Continue to Site

Eng-Tips is the largest engineering community on the Internet

Intelligent Work Forums for Engineering Professionals

Register Log in
  • Congratulations The Obturator on being selected by the Eng-Tips community for having the most helpful posts in the forums last week. Way to Go!

simple stress/strain validation

Status
Not open for further replies.
KenPob

KenPob

Structural
May 29, 2013
8
Hi,

I am a structural engineer, and I have recently began using the Abaqus as a finite element software. After numerous attempts and researching a lot of information, I have not been able to validate a simple test.

What I am trying to do is model a non-linear steel part in 3D (as a solid) and trying to validate the stress/strain curve I receive from the Abaqus to the one I have inputted into the material property. I used the elastic and plastic models in the Abaqus/CAE. In all honesty the numbers are not important me (i.e. which structural steel, it could be 60 ksi grade or whatever), but I just want to know how to model it correctly so that the stresses and strains match up. I have read several topics here, but none seem to help.

Does anyone have a very basic input file they could share that has a working non-linear structural steel material property that matches the Abaqus stress/strain to the theory/actual stress/strain.

This problem has me stumped and I have been stuck on something so seemingly simple for a while now.

Thank you for any help you may provide.
 
Replies continue below

Recommended for you

Sort by date Sort by votes
Here it is:

Input File

would you like me to just paste it in, or is the above link alright?

Thank you for your quick reply

 
Upvote 0 Downvote
When I had first modeled this, I did not have a load at that location. Someone I know suggested doing that to see if any change would occur. That load is very small, and did not have any effect on the results, however.

For some reason, the analysis is not capturing the linear and non-linear behavior very accurately. The non-linear also seems to be more accurate than the linear results, because the slope of the elastic region is not even close to 28-29 million psi.
 
Upvote 0 Downvote
Correct me if I am wrong: I imagine the material properties are based off of uniaxial tensile tests, which is why you are simulating a tensile test. If so, you are *not* enforcing a uniaxial strain/stress state (for example, pinning the nodes on one end). Secondly, because of time incrementation parameters in the static analysis step definition, the solver quickly jumps to the plastic region and thirdly, because of your chosen options in the output field requests (interval), you are missing some data. Try the following:

Code: 
** BOUNDARY CONDITIONS
** 
** Name: Fixed Type: Symmetry/Antisymmetry/Encastre
*Boundary
Set-5, 2, 2
** ----------------------------------------------------------------
** 
*Step, name=Load, nlgeom=YES
*Static
0.01, 1., 1e-4, 0.01
** 
** BOUNDARY CONDITIONS
** 
** Name: PullUpDisplacement Type: Displacement/Rotation
*Boundary
LoadNode, 2, 2, 3.5
** 
** LOADS
** 
** Name: Load-1   Type: Concentrated force
** *Cload
** LoadNode, 2, 1.
** 
** OUTPUT REQUESTS
** 
*Restart, write, frequency=0
** 
** FIELD OUTPUT: F-Output-1
** 
*Output, field
*Node Output
CF, RF, U
*Element Output, directions=YES
LE, NE, PE, PEEQ, PEMAG, S
*Contact Output
CSTRESS, 
** 
** HISTORY OUTPUT: H-Output-1
** 
*Output, history, variable=PRESELECT
*End Step

However, you still need to create a uniaxial strain/stress state. A quick and easy way to do this is to create one cube of unit dimensions, use equation constraint just as you did previously, and the output RF and U will automatically be equal to stress and strain.

Are you new to this forum? If so, please read these FAQ:

 
Upvote 0 Downvote
Thank you so much, it has finally worked.
 
Upvote 0 Downvote
Sorry for the long time to reply for some reason I did not receive an e-mail notification.

Yes I tried it on a cube, and applied a uniaxial strain, and the results match very nicely.

I am currently doing the same on a concrete cube, using the Concrete Damage Plasticity Model where I am required to input Compression and Tension Behavior of the Concrete. However, this will obviously be a bit more involved than steel due to the nature of concrete material properties.

For some reason, the tension test on the concrete matches the theoretical data quite nicely. Meaning when I apply an upward (tensile) displacement, the stress/strain curve from Abaqus matches nicely with the theoretical data.

But when it comes to the compression test, where I apply a downward (compressive) displacement, the stress/strain curve from Abaqus does not match as nicely. The data in the elastic region matches in a relatively good way, however, in the plastic region my concrete cube will not fail like the steel cube did. The stress keeps increasing as the strain increases without actually me seeing a drop off. So I am suspicious as to why that is, because the tension test saw a failure behavior in the Abaqus results, but the compression test seems to never fail. If you have some insight on this matter, that would be greatly appreciated as well.
 
