Discussion Groups

## Simulation Mechanical and Multiphysics

Member
Posts: 5
Registered: ‎05-22-2012

# Steady state simulation between rail and wheel. How to set point/ line contact?

998 Views, 8 Replies
02-20-2013 06:13 AM

Hi Everybody,

I was trying to find solution to my problem within this forum, but unfortunatelly I didn't find one, if you already saw similar problem, please provide the lik to the subject.

It is my first use of Autodesk Simulation Multiphisics 2013, so I am asking you for some patience with me . My objective is to run steady state simulation of contact between wheel of the train and a rail (the results that I am looking to obtain are: are values of normal stress, shear stress and size and geometry of the contact area). My parts were designed with aid of Autodesk Inventor  2013. I get results with no match to reality. First: where wheel has it's original curvature (point contact), Second: where only profile of the wheel is used but it is not "round", but straight (line contact). Hope that you understand what I mean.

What I was expected to get is elliptical contact shape area with maximum stress values in the center of the ellipse (point contact) and linear contact with maximum values of stresses on the contact line. What I get instead is this... (see attachments). Please let me know how can I solve this problems.

All the best,

Joanna

Valued Mentor
Posts: 498
Registered: ‎08-30-2012

# Re: Steady state simulation between rail and wheel. How to set point/ line conta

02-20-2013 11:41 AM in reply to: joanna.kuszczak

Hi Joanna,

Here are my suggestions of what you should be doing. You may already have these features -- it is hard to tell from the images.

1. The mesh needs to be very fine at the contact area -- much finer than the expected size of the contact ellipse. So if the ellipse is expected to be 5 mm by 3 mm (just making up numbers), the mesh size should be around 1 mm. Use refinement at the contact area. (Perhaps split the surface of the wheel and rail in Inventor around the contact area, and then specify a surface refinement.)
2. Use either "Nonlinear > MES" or "Nonlinear > Static Stress" as the analysis type. (One of the images appears to be linear static stress. I think it will be very hard to get the results you want with an automatic mesh in linear stress.) If using static stress instead of MES, it is helpful to make sure that all of the parts are statically stable; this makes it easier to converge. You may need to use some "weak" truss elements to make a statically stable wheel in the vertical (Z) direction.
3. Use surface-to-surface contact between the wheel and the rail.

Note that you could cut the CAD model in half (plane parallel to YZ plane through the center of the window) and use symmetry to reduce the size of the analysis.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Member
Posts: 5
Registered: ‎05-22-2012

# Re: Steady state simulation between rail and wheel. How to set point/ line conta

02-21-2013 06:48 AM in reply to: AstroJohnPE

Thank You so much for the reply John.

1. I was using mesh refinement of 0,8mm for the most critical surfaces (Expected ellipse of contact around 4x5mm, received analiticaly). What do you exactly mean by

AstroJohnPE wrote:
Perhaps split the surface of the wheel and rail in Inventor around the contact area, and then specify a surface refinement.

Are You suggesting that I should delete point-to-point constraint in Inventor and just ground both components? Might it resolve the simulation?

2. I used Non linear> Static Stress for the previous simulation. Tried MES with Non linear material model analysis type as well. I set type elements for both parts for "Brick" after reading your post I changed wheel element type for "Truss" (Material model: Curved, Cross-sectional area:3mm)

3. I set the contact as (Default:Bonded) and specified the planes in contact as Surface-to- Surface.

The same problem is repeating with this settings.

Valued Mentor
Posts: 498
Registered: ‎08-30-2012

# Re: Steady state simulation between rail and wheel. How to set point/ line conta

02-21-2013 09:28 AM in reply to: joanna.kuszczak

Hi Joanna,

Your mesh looks fine enough from what I can see, so my suggestion about splitting the surfaces is not necessary. (But I have tried to explain it in the attached image. Instead of using refinement points, I was suggesting using a refinement surface. But you would not want to refine the entire top surface of the rail or the entire perimeter of the wheel. You would want to split those surfaces so that there is a small region around the contact location where you specify the refinement.)

