Non-Linear Beam Analysis - Plastic Deformation

I am attempting to create a simulation study that would match real world results for an aluminum profile that we have designed (96" long, 6063-T5; fixed on both sides and has a 200 lb concentrated load in the middle). We have the real world displacement data for the described loading situation, and I want to get close to it in a reasonable and reproducible manner.

I have attempted modelling the profile as a beam, and running the simulation in the von-Mises plasticity material model, but that fails almost immediately, stating that the iterations are not converging.

I also modelled it as a solid, fixed both end faces and tried both a concentrated force (at a point) and a force at a face made by a split line, and received the same error (albeit with a  longer solve time). 

I've attached screenshots to show how the profile looks, and the loading situation. I can't help feeling that I am missing something fundamental to how I am supposed to set this up. Please help!

PS. The only successful runs I've had were through the solid model, utilizing the "Plasticity - Tresca" material model, though I haven't the slightest idea why and it makes me question the validity of those results (along with the fact that the resultant displacement implies that it is significantly stiffer than it's real world counterpart, which is not expected due to the way the test was conducted).

PPS. I did try to increase the convergence tolerance, from the default 0.0001 all the way up to 10, but it always fails.

SolidworksSimulation
Answers 25
SF
SF 2015-05-04 Best Answer

I would recommend starting simple.

Does it solve with linear.

Does it solve with nonlinear solver but linear material.

Then you can start diving into nonlinear materials. If it works without the nonlinear material, I'd look at the definition of your nonlinear material.

HA
HA 2015-05-04

Jared,

It does solve with linear, in both the material and the study type. I first started simple with those, but was not satisfied with the results received. hence the move to non-linear. I am using the default values that Solidworks has for 6063-T5 for all studies, it seems that the Hardening Factor and the Tangent Modulus are left blank in the material definition for this Aluminum, I assume that the tangent modulus is calculated during the solve and that the Hardening Factor is not necessary for this situation, though I am not sure. I do believe that the non-linear modelling is the best way to go, as it has gotten me the closest to the true displacement.

BM
BM 2015-05-04

to the best of my knowledge beams with NL material properties are not supported. you need a beam element with a sophisticated cross section definition which is not in SWX Sim.

HA
HA 2015-05-04

Hi Bill,

I suspected that this may be the case, since I have not been able to get any sort of result out using the von-Mises plasticity material model. I therefore tried to circumnavigate that possibility by modelling the part as a solid. However, it only runs using the Tresca plasticity model when I do so, leading me to question if there is something about the setup that might be preventing a von-Mises type of analysis, and whether it is causing inaccuracies. What are your thoughts? 

SF
SF 2015-05-04

Have you tried running with tangent modulus value? I believe that might be the issue as there may not be a fully defined stress-strain curve.

SF
SF 2015-05-04

this is with solid elements correct? not beams?

can you post your material information.

SF
SF 2015-05-05

You said it runs with linear material - does it exceed the yield stress ?

Even if it shows yielding at some stress concentrations (end conditions or at applied load locations) it may not require a non-linear analysis to match the test data. This local yielding is small by comparison to the bending of a long beam.

What test data are you trying to correlate (displacements, strains, etc.) ?

I have found many of my problems with correlation are test setup (fixed ends aren't really fixed, load cell is misinterpreted, displacement transducers locations not same as in model, strain gages not reading correctly, etc.). This is an open section and will twist if not loaded thru the shear center.  Did the load application restrain the twist ?

Do hand calcs of the test data correlate to the model and test data ?

Mark

HA
HA 2015-05-05

​ and ​,

I'm using the default values provided by Solidworks for the material we used during testing, 6063-T5 aluminum. I cannot find any distinct tangent modulus value for this material and when I did research it seemed to be to be something that changed as the study ran through the stress-strain curve. Perhaps it is as you said and there is no properly defined stress-strain curve for this material in SolidWorks?

These are the material properties for linear elastic:

And these are the material properties for von Mises plasticity:

I do not see any values under the "Tables & Curves" tab when I select "Stress-Strain Curve," does this mean that it is undefined, or simply that I cannot see the defined curve since it is set up by default?

comment imagecomment imagecomment imagecomment image
HA
HA 2015-05-05

Yes, it is with solid element, not with beams. Please see above for the material information.

HA
HA 2015-05-05

Mark,

I am attempting to correlate displacement data. I remember it yielding during my earlier runs, which along with a small permanent set during actual testing, led me to conclude that it might be going through some plastic deformation. However, I just now did a quick run and it's not yielding (which also makes sense since it's only 200 lbs). The deformation is calculated at around 1.1" whilst real world measurements set it at around 1.4". This is an aluminum reinforcement piece inside PVC railing, it is bolted to posts on both sides and is tested along with the full railing assembly (the 200 lb concentrated force placed at the top midspan). Common sense tells me that the additional resistance provided by the layers of material around it, along with the multiple balusters on the bottom should make it stiffer, not more flexible than my simplified testing model. I'm trying to reduce further complexity by testing only the engineered aluminum, and not the full assembly.

comment imagecomment image
SF
SF 2015-05-05

if there is no stress strain curve, i'm not surprised that it gets upset when it reaches yield, it has no material data at that point

HA
HA 2015-05-05

Alright, I managed to obtain some stress-strain data for this material, and applied it to the material in SolidWorks, after a bit of finagling (it kept erroring out and saying that the curve should not start at the origin)

Following that error, I adjusted the Stress-Strain curve, and interpolated what the strain would be at the yield point, then started the curve from that point. Running with that led back to this recurring error:

The above runs were done with the beam model, just to see if perhaps the stress-strain would make a difference for them. The solid model gives a similar error if the curve starts from zero, and the following error once it is started from the yield point:

I have tried reducing the Singularity-elimination factor, as well as raising the convergence tolerance and I am unsure how to adjust the ETAN reliably. Thoughts?

comment imagecomment imagecomment imagecomment imagecomment imagecomment image
SF
SF 2015-05-05

recommend posting the model

ETAN you just estimate from the stress strain curve

HA
HA 2015-05-05

Is ETAN a single value or a varying derivative? How would I go about estimating it?

