AnsweredAssumed Answered

Static simulation fails while real product succeeds

Question asked by B. Bijl on Dec 5, 2018
Latest reply on Dec 6, 2018 by Bill McEachern

Like • Show 1 Like1
Comment • 27

Dear Forum,

I'm running into a problem using solidworks simulation. To be very clear I'm not a professional using static simulations. I know the basics.

A coupler plate for some machinery we have here needs to lift 2.5 Tons. To get a proper certificate it needs to lift up to 200%, meaning 5 Tons.

It did this without any problems or deformations in the product. But when I try to simulate this in Sw, it shows that it should fail. The biggest stress areas Sw shows are logical though.

Attached is the product.

Below some screenshots:

The hoist ears are welded on the bend plate. Can this be the issue?

I would be very happy to get some advice from you guys on my problem.

Cheers,

Boris

Attachments

Coupler.zip3.1 MB

No one else has this question

Outcomes

27 Replies

Dave Bear Dec 5, 2018 8:40 AM
Mark Correct
Correct Answer
Hi JM Van Oossanen,

Okay, just a couple of things to point out as a Rigger which I have past experience in.

Why would you have this 'cut-away' present as it will only present itself as a weak point in the overall lifting structure?

Is the hole between the lifting fixture necessary as it appears that the corners are what may be showing the weakness?

But most importantly, what happens if you try your design with your lifting fixture running parallel to your lifting lugs?

Or, better still.....................
Just as a side note, although it does happen, a certified lifting device will very rarely have any holes, cut-outs, perforations or such unless they are for a specific purpose.

Just some ideas above for you to ponder.............

Dave.
Like • Show 4 Likes4
Actions
- B. Bijl @ Dave Bear on Dec 5, 2018 9:26 AM
  Mark Correct
  Correct Answer
  Hi Dave,
  
  Great info, thnx!
  I didn't model this device myself, and with the lack of proper knowledge I haven't seen any of these issues / points of improvements.
  I will try these ideas in the model. Happy to learn more every day
  
  My question still stands though. Because why does it fail in Solidworks, but succeeds in a realized form?
  Like • Show 2 Likes2
  Actions
  - Steven McCallion @ B. Bijl on Dec 5, 2018 9:40 AM
    Mark Correct
    Correct Answer
    How refreshing, someone coming with experiment and demanding to know why the simulation is wrong!
    
    "To be very clear I'm not a professional using static simulations. I know the basics."
    Yep, well unfortunately the definition of 'professional' when it comes to simulation is rather ... loose. If you can match this simulation to your experiment then as far as I'm concerned you're far more of a professional than 99% of simulation users.
    
    1. What elements are you using and are they appropriate?
    
    2. Have you done a mesh convergence test? NAFEMS The Importance of Mesh Convergence - Part 1 engineering analysis and simulation - FEA, Finite Element Analysis, C…
    Like • Show 1 Like1
    Actions
    - B. Bijl @ Steven McCallion on Dec 5, 2018 10:40 AM
      Mark Correct
      Correct Answer
      Hi Steven,
      
      1. Can you elaborate maybe?
      Elements of parts (sheet metal, solids, etc)?
      
      2. I haven't ! Will read through this information after work
      
      And thank you for the motivation !
      Like • Show 1 Like1
      Actions
- James Riddell @ Dave Bear on Dec 5, 2018 10:56 AM
  Mark Correct
  Correct Answer
  B. Bijl, if your FEA stress is higher than the 235 MPa yield limit then, yes, it fails. If it does NOT fail under proof loading then your FEA model is wrong.
  
  You have incorrect boundary conditions. The elements are probably not connected properly. Don't feel bad about simplifying your model - it will never be exact.
  
  Have you done any hand calculations? What would you expect to see?
  Like • Show 2 Likes2
  Actions
  - B. Bijl @ James Riddell on Dec 6, 2018 6:27 AM
    Mark Correct
    Correct Answer
    James,
    
    The elements are connected via contact set, bonded. Using the automatic function. Since it's already a very simpel model I don't really know how to simplify it even further.
    
    Those contact sets, and conditions are still not completely clear for me, so I can imagine I've done something not totally right.
    Like • Show 0 Likes0
    Actions
Frederick Law Dec 5, 2018 9:38 AM
Mark Correct
Correct Answer
Stress concentration.
Safety factor.
The area getting max stress are corners. The sharp 90 deg on the lifting lug is welded to the bend part which will be a fillet.
The fillet will never see stress that high.
The sim never say part will fail. It say max stress is higher then yield.
Yield on material is minimum. So material could have higher yield.
Even if not, material will stretch and yield will go up.
So the part will deform a little but won't break.
If stress is higher than Ultimate, its another story.
Like • Show 4 Likes4
Actions
- B. Bijl @ Frederick Law on Dec 5, 2018 10:40 AM
  Mark Correct
  Correct Answer
  Hi Frederick,
  
  ''The sim never say part will fail. It say max stress is higher then yield''.
  - Doesn't this means the material will fail? As soon as the von Mises goes higher than the yield strength of the material it will deform permanently, right? Material we used is normal S235JR steel.
  
