Learning Forum

[Gijoys4v]

I tried to solve a problem , but end up with some issues ; please help me to proceed. figure below shows what i have done

[peteroznewman]

Answered in this post.

Please ask the question only once.

[Gijoys4v]

 

 

I have 3 solids kept one over the other which is in bonded contact. Left face of all solids is fixed (zero displacement in all direction) in the first time step it is cooled from 1000k to 500K. In the next time step(2^nd), I have to fix the left face of the solid and at the same time step a displacement have to be provided from the right side of all solids. (at the same time the top and bottom face of the assembly is restricted to move in upward and downward direction, this is made by giving displacement constraint). This is the problem I have to solve. But it shows DoF warning as I said earlier.

 

[Gijoys4v]

I have seen your answer. all solids are of different dimension(thickness). symmetry cannot be considered

[peteroznewman]

The constraint pattern doesn't make sense.

When material is cooled, in shrinks in all three directions, I will just talk about 2D for simplicity, with X-axis horizontal and Y-axis vertical.

For a model of a part that is sitting on a table, it is valid to pick the left edge to have X = 0, and the bottom edge to have Y = 0 so when the temperature cools, the part gets shorter in the X direction and shorter in the Y direction.  It is free to do that with the above constraints.

For a model of a part that is sitting on a table, is not valid to pick the left edge to have X and Y = 0, and the bottom edge to have X and Y = 0 because when the temperature cools, the bottom edge of the part cannot get shorter in the X direction and the left edge cannot get shorter in the Y direction.

If the table is a special steel that has a very low CTE and the part is glued to the table and the Young's modulus of the part is 1000 times smaller than the Young's modulus of the steel table, then it would be valid to model the bottom edge of the part with X and Y = 0.  If the steel table was machined to provide a pocket for the left edge of the part and that was also glued, then it would be valid to have the left edge have X and Y = 0. When the part is cooled, the material will shrink and stress will build up in the part due to the constraints that prevent two edges from shrinking.

Is the part glued down to a substrate that has a zero CTE and is practically rigid compared with the part?  Or is the part sitting on the table?

What is the physical mechanism that creates a displacement of the right side of the part in time step 2 if the right side was free to move in time step 1?

What is the physical mechanism that prevents displacement of the top of the part in time step 2 if the top of the part was free to move in time step 1?

[Gijoys4v]

in the above problem, in the first time step the bottom and above part is not supported or fixed. it is only fixed at the left side. sothat during cooling in the step1, it can shrink in x direction and y direction. cooling is provided only in the first time step. so in the first time step it will be acting like a cantilever beam(of three layers) which is cooled from 1000K to 500K. After the cooling process in the first time step I have to apply a displacement to the right direction inoorder to findout the stress induced in the bodies. That is why I had given a displacemnt in the second time step. During this process(means the displacemnt applying step), I dont want to move the bodies in any other direction othertahn the applied displacement direction. Thats why I had given support on the top and bottom in the second time step. 

is my problem correctly defined?

 

[peteroznewman]

I have to apply a displacement to the right direction in order to find out the stress induced in the bodies

No you don't.  You just insert a Stress result into the Solution branch of the outline.  Cooling a block of uniform material sitting freely on a table induces zero stress. It is only a layered structure with different CTE that will induce stress when cooling.

If you want your layered structure to be supported in a cantilever beam way, then you can hold the left edges fixed while cooling. You will get some localized high stresses due to the constraint at the left edge that would not be there is the left edge was not fixed.

Or do you mean that after cooling, the layered structure wants to bend, and you want to straighten it to get the stress in the layers after straightening?

[Gijoys4v]

the layered structure is having different CTE. I want apply a tensile load(in the form of displacement) to the right

---

> after cooling the structure.

[peteroznewman]

In the discussion titled https://forum.ansys.com/forums/topic/applying-strain-obtained-to-next-analysis/
you were asking about bonding layers at one temperature, then cooling, which induced bending in the layered structure.
You wanted to add a third layer at a lower temperature then cool it some more.

So in this analysis, are you bonding all three layers at 1000 K? When it cools to 500 K, the left-end cantilevered structure will bend if there is no other loads or constraints at the right end.

I understand you want to apply a tensile load at the right end. There are several ways to do that and it depends on how the structure is controlled at the right end.

1) Force in the X direction.

2) Rigid encasement at the right end used to apply an X displacement only, leaving rotation and Y displacement free.  This is like a Pinned constraint.

3) Rigid encasement at the right end, and apply an X displacement of a point only, rotation and Y displacement are set to be zero.  This would be like the rigid encasement is fixed to a linear slide that only moves in X.

