## General Mechanical

#### Non-Linear Analysis_Multilinear Theory

• Abdul Malik
Subscriber

Hello Members,

Sorry Yesterday i couldn't upload anything due internet issues that why i have deleted the post.

I am working on workbench to model the tensile test with multi-linear theory. I took a test data from the book and try to solve it with ansys workbench. I have modeled the half specimen due to symmetry but haven't use the symmetry option from DM. I am facing some problems with the model first it does not show necking at the end of specimen but somewhere in the middle of half specimen.

Any Suggestions how to get the real behavior. The test data i used i below in the image. I have used the Raw true stresses and True plastic strains for multi-linear theory taking first point in table as Yield stress at plastic strain 0.

I am attaching the workbench file.

Many Thanks

• Sandeep Medikonda
Ansys Employee

Abdul,

Not everyone is able to download the files, so if you can show inline images of the boundary condition and results as you did with the stress-strain data, it would be more helpful.

Its not clear to me if you are using the symmetry feature in Mechanical? If not, please see here:

Regards,
Sandeep
Best Practices on the Student Community

• Abdul Malik
Subscriber

Thanks for the response, I haven't used any symmetry from DM. Because it was causing some other errors which still i couldn't solve. the solution was not converging.

I am uploading some pictures from the results

Many Thanks. I am trying to solve the same problem on complete geometry but that is not working the whole geometry get distorted and i received several errors.

regards

• Sandeep Medikonda
Ansys Employee

Use symmetry in Mechanical as shown in the video, not in DM?

1. Your mesh is too coarse.

2. This geometry looks sweepable, try to use Hex elements.

3. You are reaching your max. stress which is causing the problem to stop. Input a dummy point.

4. Do you have large deflection on? Post a snapshot of your analysis settings.

Regards,
Sandeep

• Abdul Malik
Subscriber

Thank for the recommendation.

I applied all unfortunately  the problem still remain the same. Nothing has changed.

below is the analysis setting is.

Many Thanks

Kind Regards,

• Sandeep Medikonda
Ansys Employee

Peter, if you have a few minutes. Can you help Abdul here?

• peteroznewman
Subscriber

Sandeep, A question I have had for a while is whether the mulitlinear kinematic hardening curve can have more than six points in it.  I read in the ANSYS Help that the TBDATA command, which I believe holds the curve data, can only hold six points.

Abdul, you can certainly delete several points on your curve that are not needed to maintain the shape. See if you can come up with a table that has only six points until we hear back from Sandeep.

You were given some good advice from Sandeep that your mesh is too coarse.  I suggest you start with an axisymmetric model to get some results much faster, and you can have a much finer mesh while still getting results in a reasonable wait times. An axisymmetric model is a radial slice. The axis must be the Y axis and the radial slice must be drawn on the positive X axis. You can draw the full length of the sample and not use a second plane of symmetry at the center of the length.  You must set the properties of the Geometry cell in Workbench to 2D before you attach the surface of the radial slice to Mechanical.

You also have unreasonable expectations regarding where the necking will occur. It does not need to happen at the exact center of the sample length. If you look at real samples, the necking occurs all over the length.

I made a quick model without looking at any dimensions from your model, and this is what the result looks like...

Regards,
Peter

• Sandeep Medikonda
Ansys Employee

Peter,

We can input multiple points for a curve, using multilinear kinematic plasticity and it would write them out under TBPT and not TBDATA. I just tested this.

This translates to:

```TB,PLAS,1,1,100,KINH
TBTEMP,7.88860905221012e-31
TBPT,,0,7.2790357
TBPT,,0.005257912,7.717585
TBPT,,0.010699119,7.9662418
TBPT,,0.016493532,8.1639913
TBPT,,0.022337942,8.3374619
TBPT,,0.028233342,8.5073642
TBPT,,0.033894386,8.6800701
TBPT,,0.03983034,8.8524645
TBPT,,0.045735934,9.0141681
TBPT,,0.051567974,9.1754035...```

Now, the TBDATA is written out for a BISO material model and that only allows 6 temperatures. So as a test, I input some random data:

In the input deck, this translates to:

