Hi,
I have been trying to simulate a physical tested clamp working safely under the load of 40KN with SWX simulation by the results value of this test is just freaking me.
I don't know what to do with it, where I am going wrong. I have simplified the model for simulation but still unable to get the safe results.
Looking forward for some desperate help. I have attached the model for further reference.
Thanks in advance,
Yash
I've checked your model and the main issue there is the presence of geometric singularities due to sharp inner corners. Regardless of material properties or fabrication processes, sharp inner corners are not common or impossible in real parts, there will be always radii as small as they would be. Thus, results near sharp corners are not correct.
Sharp edges in finite element analysis evaluate as infinite stresses due to a strain direction discontinuity just in the corners.
In order to overcome this problem, estimate a real fillet radius (no matter how small) and apply proper mesh controls in the edges and face of such radius. Use curvature mesh control to mesh more than six elements at fillets. Check Peterson's Stress Concentration Factors, pretty good literature regarding these subjects.
Regards
Thanks for your time Jerry,
The results m worried about you are stress and fos
Load & fixture:-
Stress Value much higher then the yeild strength...
FOS value is 0.4, as idelly it should be atleast 1.
Thanks for your concern Angelo, I got your point but just one clarification
If you are talking about these corners marked as shown in the below pic.
It does have fillets "Fillet242" which I suppressed just to simplify the model as the stress value with the fillets where much higher than the current value.
Thanks again for reference literature.
Regards,
Yash
Yash. Although Angelo makes a good point about stress concentrations, I have run your model to convergence and the regions that are predicted to exceed yield go well beyond this corner.
So the only suggestions I have are to double check your load magnitude, material properties, and the manner in which you are loading the part.
Just a guess, but I doubt this part is loaded the way you have the simulation set up. I think you need to split the face you have the load applied to - I would expect the load to pount only downward and not to be applied to this purple area.
Hi Yash, What are there at hole connect? Example pin, shaft,..
Hi Jeremy,
I think you are right and I tried your suggestion but I am still unable to get the right results.
Thanks & Regards,
Yash
Thanks Paul for your time, I just want one suggestion that in the mesh control option as Angelo was pointing is there any kind of specific element size or ratio which I can apply.
Regards,
Yash
Hi Satit,
Bolts and pin, does it makes a difference???
Regards,
Yash
Hi Angelo,
Can you suggest any kind of specific element size or ratio which I can select for mesh control.
Regards,
Yash
I'm not sure. becuase high stress concentration at fillet. I have questions :
1. What is this model part of this works?
2. How does the model part work?
3. I have a question about the area at the force action on the model. Please see above picture;
I have recalculated as shown in the results displacement below.
I need to know that why displacement along axis Z was most each axis? Have we selected the wrong area model?
Thanks for your concern Satit.
These parts are Conductor clamp & connectors used in electric distribution line. The curved surface is used to hold the high voltage electric wires.
The area at the force action is might be wrong as Jeremy Feist above suggested, I should have used the split lines in it.
As you said "wrong area model", am also now getting this feeling, actually I was working on it with the inputs given by one of our customers. I welcome your valued comments, regarding what can be the correct condition according to you.
Best Regards,
Yash
Yash, what is the right result in your opinon? I have tried to run the model to convergence, and my results are very similar to the ones Paul Becker displays below. Do you have actual results from real testing where i.e. the displacement is different from what you see in simulation? Can you please elaborate "right results"
Hi Mikael,
Right result here means the fos value should be equal to or more than 1, since the model is working safely till 40KN. I dont have the actual displacement results of the real testing,so I wont be able to comment on it. The only input I have is the model is working safely upto 40KN, the cracks develops after the load value increases beyond 40KN.
The convergence predict so many regions that exceeds the yield value, I tried numerious mesh controls on these regions but still the result value well exceeds the yield value.
Please do correct me if you find me wrong any where or in any process. Do let me know if any further information i required.
Regards,
Yash
Ok. If the actual part is working with repeated load without breaking then I understand your concern. I normally look in a section of the stress result to see how deep the stress goes thru the thickness of the part. Yielding is not the same as breaking, and sometimes you see that the stress is very shallow. Had a similar case where the simulation showed stress over yield strength in 40% of the section. In an actual test the part was still in one piece after unloading. But when we repeted the load a couple of times on the same part it broke. For this part we also measured the deformation during loading and compared this to the simulation results and it was pretty accurate.