Upvote 0 Downvote
Here is the material definition part of the input file:

** MATERIALS
**
*Material, name=Concrete-CDP-Cube
*Density
0.0002246,
*Elastic
3.56045e+06, 0.2
*Concrete Damaged Plasticity
31., 0.1, 1.16, 0.666667, 0.
*Concrete Compression Hardening
356.028, 0.
699.719, 3.45483e-06
1029.01, 1.09436e-05
1343.13, 2.26845e-05
1641.87, 3.8735e-05
1925.35, 5.90599e-05
2193.91, 8.35659e-05
2448.02, 0.000112122
2688.21, 0.000144575
2915.1, 0.000180757
3129.29, 0.000220492
3331.43, 0.000263604
3522.14, 0.000309916
3702.04, 0.000359256
3871.71, 0.000411454
4031.75, 0.000466351
4736.28, 0.00315966
4881.3, 0.00712494
5264.16, 0.0742979
*Concrete Tension Stiffening
360.536, 0.
342.657, 0.000104944
291.385, 0.000219139
259.737, 0.000327882
237.582, 0.000433981
220.894, 0.000538555
207.706, 0.000642148
196.923, 0.000745063
187.879, 0.000847487
180.144, 0.000949537
173.422, 0.0010513
167.507, 0.00115282
162.245, 0.00125416
157.522, 0.00135533
153.25, 0.00145637
149.359, 0.0015573
145.795, 0.00165812
142.514, 0.00175886
139.479, 0.00185951
136.66, 0.0019601
134.032, 0.00206062
131.574, 0.00216109
129.268, 0.00226151
127.099, 0.00236187
125.053, 0.0024622
123.118, 0.00256248
121.286, 0.00266272
119.546, 0.00276293
117.892, 0.00286311
116.315, 0.00296325
**

I have been reading up as much as possible, trying to find out more information on this material model. I have yet to determine how I would define "damage parameters" as that is an additional option for Concrete Damage Plasticity, even though I have read up on the information, it might be difficult to get some values without test data, which I don't have. But then I am not sure if I need the "damage parameters" since my tension behavior matched nicely and showed the decreasing branch of the stress/strain curve, and I did not define "damage parameters" for that.
 
Upvote 0 Downvote
Are you sure your units are correct? Most FEA codes (including Abaqus) are agnostic to the choice of unit systems; the user must ensure consistency in units. Also, are you sure your material data is correct?

Are you new to this forum? If so, please read these FAQ:

 
Upvote 0 Downvote
By the way, the reason why I think your problem may have to do with the material definition is because of: 1) a tool in /CAE called Job Diagnostics and 2) warnings in the .msg file. One must be very careful when it comes to warnings in the .msg/.dat files. Also, if you are not aware of Job Diagnostics, go through the following two examples in the documentation: connecting lug with plasticity and nonlinear skew plate.

Are you new to this forum? If so, please read these FAQ:

 
Upvote 0 Downvote
The above posts have actually helped me solve some of the problems I am having with my model that I discussed in this thread:
So I would like to thank you for that. I have been also to confirm my stress-strain data for compression and tension thanks to this thread. Currently, I am working on shear behavior though, as that is my main concern so if that might be a future concern of yours I look forward to seeing what help can be provided through this thread.
 
Upvote 0 Downvote
I am currently interested in validating the stress/strain compression data of my concrete cube. The tension data has been validated, but I am still trying to resolve the compression data.

Shear and Flexure are also an interest to me, but I have not read up on that to see which material model would be bested suited for this. (I have taken a look at your thread). As far as I can tell, the Concrete Damage Plasticity model is acceptable for compression/tension behavior, but I am not sure how to capture the shear behavior in an accurate manner.
 
Upvote 0 Downvote
If the element formulation (i.e., type of element) allows constant or may be even linear shear (if it is a quadratic element) deformation as a straining mode (i.e., eigenvector or mode shape in a frequency analysis; eigenvalue tells you the stiffness in each one of those straining modes), then all you need to make sure is that your material data, boundary and loading conditions match the experiment. And finally, spatial discretization (i.e., mesh size) must be fine enough to model variations in stress in the problem being modeled such as stress concentrations near a hole, transition from compression to tensile in bending, etc.

Are you new to this forum? If so, please read these FAQ:

 
Upvote 0 Downvote
If the previous post confused you, don't worry about it. [By the way, in a way, that post is the essence of FEA.]

All you need to do is make sure the element type allows the type of deformation you expect in your problem - which can easily be done by reading the documentation for any given element type.

Are you new to this forum? If so, please read these FAQ:

 
Upvote 0 Downvote
Would the following error: "The plasticity/creep/connector friction algorithm did not converge at # points"
entail that the incorrect element type is being used for the expected deformations?
 
Upvote 0 Downvote
The problem is, I have been unable to determine the cause of this problem. I have read other posts and articles about this problem but to no avail.
 
Upvote 0 Downvote
Status
Not open for further replies.

Similar threads

yassou
  • Locked
  • Question
Bulk Vs Foam Stress-Strain ?
Replies
3
Views
168
FEA way
FEA way
BigMims
  • Locked
  • Question
Strain field smoothing 1
Replies
2
Views
165
BigMims
BigMims
C
  • Question
Generalised plane strain using Abaqus Explicit
Replies
1
Views
803
FEA way
FEA way
Bishal123
  • Locked
  • Question
ABAQUS shear strain rate
Replies
1
Views
232
FEA way
FEA way
abc123ali
  • Locked
  • Question
Result error in choosing plane stress-strain thickness
Replies
9
Views
225
FEA way
FEA way

Part and Inventory Search

Sponsor

Back
Top Bottom