Also, the element type for the CAD parts must be brick elements (or tetrahedron elements if you had selected that type of mesh). In a static analysis, it is not always safe to depend on contact to prevent the wheel from moving an infinite distance. For example, at the first time step, the force of F causes the wheel to accelerate and move to infinity. The software only sees that the wheel is not near the rail, so it cannot possibly be in contact! It is not always smart enough to detect that the wheel has passed through the rail. So by adding one or two truss elements in the vertical direction, the force F causes the springs to elongate 1000 mm. The software detects that it is within range of the rail, so it checks whether contact has occurred. It determine that it has, and that the wheel has passed through, so it does another iteration where the contact is considered. The truss elements are two lines drawn in the model after meshing the CAD parts. This is also shown in the attached image.

One thing to check is the reaction force. If the wheel is making contact over the entire area (reaction force is not 0), then the contact is working, and something else is causing the ring of high stress.

If you are still unsure about the results, you may need to create an archive of the model and attach it to a reply. Please see this description for creating and posting the archive.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Member
Posts: 5
Registered: ‎05-22-2012

# Re: Steady state simulation between rail and wheel. How to set point/ line conta

03-21-2013 11:11 AM in reply to: AstroJohnPE

Hi,

I created Part 3 consisting of two lines as was shown on the picture attached to the forum. They were specified as Surface 1 and 2 of Part 3. Although some error is occuring when I wanted to check the model/ run simulation.

Model [C:\Users\...ds] opened for generating contact surfaces...
No general impact plane
Error: Bad data for element[24623] in group[1]!

Probably I have some error in determination of proprieties of this part. I'm not sure exactly where. Element type:truss, with crosssectional area:1, material model: linear (the same error occures with curved/ nonlinear). I specified material as customed, mass density:1, young modulus:1.

I am attaching an archive to this post to facilitate comunication and understanding. Thank You for the support!

Joanna

Valued Mentor
Posts: 498
Registered: ‎08-30-2012

# Re: Steady state simulation between rail and wheel. How to set point/ line conta

03-22-2013 03:49 PM in reply to: joanna.kuszczak

Uh, the zip file only contains three files from the .mod folder. Please open your model in the software and use the "File > Archive > Create" command. After it is done, change the extension of the file from .ACH to .zip, and then post that to the discussion group.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical
Member
Posts: 5
Registered: ‎05-22-2012

# Re: Steady state simulation between rail and wheel. How to set point/ line conta

03-25-2013 11:08 AM in reply to: AstroJohnPE

I managed to run simulation with the specified parameters, unfortunatelly the results looks similar to the ones that I obtained at the beginning- the highest stress values are out of the centre of ellipse contact. I'm sending a link to the archive file, as the file is too big to attach it within the forum:

Regards,

Joanna

Valued Mentor
Posts: 498
Registered: ‎08-30-2012

# Re: Steady state simulation between rail and wheel. How to set point/ line conta

03-26-2013 08:30 PM in reply to: joanna.kuszczak

Hi,

I think -- but cannot confirm my suspicion -- the mesh is too random. The un-even surface mesh has probably lead to an uneven interior mesh (odd shape tetrahedron elements, distorted 8-node bricks, and so on), and the slight differences in the stiffness of each distorted element gave the unexpected results.

The attached images look much better, and I did not make very many changes to the model.

1. I removed the constructure vertex that was on the contact surface.
2. I remeshed the model but did not change any settings.
3. I changed the Element Definition for the truss elements to "Linear" material model.
4. I changed the material properties to "GE PlasticS NORYL ....".
5. I did view the settings for the surface contact, but I think that I did not make any changes.

I just noticed that fully fixed surface constraints were applied to the truss elements being used as springs to provide some stability. Of course, this puts a fullyfixed constraint on each end of the spring, so it cannot move at all. Worse, it is preventing the wheel from moving. Oh well, time to go to bed.

I think the slight distortion of the stress pattern on the rail is due to distorted elements just under the surface. The only way to get a perfect mesh is to create the mesh by hand which is actually easy in this case.

One final thing: the analysis is literally simulating a small "pie" section of wheel cut out of the larger wheel. That is, with no symmetry boundary conditions, there is no material resisting the sides of the wheel from pushing out (or in). Applying symmetry constraints to the small pie section is not correct either because that would be like having the wheel making contact every N degrees.

John Holtz, PE
Mechanical Engineer
Pittsburgh, PA

16 years experience with Simulation Mechanical