#1 and #2 are similar, except one applies the force, the other applies the the displacement.  #3 is different from #2.

I don't understand why you would want to constrain the entire top and bottom surfaces. Is the layered structure in a clamp over the full length?  That doesn't make sense if you are pulling on the right end.

[Gijoys4v]

I have two plates say A and B with different CET. First I have to coat A on B. That I done by simply placing A on B in workbench. And I provided bonded contact between those two. Next I have to cool the system to 500K from 1000K. That too I done simply. Next I have to electroplate another material say 'C' on A and B at temperature 500K. I don't know how to introduce a new material at this step. Even though if I introduce the new material at this step, it may not cover the entire material A and B as it was already deformed due to the temperature reduction. So what I did was at the beginning itself I made all the layers and system will be like 'CABC'. Here I made the contact between CA and BC dead and I made it alive only when the system reaches 500K. The problem is when I run the solver, it get crashed. I think the problem may be due to the lack of constrain in the element C. As B is in contact with A, there was no constrain problem for A and B. If I give a constrain or support to the 'C' at temperature from 1000 to 500K whether it may affect the answers. Then the whole system I have to cool to 300K.Then I have to apply a deformation displacement (not allowed to give force)to one end of the system making other end fixed. Aim was to find out the stress in the system after all these process.

[Gijoys4v]

I don't want the layered structure to bend

[peteroznewman]

What physically prevents the layered structure from bending?

[Gijoys4v]

Actually I mean, Iam not inducing a bend. Or giving any boundary condition to induce the bend.

[Gijoys4v]

In my previous post, I tried to elaborate my problems. Please check

[peteroznewman]

It's best to clearly explain what is physically happening, and try to build a model to simulate that.

When the temperature changes for a structure with layers of material with different CTE, it wants to bend.

If you apply axial tension to a structure, some of the bend will straighten. The higher the tension, the less the bend, unless the tension is applied eccentrically, then the tension can induce bending.

If you clamp the full length of a bent structure down onto a platen, it will straighten.

Are you only applying tension, or are you also applying a clamping force to press the structure down to a flat platen?

[peteroznewman]

I want to distinguish between items you may have added to the model because you thought it would help the model to converge from items that represent a condition physically present in the experiment.

[Gijoys4v]

Have you seen the problem I tried to define elaboratly( please check my 4th previous post above this ).

In that C is copper and A & B are alloys of different CET which is having high varaition.

[peteroznewman]

Yes, I saw that. I want to know physically, how the sample is held by fixtures in the lab.

What physical objects touch the sample?  Is there a hard surface below the sample and a hard surface above the sample?  If so, is there a downward force on the hard surface to compress the sample through the thickness.

What is the geometry of the additional bodies that create the tension? Show a sketch.

[Gijoys4v]

[peteroznewman]

Thank you for the figure.  That tells me that the answer to an earlier question is #3.

3) Rigid encasement at the right end, and apply an X displacement of a point only, rotation and Y displacement are set to be zero.  This would be like the rigid encasement is fixed to a linear slide that only moves in X.

It also tells me the the answer to this previous question: Is the layered structure in a clamp over the full length?  The answer is no.

That tells me that there should be no constraints applied to the top and bottom surfaces of the layered structure at the end of the simulation.

You said "Here I made the contact between CA and BC dead and I made it alive only when the system reaches 500K. The problem is when I run the solver, it get crashed."  If the left edge of C is Fixed, just like A and B, then the solver should not crash. Please attach a Workbench archive to look at that problem.

New question:  Is the deformation of the sample a specific value?  What is that value?  How long is the sample?

One idea is for bodies A and B which are fixed at the left end, to have a zero displacement at the right end when the temperature is 1000K.  As the temperature is reduced to 500K and then 300K,  a tensile stress will develop in the material.  The strain in materials A and B will be CTE*700K. That is equivalent to leaving the right end free, allowing the length of the sample to shrink as the temperature drops by 700K and then applying a deformation to pull it back to its original length. If you want more or less deformation, then you can just change the Displacement BC at the right end after the last step.

[Gijoys4v]

You told me:  If the left edge of C is Fixed, just like A and B, then the solver should not crash. 

but I have doubt;- if we fix one edge of the C fixed at the entire cooling process whether the fixed end will induce some stress in the C during its cooling. So whether it may affect the final answer.