SF
SF 2015-05-05
MM
MM 2015-05-06

I've looked at your file, and the first thing I notice is that the general stress in your linear simulations are well below yield with your setup. So Non-linear shouldn't give you the desired result since it follows the linear solution up to yield.

I'm not sure that I understand your test setup, but using fixed fixture on two surfaces is very hard to replica in the real world. Like supergluing the surfaces against a infinitly stiff wall. If I try your setup but with only the 2 bottom edges fixed (like a hinge), I get the result below. If I look at X displacement the result is 1,43 inches. But observe, that the part, due to its shape, is allowed to twist since the load is not thru the shear centre. This is probably not the case with the real product since the "ladder steps" would minimize that behaviour.

comment imagecomment image
JR
JR 2015-05-06

I have not looked at your data but I presume you know that the input for material data for non-linear plasticity is not SS, correct?  I believe it is 'true-stress' vs. 'log-strain' - the acceptable interpretation is in the SW documentation.

That being said, why should you need that?  Don't you expect the material to hold the 200# load w/o permanently deforming?

JR
JR 2015-05-06

​, based on the above picture, I would suggest that you do not have the correct restraints on the ends.  (I presume you are trying to model the fat, drunk guy at the party leaning on the railing.)  A more forgiving restraint would give you more deflection obviously.

Also, have you tried your analysis with a standard C channel that has the same moment of inertia values as the shape you actually have?  That might give you more reproducible results.

HA
HA 2015-05-06

Haha , yes, you presume correctly. In response to your previous comment, I do not expect the said fat, drunk guy to permanently deform aluminum railing. However, when I saw that my results had some localized yielding, I thought that they might affect the results in a way that stopped the railing to stop deforming prematurely; so I tried to move to an analysis that goes past yielding. I had figured that the fixture was a bit too unrealistic, but could not think of a better way to do it. ​ had a great solution below (didn't think to restrain edges), and I think that it may be the way to go. I had also thought to do hand calcs, or a simplified model of it as a C-channel but it didn't occur to me to simply use the same moment of inertia values (I was having difficulty visualizing how to accurately simplify it), so that helps a lot and I thank you. Such a simplification will help further with the validation.

I do have a follow up question regarding your comments about stress strain data, however, as I have other specimens to validate which do go past yield. I have not had as much trouble with those, but in the interest of being as accurate as possible, I'd like to ensure that I understand the type of data that needs to be input for non-linear plasticity. Could you elaborate further on what the appropriate interpretation is?

HA
HA 2015-05-06

​,

Thank you! That seems to be exactly the type of result I'm looking for. I will explore further, but I imagine that this solves most of the problems. As far as the twist goes, I've had trouble trying to locate the force at the shear center; I tried to locate the center of mass, and use it as a reference point to locate the force, but SolidWorks doesn't seem to allow you to use the center of mass reference point in that way. Do you have any tips on properly locating the force through the program? 

JR
JR 2015-05-06

If you go to 'Simulation Help', search for 'Input for Stress/Strain Curves' for the definition(s)/requirement(s) for input.

Analysis Options
Material ModelSmall Strain, Small DisplacementSmall Strain, Large DisplacementLarge Strain, Large Displacement
Non Linear ElasticTrue Stress, Engineering StrainTrue Stress, Engineering StrainN/A
Elasto - Plastic von Mises Plasticity, Tresca Plasticity, Drucker PragerTrue Stress, Engineering StrainTrue Stress, Engineering StrainTrue Stress, Logarithmic Strain
Hyper Elastic: Mooney-Rivlin, Ogden Blatz KoEngineering Stress, Stretch ratioEngineering Stress, Stretch ratioEngineering Stress, Stretch ratio
Super ElasticTrue Stress, Logarithmic StrainTrue Stress, Logarithmic StrainTrue Stress, Logarithmic Strain
ViscoelasticTrue Stress, Engineering StrainTrue Stress, Engineering StrainN/A
MM
MM 2015-05-07

Finding the shear center is not so easy. On my picture above it is on the left side of the part. On a simpler U-beam you could calculate it, but I don't know any way to find it in Solidworks. To locate a force on a point that isn't on the part you need to use a remote load/force. So if you want to add a load in the center of gravity, first you calculate it, to create a reference point. Then you add a coordinate system in that point and finally add a remot load/force.

I would use a simpler approach in this case and do split lines for each "ladder" step and restrain these surfaces from movement in the normal direction. Not perfect, but good enough i think.

JR
JR 2015-05-07

http://www.mechatools.com/en/shapedesigner/properties.html

The above appears to be some software that will calculate the shear center of any geometry (see the second box items).  (Full disclosure: I have never used this software, have no affiliation with the company and can't attest to its accuracy.)

For a rough first pass I would suggest to "match" a C-channel cross-sectional area with similar "leg" length and use the shear center of that.  BTW, you don't need to place another coordinate system to locate a remote mass/force, you can just key in the point based on the global coordinate system.

HA
HA 2015-05-07

Thank you James, that  helps and I will be sure to keep on investigating.

HA
HA 2015-05-07

​, split lines are a great idea! it will certainly make it a bit more realistic. I will explore that option.
de

​, I will also explore the software for calculating the shear center, though I think that an approximation based on the C-channel may be the best bet.

I may just try to avoid the inherent torsional error altogether by finding a way to accurately depict the loading situation using split lines as well. Thank you for all of your help guys!