Log In

Come Join Us!

Are you an
Engineering professional?
Join Eng-Tips Forums!
  • Talk With Other Members
  • Be Notified Of Responses
    To Your Posts
  • Keyword Search
  • One-Click Access To Your
    Favorite Forums
  • Automated Signatures
    On Your Posts
  • Best Of All, It's Free!
  • Students Click Here

*Eng-Tips's functionality depends on members receiving e-mail. By joining you are opting in to receive e-mail.

Posting Guidelines

Promoting, selling, recruiting, coursework and thesis posting is forbidden.

Students Click Here


Dear experts, I am a beginner wi

Dear experts, I am a beginner wi

Dear experts, I am a beginner wi

Dear experts,

I am a beginner with ANSYS Mechanical. I worked a lot in CFD with FLUENT, CFX, ANSYS ACT (acoustics)...so I am familiar with the GUI and the Workbench environment.

I am trying to simulate a load on a hinge with static structural analysis. Load of 500 kg, applied on an 50 mm long face located in the top of the hinge. Gravity is also included in the model. The part is fixed using Fixed support condtion.Please find attached a picture of the conditions imposed.

The dimensions of the part are around 24 cm long, 9 cm high and 0,3 cm thick.

I have information about the deformation for several loads.. What I did and will try to do (in a second step) is:

1. First I did a linear elastic analysis with several steps (increasing the load according to experiments) and compared the deformation results of the zone where the load is applied with test results. This provide good agreement between both results (FEM and measurements) except where larger deformations occur (around more than 400 kg where plasticity clearly appears). It must be noted that the tests are performed as follows: load applied, discharge, measurement. Without changing the part, load is increased and applied again, then discharge and then measure again. They repeat this process until deformation is relatively large (around 5 mm)

2. Having this in mind, I will try to include non linear effects to the model. I will do 8 steps (load:150 kg, load: 0 kg, load:250 kg, load:0 kg, load:375 kg, load: 0 kg, load: 500 kg, load: 0 kg. After each discharge, I will compute deformation of the zone where load is applied and compare with tests. I think this should give better aproximation in plastic region.

What do you think about this methodology? Do you think is a better approach due to the way experiments are carried out?

I think I will have to face with several problems in the non linear approach...sometimes I have seen error messages when switch non linear effects to "On"

I am playing with bilinear isotropic hardening and bilinear isotropic hardening. I am experiencing several converge issues (usually ANSYS tells that there are several highly distorsed elements...).

I think the good way to this (and follow closely the tests) is to do a load-unload including non linear effects and large deflections. But it tooks too much time to compute and the most of the time it does not converge...

I am using standard values for steel in isotropic/kinematic hardening. Do you think this is enough? What other things can I try? I am now using mostly hexaedral meshes.

The experiment measures the displacement where the load is applied (on a given surface). I try to track the same by checking directional deformation in suitable axis.

I am trying the adaptative meshing during runtime, but sometimes it doesn't work.

I am also trying to introduce multilinear s-s curve for stainless steel.

A few more info about my problem (really stuck on it). By reducing the mesh size (and temporaly suppresing adaptative meshing) I have managed to make it run a couple of times. Here I summarize what is happening:
1. The computation is higly inestabe, and using the same settings sometimes it converges, sometimes it doesn't.
2. Usually, when the simulation converges without errors, the results are not corresponding with tests (for a load of 500 kg we should expect a deformation of the surface where the load is applied of about 4-5 mm). The results are showing much higher deformation (around 20-40 mm). It seems that it lose the path during intermediate steps...
3.I tried to introduce s-s curve in order to be more accurate with material description, but using it (multilinear kinematic or isotropic), simulation crashes. I don't know if I should provide s-s values beyond the typical ones (true stres-true strain available in the state of the art, I mean, s-s clearly in the plastic zone...). If so, where can I find this values (curve or table) for example for stainless steel?
4. As I mentioned, the tests are carried out as follows: apply load, then remove it, then measure deviations from original position (in mm) where load is applied. So, I understand that in order to reproduce this, I have to consider non linear effects (the lower load they used is 100 kg which produce a deformation of 0,1 mm), in two steps: load and unload, and check what happens with deformation in the second step.

The elastic lineal approach give more or less accurate results for low loads (probably in the elasto-plastic region), but when plastic deformation occurs, lineal elasticity dramatically underestimate deformation, but considering the non linear effects it overestimate deformations a lot or even crashes.

I do not know what to do honestly...

Thanks for the support.

I include info of several runs (solver output) and pics of eng.data and the error I am usually obtaining.



RE: Dear experts, I am a beginner wi

How much calculated deformation value differs from measured with maximum load (linear analysis)? Please share picture of the
stress distribution of this model (where is plasticity occurring?). There are two types of nonlinearities
you _possibly_ need in your model: material and geometrical. You could first just try modelling a plastic material
and set large deflections OFF. Also use adaptive meshing as the last resort.

Also what is the purpose of the simulation? You want to know how close the part is to breaking with the maximum load?


RE: Dear experts, I am a beginner wi

You are loading with a force on a plastic material. If your tangent modulus is small (or zero) convergence with force loading can be difficult. Try loading with a deflection. This is generally more stable. You can get a reaction force to determine the load if need be. Also, be aware that material will yield at the the first data point in the MISO curve, so if you try and fit the miso curve too closely to your data, you may be understating your yield strength. Lastly, you need to start with a fine mesh with good element shape. For analysis options, I would set auto time stepping to on, and initial to 10, min to 5, and max to 80. In output controls, make sure Store Data Results is all time points so you can look at your last converged substep.

Regarding stress strain date, the ASME pressure vessel code (Sect VIII Div 2 Annex 3-d) has what you need. Other sources are the Aerospace Structural Metals Handbook and the MMPDS Handbook.

Rick Fischer
Principal Engineer
Argonne National Laboratory

Red Flag This Post

Please let us know here why this post is inappropriate. Reasons such as off-topic, duplicates, flames, illegal, vulgar, or students posting their homework.

Red Flag Submitted

Thank you for helping keep Eng-Tips Forums free from inappropriate posts.
The Eng-Tips staff will check this out and take appropriate action.

Reply To This Thread

Posting in the Eng-Tips forums is a member-only feature.

Click Here to join Eng-Tips and talk with other members!


White Paper – Your Construction ERP RFP Checklist
Selecting business software for a medium to enterprise-sized construction concern is extremely challenging in large part because most enterprise resource planning (ERP) suites originated in the world of repetitive manufacturing and are therefore a poor fit for a project and asset-centric business. However, midsize to large contractors need the predictable, auditable processes that ERP delivers. Download Now

Close Box

Join Eng-Tips® Today!

Join your peers on the Internet's largest technical engineering professional community.
It's easy to join and it's free.

Here's Why Members Love Eng-Tips Forums:

Register now while it's still free!

Already a member? Close this window and log in.

Join Us             Close