```TB,BISO,1,6
TBTEMP,0
TBDATA,1,200,100
TBTEMP,100
TBDATA,1,300,100
TBTEMP,200
TBDATA,1,400,100
TBTEMP,300
TBDATA,1,500,100
TBTEMP,400
TBDATA,1,600,100
TBTEMP,500
TBDATA,1,700,100
```

Here, we can only input data 6 temperatures but for multilinear plasticity, there shouldn't be any limit.

@Abdul: I agree with Peter that necking doesn't necessarily have to occur at the center. Do you have experimental evidence to suggest otherwise for this material?

Regards,
Sandeep

• Abdul Malik
Subscriber

Hello peter,

Thanks a lot, sorry for replying late. As Sandeep stated, i also read in CAE associates blogs about Multi-linear theory and they haven'r mentioned about any limits but there is some sort of slope to be maintain while inserting the plastic values.

Actually, i first draw the geometry in AutoCAD then import it with either Spaceclaim or DM. I have tried to work with axis-symmetry option before but i couldn't turn out the model into axis-symmetry. If i am not wrong the above model you solved is surface element model not solid element model? Any advice when working with AutoCAD shall i made a 2D-model in AutoCAD and then import it into Sapceclaim and set to axis-symmetry?

One more thing i would like to ask when we apply symmetry to any body in DM it mean that Ansys apply full constraint (i.e boundary condition like fixed suport)  in that particular plane of symmetry?

Yes you are right but i mean the greater reduction of area should be somewhere around the central part of the specimen like in your above model?

Since the above model was not working so i started to work on full scale model and got some unexpected results as well will share if you guys would like to have a look into it. Peter i will try to reduce the model as per your suggestions and will shortly post it.

Furthermore, as we can see from picture of test data in first thread of this post the values of forces are given, if i want to use force as boundary condition which value i should pick up from the the force column to have the complete non-linear behavior. Shall i take the highest number in the force column (i.e. 25...kN) or the value at the fracture of specimen?

As i don't have the displacement values and i tried to compute it but the ansys results are not coinciding the calculated values.

One more thing how could we verify the results are correct means how you predict the results are right?

Many Thanks

Abdul Malik

• Abdul Malik
Subscriber

Thanks sandeep to inform Peter. As i mentioned above the greater reduction of area should be some where around the center of specimen. I have no evidence of this since i took this example from a book and it didn't mention about it.

• peteroznewman
Subscriber

@Sandeep, thank you for clarifying the limitations of plasticity material model, that it is only the temperatures that are limited to six values, and not the curve. It is disappointing that the Engineering Data program in Workbench doesn't enforce the six temperature limit as it will allow more than six values of temperature to be entered. This is why I wondered about inputting more curve points that it would use.  [EDIT: see Sandeep's reply below. 6 temperatures is limit for Bilnear, where Workbench does limit the input.]

• peteroznewman
Subscriber

@Abdul, if you create geometry for an Axisymmetric model, it must be in the XY plane, the axial direction must be the Y-axis and the radial slice must be on the positive X-axis.

In Workbench, right click on the Geometry cell and get properties. In the properties window, you must set Analysis Type to 2D before you attach the geometry to the Model in Mechanical. I am repeating what I said above but it seems you haven't been successful yet.

Once the model opens in Mechanical, you must click on the Geometry branch, and in the Details window the row 2D Behavior has a pull down and you must select Axisymmetric.

An axisymmetric model only needs one edge (say the bottom edge) to have a Y Component of Displacement set to zero and the whole model is properly constrained.

Apply a Y component of Displacement to the top edge. Request Reaction Force results on this displacement to plot the Force-Displacement curve.

Don't use a Force to pull on the top because there is no static equilibrium after the peak of that curve. The solver will stop with a convergence error and you won't plot the negative slope.

Plot the Total Strain against Displacement. Note that the last point in your Plasticity data is at a strain of 1.09 but the solver keeps going past that value. If that last value in the table represents the strain at fracture (elongation), then the graph below shows what value of displacement fracture would have occurred at.

If you look up that value of displacement on the Force graph, you can see the Ultimate Force. Values after that are not physical, but a result of the fact that the simulation doesn't include fracture. The solver just keeps going.

Regards,
Peter

• Sandeep Medikonda
Ansys Employee

Peter, that limitation only exists for the Bilinear models, not for the Multilinear models. When you use the Bilinear models, you will notice that Mechanical no longer accepts data after the 6th temperature. It has nothing to do with the TBDATA command.

Now, TBDATA can take more than 6 parameters (i.e., the parameters in each row for each temperature). So let's say, you want to use 3 Kinematic models in the Chaboche model.

The TBDATA command will store more than 6 parameters by increasing STLOC in that command to 7