Next doubt:- From 1000 to 500K there is no contact between CA and BC. so the fixing of one end will help to avoid the constraint problem while cooling. But at 500K I made the contact alive. So there is the contact between CA and BC. so whether there is the need of the fixed end of C again in other proceeding step. So whether we can add inplace of fixed end for C, a displacement constraint we can switch OFF this constraint after the first step(ie the cooling of BA from 1000 to 500K)

Step 1 :- cooling of AB from 1000K to 500K.( at this time a displacement constraint is given to the vertex of C. )

Step2: - Making contact between AC and BC alive(at the same time the displacemnt constraint given to C is inactivated)

Step 3:- Cooling of whole system i.e CABC from 500K to 300K

Step4:- making the displacement( which id 5e-2mm) activate at the right end and  at the same time to the other end the zero displacemnt is activated.

whether it will work. During the solution it went to an error. the errors are follows

1)The solution was executed using restart information

2)The solver engine was unable to converge on a solution for the nonlinear problem as constrained.  Please see the Troubleshooting section of the Help System for more information.

3)The solution failed to solve completely at all time points. Restart points are available to continue the analysis. 

4)The unconverged solution (identified as Substep 999999) is output for analysis debug purposes. Results at this time should not be used for any other purpose.

5) Large deformation effects are active which may have invalidated some of your applied supports such as displacement, cylindrical, frictionless, or compression only.  Refer to Troubleshooting in the Help System for more details.

6) Although the solution failed to solve completely at all time points, partial results at some points have been able to be solved.  Refer to Troubleshooting in the Help System for more details.

 

7) Contact status has experienced an abrupt change.  Check results carefully for possible contact separation.

 

But the solver ran upto 1st time step. ie it get cooled to 500K. the problem begins when I activated teh contact and inactivated teh constrain oF C.

 

The length of specimen is only 10mm

 

[peteroznewman]

Regarding your first doubt, there will be a local stress riser at the two ends of the sample caused by the Displacement constraints. The strategy to handle that is to create results that exclude a few elements at either end and look at the stress only in the center of the sample.

For the second doubt, yes, you can use Displacement constraint on the left end of C that you can disable after the contact has been established, but since the left end of AB is not moving, it probably doesn't matter if C has a constraint or not after the contact is established.

Steps 1-4 look reasonable.

This model is a big improvement over an earlier model which immediately flagged a DOF error and would not run at all. At least this is running. Now all you need to do is overcome the convergence issues.  There are many posts on this site for how to do this.  The method includes:

• a) Under the Solution Information folder, change the Newton-Raphson Force plots from 0 to 5.


• b) Look at the Newton-Raphson Force plots to see which elements have the highest Force imbalance.


• c) Under Analysis Settings, set Auto Time Stepping On and use a large number of Initial and Minimum Substeps, like 100.


• d) On the Solution Information, look at the Force-Convegence plot and see if more than 26 iterations would have allowed the solver to converge. If that looks to be the case, then insert a Command Object with the command NEQIT,50 to force the solver to keep iterating for more than 26 iterations.


• e) Look at the displacement of the partial solution to see if anything is going wrong.


• f) Look at Contact Status results to check the contacts are working along the full length.

[Gijoys4v]

You told me:- but since the left end of AB is not moving, it probably doesn't matter if C has a constraint or not after the contact is established.

But why the left end of AB cant move. I havent fixed the left end of AB. Only I have given displacement constraint to C on its one vertex. AB is already having a bonded contact between each other. So whether there is any need of giving additional constraint to AB

[Gijoys4v]

https://forum.ansys.com/forums/topic/time-stepping-issue/

[Gijoys4v]

can you check the above link. It is an issue I am facing in time stepping

[Gijoys4v]

I want to solve a problem using Ansys work bench. The problem is as follows.

Suppose there is three plates (say A, B, C) which is made up of three different materials and different coefficient of thermal expansion.

1) First I have to coat B on A at 1000K and cool it to 500K.

That I did by placing B on A and given bonded contact and cooled it to 500K from 1000K.

2) Next I have to coat C on A and B at 500K.

So what I did was, I already made C and placed it on A and B. Then I made the bonded contact between A and C, B and C alive only at the required time step.

3) Next I have to cool the whole system to 300K and then fix one end and apply displacement to other end

I did this in two methods. First I did the analysis in same analysis window and I obtained an answer like this from the 4^th time step (Actually I am applying the displacement from 4^th time step)

Next I stopped the process at 4^th time step and transferred all the datas to next setup and applied the same boundary conditions and I got an answer like this.

in the second method one can see that, there is a gradual stepping occuring. which is not happening in first case. Why is it so. Actually I want to apply the load continuosly.

 for both I had given the same displacement boundary conditions and value

Please help

[Gijoys4v]

anyone came up with this issue? if solved please reply