

September 14, 2018 at 1:44 pmthanhttdtSubscriber
Hi everyone,
I do analysis for crane pedestal by using ansys, but I get some trouble while model and apply load. Could you please take a look and give me some advice
1. How to apply load SWL (safety working load)? I mean, is it necessary to model all crane's pedestal, crane's cabin, crane's boom and apply load at the top end of crane's boom Or we have another way to apply this load. Is remote force suitable to apply this load?
2. How to model a structure to act as a wire?
Thanks in advance,

September 15, 2018 at 3:53 ampeteroznewmanSubscriber
Hello,
To analyze the pedestal of the crane, you have to model all the load carrying parts of the pedestal.
You can simplify the boom to a line body and mesh it with beam elements, just make sure the total mass of the boom equals the mass of the line body. You do this be defining a custom material and adjusting the density of that material until the mass of the line body equals the mass of the boom.
You don't have to model the cabin, only the structural plates that surround the cabin and carry the load. You have to include the weight of all the nonstructural parts in the pedestal. If you have an estimate for the weight of the cabin, you can add that as a Point Mass, supported by appropriate parts of the structure. The total mass of the model should equal the total mass of the crane. You can customize the density of Structural Steel to make up the missing mass in the total for the model when compared with the actual weight of the crane.
1. For the SWL, use a vertical force in Newtons of Mg where M is the SWL in kg and g is 9.8 m/s^2
2. Use a Spring Element to represent the wire from the end of the boom to the top of the pedestal. You can estimate the spring rate from the wire properties, but it's not critical, it just affects how far the boom droops.
You have to turn on Standard Earth Gravity as a load in your model to have the weight of the parts be included.
Regards,
Peter

September 16, 2018 at 4:17 pmpeteroznewmanSubscriber
You might benefit from watching a video on using mesh connections to put a sheet body model together.
It uses a Crane Boom example.
Below is a video on using springs as cables to support a boom.

September 18, 2018 at 2:43 amthanhttdtSubscriber
Hi Peteroznewman,
Thanks for your kind support,
If I model the pedestal only and apply force like below, do you think that it can be the same like real working condition
I use fix support at A and B (as the connection between pedestal and decks)
Acceleration C is a gravity (selfweight of pedestal),
Foundation load D is the total cabin's load, I put this force at the red surface
Regarding to SWL, I change this position from the top end of crane's boom to the red surface, so that at the red surface there are a force F = SWL and the moment M = SWL*Boom_Length
For the weight of the boom, I will do the same as the SWL (I don't put it here)
As you said, wire just need when calculate the strength of boom, so I will neglect it in this case
Could you give me any comment
Thanks in advance

September 18, 2018 at 4:23 ampeteroznewmanSubscriber
Between the Pedestal and the Cabin/Boompivot assembly, there is a massive bearing to let the Cabin/Boom rotate about the Pedestal. I think you have correctly drawn the Free Body Diagram for the forces going into that bearing at the top of the pedestal if the winch that lifts the SWL is in the cabin. But if the winch is below deck and the cable goes down the center of the pedestal, then there is an additional down force of SWL. The pedestal has to support the SWL at the end of the boom AND the SWL tension in the cable. If the winch is in the cabin, the tension in the cable is an internal force that does not add to the forces going through the bearing and into the pedestal.
If you want to limit your analysis to just the Pedestal, then when you include the down force of the mass of the boom and the moment for the distance to the boom center of gravity, you will have a representative load.
I expect high stress where the pedestal meets the two decks. You can consider moving the fixed support further away from the pedestal and modeling some of the connection between the pedestal and the two decks so the peak stress in the model is not at a fixed support.
Regards,
Peter

September 22, 2018 at 10:57 amthanhttdtSubscriber
Hi Peteroznewman,
Thanks for your support, I will seperate boom and calculate reaction force at the connection between boom and pedestal, and tensile force in the wire as well.
And as you mentioned, winches are stored in the cabin.
Do you think my analysis is ok?
Thanks in advance

September 22, 2018 at 11:20 ampeteroznewmanSubscriber
Those a good clean Free Body Diagrams. You will do sum of the moments about the boom pivot to solve for T_wire, and then sum of the forces in X and Y to solve for the R_boom force components. Your analysis is okay.
Regards,
Peter

September 24, 2018 at 3:16 amthanhttdtSubscriber
Thank you very much
Best Regards

 You must be logged in to reply to this topic.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Ansys Blog
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
 Saving & sharing of Working project files in .wbpz format
 An Unknown error occurred during solution. Check the Solver Output…..
 Understanding Force Convergence Solution Output
 Solver Pivot Warning in Beam Element Model
 Colors and Mesh Display
 How to calculate the residual stress on a coating by Vickers indentation?
 whether have the difference between using contact and target bodies
 What is the difference between bonded contact region and fixed joint
 The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
 User manual

2600

2086

1317

1108

459
© 2023 Copyright ANSYS, Inc. All rights reserved.