```TB,CHABOCHE,1,8,3
TBTEMP,10
TBDATA,1,100,10,0.1,0.2,0.2,0.2
TBDATA,7,0.2
TBTEMP,20
TBDATA,1,200,20,0.1,0.2,0.2,0.2
TBDATA,7,0.2
TBTEMP,30
TBDATA,1,300,30,0.1,0.2,0.2,0.2
TBDATA,7,0.2
TBTEMP,40
TBDATA,1,400,40,0.1,0.2,0.2,0.2
TBDATA,7,0.2
TBTEMP,50
TBDATA,1,500,50,0.1,0.2,0.2,0.2
TBDATA,7,0.2
TBTEMP,60
TBDATA,1,600,60,0.1,0.2,0.2,0.2
TBDATA,7,0.2
TBTEMP,70
TBDATA,1,700,70,0.1,0.2,0.2,0.2
TBDATA,7,0.2
TBTEMP,80
TBDATA,1,800,80,0.1,0.2,0.2,0.2
TBDATA,7,0.2
```

Regards,
Sandeep

• peteroznewman
Subscriber

Thank you Sandeep for clarifying my understanding.

• Abdul Malik
Subscriber

Hello,

@Peter, thanks for the help. I succeed to form a axis-symmetry geometry. But there are some problems i am facing.

In below picture, the member start showing reduction at three points rather to show at one point as you showed in first thread. the displacement i applied is 35 mm though.

Any particular reason of this behavior?

the below is total strain vs displacement. still the program does not reaching the strain at the fracture point.

Is that possible these results are the causes due to some sort of geometry issues or meshing problem. i have checked the results by refining mesh as well.

I am also getting this message whenever i run the non-linear analysis. " large deflection on might effect the results {..]

Many Thanks

Abdul Malik

• peteroznewman
Subscriber

Solution is mesh dependent. Please show the mesh.

Can you make the geometry have a shorter length?

• Abdul Malik
Subscriber

yeah sure i will make it and post it in a short while. Below is the mesh the minimum element size is 0.5 mm.

I am also getting this message whenever i run the non-linear analysis. " large deflection on might effect the results {..]

Many Thanks

• Abdul Malik
Subscriber

Hey Peter it works, Thanks a lot for your help.

I am posting some results. which i got.

Is that possible in ansys to model rupture  of material ?

One more thing from the below graph that Ansys keep the stress constant when it reach the maximum stress value in Multi-linear theory table. but it surpasses the strain values.

And if you shed some light on the force convergence diagram. and recommend some readings to understand the force convergence diagram.

Many thanks,

Abdul Malik

• Sandeep Medikonda
Ansys Employee

Ok Nice, Thanks for sharing these results. Can you close off the thread by marking peters post as the answer so that it will help someone else in the future?

• peteroznewman
Subscriber

Abdul,

Here is a discussion on the Force-Convergence Plot. Your plot looks just about ideal.

When the strain reaches the last value in the Multilinear Plasticity table, it just uses the last value of stress with a zero Tangent Modulus and continues to stretch the elements as long as the element distortion doesn't stop the solver.

There is a switch called ekill that can take an element out of the model, but it is generally adequate to find the time in the load history when the Total Strain reached the Elongation value or the Strain at Break, and don't plot any data past that point.

I have a tutorial about ekill.

Regards,
Peter

• Abdul Malik
Subscriber

Thanks a lot Peter for your help, i am learning a lot new things.

Do we need to change some thing in Commands (APDL) section for  Ekill (i.e. any value of strain or some other parameter). ?

I am also following your tutorial regarding fillet welded connections. As the task is to model the high strength lap joints with longitudinal welds. The varying parameters are:

Length of longitudinal welds

Strength of base metals which is high strength steel (S460, S500, S700)

strength of welds relative to base material (G69,G42,G81)

Can we do this parametric study in one model?

Any recommendation would be appreciated.

Many Thanks

Abdul Malik

• peteroznewman
Subscriber

Abdul,

This topic is solved.

Please start a New Discussion to ask about a Parametric model to study length of welds etc after you have watched this tutorial for what to do in Workbench. Make sure to mention which Geometry editor you are using: DesignModeler or SpaceClaim, as they do design parameters differently.

You can also start a separate New Discussion on any issue you have implementing ekill after careful review of the tutorial.

Regards,
Peter

• Abdul Malik
Subscriber

Thanks Peter,

I will start the new session after completing my homework.

Regards,

Abdul Malik