model or the Nastran output file?

I've attached a simple model which shows the model setup:

thanks,

John

[John_Holtz · Accepted solution]

Hi John ( @johnster100 )

I think the force in the rigid connectors is not available. 

Fortunately, you should not be using a rigid connector anyway, so the proper way to do it will provide the force in the sling. See this article: How to perform analysis of lifting frame in Nastran. You will then be able to look at the force or stress result in the rod elements. (You may need to activate the Force output by editing the analysis type, but I do not remember all of the details.)

[John_Holtz · Accepted solution]

Hi John ( @johnster100 )

I think the force in the rigid connectors is not available. 

Fortunately, you should not be using a rigid connector anyway, so the proper way to do it will provide the force in the sling. See this article: How to perform analysis of lifting frame in Nastran. You will then be able to look at the force or stress result in the rod elements. (You may need to activate the Force output by editing the analysis type, but I do not remember all of the details.)

[johnster100]

Thanks for that John.

What is the problem with using the rigid connector? I find the rods annoying to use as these elongate themselves. This  makes measuring the actual displacements in the structure itself difficult, i.e. you have to subtract the rod elongation.

thanks,

John

[johnster100]

Thanks for that John.

What is the problem with using the rigid connector? I find the rods annoying to use as these elongate themselves. This  makes measuring the actual displacements in the structure itself difficult, i.e. you have to subtract the rod elongation.

thanks,

John

[John_Holtz]

The main problem with the rigid connector is they do not provide a force which is one result that you wanted. You can increase the area of the rod elements to simulate a "rigid" wire.

The other problem with the rigid connector is that it prevents the lift points from moving relative to each other. The rod elements have a tension which puts the frame into compression, and therefore the lift eyes can deform toward each other. This is more realistic than the rigid connectors.

[John_Holtz]

The main problem with the rigid connector is they do not provide a force which is one result that you wanted. You can increase the area of the rod elements to simulate a "rigid" wire.

The other problem with the rigid connector is that it prevents the lift points from moving relative to each other. The rod elements have a tension which puts the frame into compression, and therefore the lift eyes can deform toward each other. This is more realistic than the rigid connectors.

[wCorreiaHBYAR]

Increasing the area of the rod connectors shifts the system COG and introduces additional unwanted moments which cause large displacements. do we have a solution to this? 

[wCorreiaHBYAR]

Increasing the area of the rod connectors shifts the system COG and introduces additional unwanted moments which cause large displacements. do we have a solution to this? 

[John_Holtz]

The stiffness of the rod is controlled by two things: the cross-sectional area, and the modulus of elasticity. If you are including gravity and that is changing the CG, then don't change the area. Change the modulus!

I do not remember how the rod connector material is entered. Does it use a material in the model, or does it use input on the rod dialog? If it uses a material in the model, then create a material that has no  mass density. Then the CG will not change regardless of how larger or small you make the rods. 

[John_Holtz]

The stiffness of the rod is controlled by two things: the cross-sectional area, and the modulus of elasticity. If you are including gravity and that is changing the CG, then don't change the area. Change the modulus!

I do not remember how the rod connector material is entered. Does it use a material in the model, or does it use input on the rod dialog? If it uses a material in the model, then create a material that has no  mass density. Then the CG will not change regardless of how larger or small you make the rods. 

[djamal.rayane]

hello

help me plz

https://knowledge.autodesk.com/fr/support/inventor-nastran/learn-explore/caas/sfdcarticles/sfdcartic...

this exmple not work for me nastran 2021 !!??

[djamal.rayane]

hello

help me plz

https://knowledge.autodesk.com/fr/support/inventor-nastran/learn-explore/caas/sfdcarticles/sfdcartic...

this exmple not work for me nastran 2021 !!??

[John_Holtz]

Hi @djamal.rayane 

If you zoom in on the joint between the beam elements and the cable, you will see that the cable is not connected to the beam element.

The beam elements are created at the centroid of the cross-section, and all of your sketch lines (for the beams and cables) are offset to one face of the web. Here is what it looks like in the CAD environment:

[John_Holtz]

Hi @djamal.rayane 

If you zoom in on the joint between the beam elements and the cable, you will see that the cable is not connected to the beam element.

The beam elements are created at the centroid of the cross-section, and all of your sketch lines (for the beams and cables) are offset to one face of the web. Here is what it looks like in the CAD environment:

[djamal.rayane]

thank you for your help

I fix connection, but  still have a message in solver FATAL ERROR E5001.

[djamal.rayane]

thank you for your help

I fix connection, but  still have a message in solver FATAL ERROR E5001.

[John_Holtz]

Hi @djamal.rayane 

The problem is the cables are still not attached to the frame. The cables are attached to a sketch point that is not associated with the frame members. In other words, having the endpoints at the same coordinate in space are not sufficient to joint them all together.

This is what you should do so that the cables use the same points as the beams from the frame:

1. Edit sketch 4.
2. Add a point at the top of the cables.
3. Delete the two lines representing the cables.
4. Delete the two sketch points at the bottom of the cables. (I think there were sketch points there. Maybe not.)
5. Repeat those steps for sketch 5.
6. When creating each cable in Nastran, the top end is the point in the sketch, and the bottom point is the point at the end of the frame member, such as "point<7>"@Frame 16208500...". That way, the beams and cables are using the same CAD geometry to define the end point, so all of the elements are connected together.

[John_Holtz]

Hi @djamal.rayane 

The problem is the cables are still not attached to the frame. The cables are attached to a sketch point that is not associated with the frame members. In other words, having the endpoints at the same coordinate in space are not sufficient to joint them all together.

This is what you should do so that the cables use the same points as the beams from the frame:

1. Edit sketch 4.
2. Add a point at the top of the cables.
3. Delete the two lines representing the cables.
4. Delete the two sketch points at the bottom of the cables. (I think there were sketch points there. Maybe not.)
5. Repeat those steps for sketch 5.
6. When creating each cable in Nastran, the top end is the point in the sketch, and the bottom point is the point at the end of the frame member, such as "point<7>"@Frame 16208500...". That way, the beams and cables are using the same CAD geometry to define the end point, so all of the elements are connected together.

[djamal.rayane]

thank you it works 

[djamal.rayane]

thank you it works