  I did mean by the word 'fail' that according to Solidworks it should deform plastically. Not that is should shear / tear / break.
  
  ''The fillet will never see stress that high''.
  - That's what I thought. I've tried to fiddel with the weld connections. But didn't get a realistic result so stepped away from it again.
  Also, I can only imagine moddeling or somehow recreating a weld in Solidworks is going to be a pain...
  
  ''If stress is higher than Ultimate, its another story''.
  - I don't know what you mean by this.. The stress in my model does reach a maximum of 1,214e+09. While the max of S235JR steel is 2,350e+08. So this would mean it fails, since it passed max (or ultimate).
  Like • Show 2 Likes2
  Actions
  - Frederick Law @ B. Bijl on Dec 5, 2018 10:52 AM
    Mark Correct
    Correct Answer
    I ran the simulation and max was 2,500e+08.
    Its so close to yield, I won't worry too much. Since you tested the product already.
    Of course you should change the design to eliminate that.
    
    Also, the high stress concentrated spot does affect fatigue on repeated loading.
    Better check the requirements.
    Like • Show 2 Likes2
    Actions
    - B. Bijl @ Frederick Law on Dec 6, 2018 6:27 AM
      Mark Correct
      Correct Answer
      What did you do different than I did? Since I get a different value.
      
      Can you maybe show me please ?
      Like • Show 1 Like1
      Actions
      - Frederick Law @ B. Bijl on Dec 6, 2018 8:38 AM
        Mark Correct
        Correct Answer
        I didn't know you changed Max value on the chart to 2,500e+08.
        I rerun sim with "treat part as solid".
        I did not change load and fixture.
        Looking at this, I'll say it fail.
        I'm not too worry about the red in the corner but the green area is bad.
        Like • Show 0 Likes0
        Actions
        James Riddell @ Frederick Law on Dec 6, 2018 9:25 AM
        Mark Correct
        Correct Answer
        Frederick Law you have this BOTH restrained and loaded incorrectly. It's not even remotely close to RL conditions.
        Like • Show 1 Like1
        Actions
        Frederick Law @ James Riddell on Dec 6, 2018 9:27 AM
        Mark Correct
        Correct Answer
        I rerun sim with "treat part as solid".
        I did not change load and fixture.
        Like • Show 0 Likes0
        Actions
        James Riddell @ Frederick Law on Dec 6, 2018 9:28 AM
        Mark Correct
        Correct Answer
        Frederick Law wrote:
        
        I did not change load and fixture.
        "Two wrongs don't make a right." ~ Every mother everywhere.
        Like • Show 1 Like1
        Actions
        Frederick Law @ James Riddell on Dec 6, 2018 9:33 AM
        Mark Correct
        Correct Answer
        James Riddell wrote:
        
        "Two wrongs don't make a right." ~ Every mother everywhere.
        But 3 left does
        
        There more thing wrong then load and fixture. I'll let the OP fix everything.
        Also I just try point out why sim doesn't agree with real world, not teaching how to use sim properly.
        
        That's your job
        
        Just because SW haven't find a fix so I can run 2018 and 2019 together with online license
        Like • Show 0 Likes0
        Actions
- James Riddell @ Frederick Law on Dec 5, 2018 10:22 AM
  Mark Correct
  Correct Answer
  Frederick Law that is not an accurate description of the comparison between FEA and proof loading. If stress reaches the material yield then it is a fail - period.
  Like • Show 2 Likes2
  Actions
  - Frederick Law @ James Riddell on Dec 5, 2018 10:39 AM
    Mark Correct
    Correct Answer
    Agree.
    Problem is the part is not modeled 100% to the product. Especially the sheet metal part. Bent relief, tear etc.
    To be 'safe' we would 'beef' it up so stress would not get pass yield.
    In this product, it should be CMM after load to see if it deformed.
    
    On the other hand, it won't take much to get stress a bit lower. Like a thicker sheet metal. Longer lifting lug. Or what Dave suggested.
    Like • Show 1 Like1
    Actions
    - B. Bijl @ Frederick Law on Dec 5, 2018 10:59 AM
      Mark Correct
      Correct Answer
      This modeled product is exactly as it is realized.
      
      And the whole thing is, I can make it stronger in solidworks by increasing the thickness of the sheet metal, but the real product is already strong enough..
      Like • Show 1 Like1
      Actions
      - Frederick Law @ B. Bijl on Dec 5, 2018 11:17 AM
        Mark Correct
        Correct Answer
        We could never model and run sim 100%.
        Material spec is a range. We usually take the minimum to be safe. Material received could have higher yield.
        After the part is bent, bend area is work hardened so higher yield again. The bent usually looks different then model.
        Is the model use thickness from measured part? Or 'nominal' ?
        
        Just answering your question: Why sim and real is different.
        
        All the uncertainly is why we use safety factor. Its easier to over engineer the product than get all the spec exactly and hope nothing went wrong.
        
        Sim gave a reference if your design is on the right path and area for improvement.
        