Anyway, I hope that somebody more experienced can help you with this matter.
Would you know the weight of the cable? Don't know if it would be better to apply a remote mass with gravity, instead of applying a force.
See quick pic.
Interesting point from Mikael about depth of stress concentration.
Several good points have been made here. The area where over which the force was applied does appear to be inaccurate, given that the load comes from a cable running along the lower cupped portion of the part. The load applied to the vertical face would result in more bending than the part would actually see. Have you re-run with split lines to isolate the load to the actual area of contact? Also, I'm assuming this was run as a linear static study. That is fine, but be aware that any information on stress magnitude above yield is meaningless. Also, the region of material that is predicted to exceed yield is likely exaggerated because due to the same reason... stresses are calculated from displacements and are extrapolated linearly from E, although in reality, the stress-strain curve does not follow a linear path post-yield. This results in an artificially still part.
Two questions going forward would be: 1) Is yielding still predicted with the updated, correct loading and 2) If so, what is the actual response post-yield. If you need to know #2, then you will have to run this as a nonlinear static study using accurate data for the nonlinear stress-strain curve and material model. If you are also talking about the effect of repeated loading, then you will need to take into account hardening, which can be specified in the nonlinear study properties. This is likely what cause the part failure in the physical test Mikael described above, similar to bending a paperclip back and forth until it breaks.
I ran it again with the load face limited to what I would roughly expect to be the cable contact area. The restult actually looks worse than before. Approximately 72% of the part is predicted to exceed yield. Again, post-yield data must be taken as approximate, but I would say that it is not possible to reorient the force and have the results come out below yield. Something else is up here. Can you confirm the load and material properties? Do you really have ~9000lbs on a 5" x 3/8" thick aluminum bracket?
Plot below shows volume of material above yield limit (~72%)
Fixed restraints are always dangerous, they cause very high reaction forces and moments to develop. Those can be equally damaging to a structure than the actual loads! so vigilance is in order.
I would recommend, you model the pin that goes through the hole as well and run a contact analysis, you can still use a static study and under the study properties turn on "Large Displacement" if the pin is not shock loaded and the deformation is not too large.
I didn't bother reading the whole thread but when things go post yeild the elements essentially turn to mush (dramatic reduction in stiffness -well for alot of materials. ?Some amterials like the 300 stainlesses it is much less dramatic. Just take a look at a stress strain curve to see how it behaves - mil hbk-5 might be useful). Thus stress risers can bleed out, load can align with the restraints reducing bending moments or allowing another laod path to take up a fraction of the load proportional to the stiffnesses. if you want to check the viabilioty of this design take the minimum section and just do P/A. If it exceeds the ultimate strength then the problem formulation is wrong if experimental evidence exists that says the device can withstand the load. Material properties maybe in error for example. Maybe the item is forged and has been mechnically work hardened during manufacture, etc.
Either way a non-linear analysis is required. You can't figure it out with a linear analysis as no load redsitribution can occur whether it be material, geometric or contact induced.
Thanks Mikael for your time and concern, you did make a good point of the depth of stress. I am very much hopeful that I will definitely get the answer at this forum.
And I must say this that its people like you and your ready to help attitude makes this forum so special.
Best Regards,
Yash
The result does gives a favorable value but I am not really sure about the type of load , I really need to check it my customer and if its relevant to them, than the correct weight of the cables can get us to the right results I hope.
Thanks & Regards,
Yash
I will check it and get back to you Kevin.
Regards,
Yash
Hi Paul,
I also ran it the way you did, in some of early efforts and as the result was more worse so I didn't considered it. I have also googled a lot to confirm that the material properties and the load conditions are correct or not. What I found that these strain clamps are actually designed for various standards starting from 20KN and goes upto 50KN.
I have also attached the snapshot for the material propeties of LM6 which I got,
You have also made a point about the Non-linear analysis, can I just know what make you to consider this as a non-linear analysis?
Thanks & Regards,
Yash
Yash,
I don't have access to SW Simulation right now (and don't really have time to spend on it if I did have access), so I can't be much help. Plus I am not at all familiar with how it works, most of my FEA being done with ANSYS. I might be able to help a bit if you could show some of the results that you are worryied about and give some more explanation of your model, boundary conditions, and what you are expecting.
It looks like your file was first compressed with rar and then zipped. A lot of people don't have the rar software, so it would be much better if you just zipped the files or let the forum software zip them for you.
Jerry Steiger