Crane structure analysis

[Anonymous]

Hi,

i am trying to do a simulation of the stresses that occur in the frame of a crane on board of a Swedish military submarine rescue ship. (They have problems with cracks in the top flanges.)

I have used the model in ADAMS previously, but i really want the stresses that occur in the structure and i also want to do some fatigue calculations, and since i have used Inventor to do the whole model i thought it would be easy to simulate it in Autodesk Simulation.

One of the problems is when i try to do a static analysis, i get problems with the mesh. I have to make a whole new model because it complains about all the small bolt holes in flanges not being "watertight". This is not a problem in ANSYS, where the model meshes perfectly. I am guessing that Simulation does not make the mesh fine enough around small geometries, the only way of solving this is by doing a super fine mesh, but doing that kills the performance, i get about 0.1 frames per second and i can imagine that the simulation time would be epic. Is there any way of solving this?

And I am able to set parts that are of no interest (and that shouldn't deform) to Rigid, but Simulation still meshes these parts for some reason, is there any way of shutting this off?

The most important for me is to do a dynamic simulation, so i use MES with Nonlinear Material Models. But in this analysis type you cant choose rigid for some reason, meaning that it has to mesh _everything_, this slows down the performance drastically, making it unbearable to rotate, zoom in and further examine the model. So i really need to find out how to make parts stiff (but still able to move). Furthermore i can't seem to figure out how to make parts rotate/move around a certain axis. 😞

Here is a picture of the crane IRL.

Here is the model i have created, with the "pitch plate" and "roll plate". They have their center of rotation where the ship has its center of rotation. It is supposed to pitch +-4 degrees with a period of 13 seconds and roll +-10 degrees with a period of 9 seconds. 

I have inculded the whole model as a step file.

All help is greatly apreciated!

[S.LI]

What a beautiful model!

Mesh is definitely necessary in ASIM MES, even for rigid parts (called kinematics element in MES), since mesh is used to describe the body geometry for contact etc.

To rotate a body in ASIM MES, there are several ways:

1.) manually adding beam elements, and applying rotational loads to beam nodes.

2.)applying remote moments.

[Anonymous]

Thanks for the rapid response!

I still have problems with the mesh though. The model meshes perfectly in ANSYS, but in Simulation Multiphysics even though the mesh is VERY tight i still get problems with "not watertight solid". Making the mesh size even finer solves some of the problems, but the impact on performance is so significant i can't imagine how long it would take to do an actual analysis.

Isnt there some intelligent meshing feature that adopts the mesh size to the geometry?

I added the model in my previous post, so please feel free to mesh it. 🙂

[S.LI]

What is the your ASIM version?

Did you adjust mesh sizes for the entire model, or part by part?

In my machine, default setting works fine except for part 2. So I adjusted the meshing size for part 2 only to 50%, then mesh is all right.

The model is too large to be attached here. So only a picture is uploaded.

[Anonymous]

Build 2012.01.00.0017 

(Time-limited) 2012 - STUDENT VERSION

I set all the settings to default now, no specific mesh size on any part, 100% on all parts. (Didn't set Element Type or anything, just generated the 3D Mesh.)

Observe the super-fine meshing on the FOOT-part (part 5 and 6 in the model), i don't understand why it does such a fine mesh. Its a pain to move around the model when the mesh is so intricate, it is a huge performance hit and its on a part that i don't even care about (it will be a rigid body).

[Anonymous]

So i reset everything, deleted the old data, opened the .stp again but this time i set Element Types on all parts first. The parts that i want to be rigid was set to 3-D Kinematic and the rest was set to Brick. Is this correct?

Anyway, meshing everything at 100%, no specific mesh to any part gives the following mesh error:

(Still extremely fine mesh on Part 5 and 6 for some reason.)

I set the mesh size for the Rollplate to 50% and meshed again (why does it have to re-mesh everything?), the Watertight problem was gone on that part but got a new watertight problem instead:

Why didn't it find this problem when i meshed previously? I don't understand.

[S.LI]

To go through these issues one by one is painful. 😞

If possible, please try the last ASIM2013 beta (I think it should be beta2), which worked well on my side.

I believe our meshing team has done a lot of work since 2012SP1.

Please let us know if 2013 is helpful.

[Anonymous]

Yeah, trust me, been trying to get this to work for over a week now, i know its painful. 😞

ASIM is soooo much more user friendly than ANSYS, i really want my stuff to work in ASIM as the tutorials are great and the support (you guys) is awesome. Its just so frustrating to get stuck at just trying to mesh the model.

I have found the place to download the beta, https://beta.autodesk.com, but i can't log in with my account. I am an Autodesk Student Expert but i guess you have to have some kind of special account to be able to log in and download from there. 😞

[John_Holtz]

Hi Konrad,

I think it is time to get realistic about what you are trying to accomplish. Perhaps you have already done a simplified model to confirm that your ideas for the model setup will work. For example:

1) Are there any parts that pivot or move? How are you going to do that?

2) How are you going to setup the pitching and rolling motions?

Until you know how to do those, don't spend your time trying to mesh the model. Also,

3) You indicated that you were interested in the top flange where cracks are appearing. I do not know where the top flange is located, but do you need to model everything just to investigate the cracks? Perhaps you need to model just that area for the cracks where you want to have a finer mesh, and a different model of "everything" if you want to analyze the whole structure.

4) I was having problems meshing the "pitch plate". It is so thin (10 mm) compared to its overall size (50000 mm long!) that the mesher couldn't handle that aspect ratio (5000:1). It would be helpful if you could change the dimensions. For example, if you are assuming that it is rigid, then make it 1 m by 1 m by 0.1 m.

5) In your image of the flange with all of the bolt holes, how are you going to analyze that connection? Unless you are going to use the bolt hole, take the holes out. (Most engineers would probably assume that the bolts are strong enough that the two flanges act as one, and therefore eliminate the holes and "glue" the two flanges together. The software refers to that as Bonded contact.)

6) What contribution do the letters "55TE SWL" in the part Top_Shrinkwrap provide to the analysis? Other than creating a distortion to the mesh, I doubt they add any value.

7) Does the floor grating in the part VAGGA need to be modeled in that amount of detail? Is it being used in real life to provide necessary stiffness to the structure? In other words, is it welded solid in real life so that it flexes as a solid? Or is it spot welded together (or maybe not even held down)? If you keep the grating, are you meshing it with a fine enough mesh to accurately predict the stiffness? It might be better to replace it with a solid plate of equivalent stiffness (and reduce the number of surfaces from 2333 to a few hundred).

In other words, SIMPLIFY the model.

When you are ready to mesh the model again, deactivate the option "Mesh > Mesh > Use VCAD" and see if that produces a better mesh for you.

[Anonymous · Accepted solution]

Thank you for your reply!

I will try to simplify the model as you say and try again. Since i don't care about the part "vagga" i will replace it with just a square weight.

I will try to do a small version of the flange-area, i am guessing i just need to apply the forces to the surfaces i "cut" as remote forces? That way i will get all the forces and moments acting on the flange.

The reason i did the whole model was to see where the stress concentrations are located, if there even are any stress concentrations around the flange or not. Since the whole structure is bobbing along with the rest of the ship i can't just do a static analysis, I want to include the inertial forces that act on the crane (hence i have included the pitch and roll plates to just have a correct roll and pitch center. Furthermore i would like to do a fatigue analysis, to see if the ship motion induces fatigue damage to the flanges causing them to crack, or if the cracks occur while lifting the rescue submarine (which weighs 52 Metric Tonnes).

Thank you for your fast response, much apreciated!