        Sim use data gathered and input by user. It doesn't know or care if the info is correct or.
        Like • Show 3 Likes3
        Actions
J. Mather Dec 5, 2018 10:19 AM
Mark Correct
Correct Answer
JM Van Oossanen wrote:

I know the basics.

But when I try to simulate this in Sw, it shows that it should fail.
Looking at a representative Stress-Strain curve note that linear static stress analysis is only within the yellow highlighted portion of the curve above - the linear elastic range. Note the location of the Ultimate Strength and especially note the Fracture location on the curve.

I assume your definition of "failure" is fracture of the part or perhaps permanent deformation in the non-linear plastic range of the curve (in which case run a non-linear analysis).

I note that you did not indicate the calculated deformation in the high stress areas. (I can't open your files to examine as you are using a later release than I have.) In any case, keep in mind that your analysis is only within the linear elastic range.

Consider further the image below.
Imagine you were starting with a flat blank to press into this deformed shape. This would be plastic deformation. Permanent deformation. Has the part failed in the process of forming from a flat blank into this permanently deformed shape? (Or simply consider the force needed to make the bends (permanent deformations) in forming your bracket from sheet metal.)

The term Safety Factor is an unfortunate misnomer. It is simply a measure of S_yield/S_calculated,
the designer needs to define their measure of "failure". Is it permanent deformation of a certain percentage? Is it fracture?
Like • Show 3 Likes3
Actions
- James Riddell @ J. Mather on Dec 5, 2018 10:19 AM
  Mark Correct
  Correct Answer
  By definition for proof-loading the part can't yield, i.e. no permanent deformation and no damage.
  Like • Show 2 Likes2
  Actions
James Riddell Dec 5, 2018 10:18 AM
Mark Correct
Correct Answer
1. You are not restraining nor loading the model in the same manner as it would be IRL.
2. Define "it fails" - is your yield limit exactly the same as the actual material (including weld filler metal)?
3. Your stress results DLR - I would expect a little better distribution of the hot-spot if the formed plate were fully connected to your clevis plates.
Like • Show 1 Like1
Actions
- B. Bijl @ James Riddell on Dec 6, 2018 6:27 AM
  Mark Correct
  Correct Answer
  ''You are not restraining nor loading the model in the same manner as it would be IRL''.
  
  Well as close, those hoist lugs/ears are attached to a beam via a locking pin. Underneath it is a plate attached with bolts to the four holes. So that's exactly as I set it in Solidworks.
  
  It fails, since it may not deform plastically irl.
  Like • Show 0 Likes0
  Actions
  - James Riddell @ B. Bijl on Dec 6, 2018 7:21 AM
    Mark Correct
    Correct Answer
    B. Bijl wrote:
    
    ''You are not restraining nor loading the model in the same manner as it would be IRL''.
    
    Well as close, those hoist lugs/ears are attached to a beam via a locking pin. Underneath it is a plate attached with bolts to the four holes. So that's exactly as I set it in Solidworks.
    
    It fails, since it may not deform plastically irl.
    B., No you are most assuredly not. You have the lift holes completely constrained. There is no pin or bolt that I know of that can 'lift' the bottom of a hole. A tell-tale for bad connection is the odd stress pattern at the ends of the lift lugs (clevis) that does not extend down the side at all. Your loading is not placed as a pin through those four bottom tab holes would be applied.
    
    Are you CERTAIN that you did not apply 5 tons to each of the tabs in the corners instead of total? That is the first place I'd look.
    
    I might have some time this weekend to look at your model if you haven't solved it by then. Feel free to PM me.
    Like • Show 2 Likes2
    Actions
B. Bijl Dec 6, 2018 6:27 AM
Mark Correct
Correct Answer
Thank all of you guys for the amazing feedback by the way!

Really helpfull, and I'm glad to see such a active 'professional' forum nowadays
Like • Show 2 Likes2
Actions
Sergio Monti Dec 6, 2018 7:55 AM
Mark Correct
Correct Answer
B., please consider also:
- Fabricators usually use S275 sheets instead of S235, please check this
- Welded area .... this is a big deal! Unless you've done a normalizing or stress relief after welding, yield strength is much higher, despite ultimate strength is not - welded parts are usually more brittle
- Bent areas have been stretched beyond the yield point to achieve deformation. Therefore new yield point will be different from standard material
- Consider that a deformation of 0.1mm can increase the yield strength quite a lot, so may be you had deformation but you're not able to see it
Like • Show 2 Likes2
Actions
Bill McEachern Dec 6, 2018 10:05 AM
Mark Correct
Correct Answer
I did not read all the posts in any great detail and I am unsure if the issues is resolved or not. If an elastic plastic analysis is done where you load and unload the product it is often the case that the difference in shape is not noticeable as the load will redistribute till it is sustained and upon unloading the shape returns to the initial shape as far as the eye can see even though local yielding has occurred. No idea about this case but you can check this hypothesis by doing a NL elasto- plastic analysis - just assuming a low tangent modulus is likely good enough to confirm or refute.
Like • Show 2 Likes2
Actions

Static simulation fails while real product succeeds

Attachments

Outcomes

Related Content

Recommended Content