cancel
Showing results for 
Search instead for 
Did you mean: 

Model different tensile and compression behavior

Builder
Builder

Dear World,

How can I model a material that has different tensile and compression limits. How cand I define a stress-strain table (curve) for such a material? All in NX10

Many thanks

Ionut

30 REPLIES

Betreff: Model different tensile and compression behavior

Legend
Legend

Hello Ionut,

 

you can specify the non-linear stress-strain-behavior in the material description. You have to define "NELAST" (maybe without "T") material parameters with positive AND negative Stress-Strain-Values. i.g. very small stress-value for a given strain value in negative range to build a nearly compression free material (thread)  or vise versa in positive range to simulate a contact like behavior.

Make sure, that you solve your problem in a nonlinear solution as SOL 601,106. Its every time the same :-)

I think thee specified Yield strength is set for the positive range.

 

To find more answers in documentation search for MATS1, NELAS(T), TABLES.

I am not at the office at the moment, therefore I can't name you the correct point in material description.

 

One hint at last - If you set strain values in your table less than the real values occuring in your simulation NX maybe tries to create a rupture in your part. But I think there is a parameter/switch to control this extrapolation behavior.

 

Best wishes.

Michael

Betreff: Model different tensile and compression behavior

Builder
Builder

Hello Michael,

Thank you again. Here in Romania we have a saying: someone gives you a finger and you take the whole hand. To demonstrate that it is correct, I will ask [you] another question:

If I choose not to extend the stress-strain curve, as soon as the stress in an element goes beyond the ultimate stress limit, the element is removed from the structure. And my problem is: I presume the stress is the Von Misses, which is a positive value, but I am interested in an area where the stress is negative and the material has different compression and tensile ultimate stress limits (that's why I was asking how to define a stress-strain curve with values in the third quarter). Is it possible to tell NX to eliminate elements when the maximal stress (positive or negative) goes beyond the limit?

Many thanks

Ionut

Betreff: Model different tensile and compression behavior

Builder
Builder

Hello,

Following your advice, I have used the NELAST material. It works, up to one point. That is, for an imposed displacement of 60 mm, with NELAST NX do not converge, while, in the same conditions, with PLASTIC, it works! I do not understant why.

Another problem:

For an imposed displacement of 60 mm, with PLASTIC material, I get in the 06 file the following message:

 

     ***WARNING: Large strain kinematic formulation is not applicable to all elements (PID= 10).

This one is confusing for me, since I am using the large strain formulation!

 

     ***WARNING: Contact surface compliance not used for contact group 101.

                 Contact compliance can improve the solution accuracy and convergence rate.

     ***WARNING: Contact surface compliance not used for contact group 102.

                 Contact compliance can improve the solution accuracy and convergence rate.

These two are not very important (as far as I know)

 

     ***WARNING: No element connection for node 613 directions 4, 5, 6

     ***WARNING: Similar warning suppressed for 10104 other nodes.

     ***WARNING: Nodal degrees of freedom without element

                 connection have been fixed for data input file.

These 3 lines are related with the fact that all solid elements have only translational DOF? I presume this is not a very important warning

 

Also in the f06 file, I got the following message:

 Over-distorted element, DET=-3.8498268E-01  GROUP=      9  ELEMENT=      1464

 Over-distorted element, DET=-7.2584116E-03  GROUP=      9  ELEMENT=      1467

 Over-distorted element, DET=-8.7679512E-01  GROUP=      9  ELEMENT=      1468

 . . .

 ...

 ELEMENT PID NNUMBER:         9      NUMBER OF INACTIVE ELEMENTS:        25

 

 THERE IS A TOTAL OF       45  OVER-DISTORTED ELEMENTS. THE DISTORTION MIGHT BE

 DUE TO EXCESSIVE STRAINS (IF LARGE DISPLACEMENT/SMALL STRAIN FORMULATION IS

 USED) OR SLIVER ELEMENTS IN THE ORIGINAL MESH.

 

The over distorted elements are located in the encircled are in the attached image. What can I do to avoid this message? I also attache an image with one element that becomes distorted

 

And finally, I want to apply an enforced displacement of 45 mm and then relax to 20 mm (to see what residual stresses and displacements remain). If For the enforced displacement I use the table:

0,0

1,45

1.4,20

and Number of stepts 520, with Time increment 0.0025,

I get only the situation for the 45 mm displacement!

Many thanks

Betreff: Model different tensile and compression behavior

Legend
Legend

Hi,

 

now you are at a stage where I'm also fighting with :-)

I also get distorted elements and I'm not able to realize how to get rid of it.

 

But answering sequentially:

1. Keep in mind that non-linear "PLASTIC" and Non-linear "NLELAST" are quite different in unloading because with NLELAST stress-strain-curve ist still active an with "PLASTIC" unloading material law will follow a straight line to zero  in stress-strain-behavior.

 

2. Large Strain kinematic formulation problem is also not clear for me and I did ask here in this forum but got no answer. May be its a standard warning and not relevant in that solution.

see

http://community.plm.automation.siemens.com/t5/NX-CAE-Forum/Unclear-warning-in-SOL601-106/m-p/344125

 

3. Contact surface compliance problem here is caused from my point of view by large strain-problem. Your elements degenerate and it's really equal if you reduce your solution time steps or such things. May be you could adopt your contact parameters in softening contact behavior but its only a guess.

 

4. Degrees 4 -6 come from solid elements an the waring is a standard warning.

 

5. Over-distorted elements with negative jacobian determinats comes from your degenerated elements.

I have such elements too and do not know what to do.

May be its better to increase integration order because its looks for me like hourglass deformation. But its only a guess.

 

see my question thread in forum:

http://community.plm.automation.siemens.com/t5/NX-CAE-Forum/SOL601-106-ATS-with-contact-yields-in-la...

 

6. Time-Steps 0 -1 - 1.4: Here is the question, Where do you control your time step behavior?

What kind of non-linear solution scheme do you use (ATS, TLA-S, ...)?

If your time step description in case control is not adopted to 0 -1.4 it will every time solve only up to 1.0 independetly what s your definition in enforced displacement. Try to define your total enforced displacement behavior in 0 -1 s in modifiing your table to

0.00,   0.0

0.75, 40.0

1.00,  20.0

 

Furthermore 520 x 0.0025 only yields 1.3 s.

 

Finally did you try to define different stress limits in material strength card for Tension (ST), compression (SC)?  I do not know the exact usage of these values but it could be a chance.

 

 Edit: It does not have an effect

" Remarks related to SOLs 601 and 701:

  1. GE, ST, SC, SS, and MCSID are ignored."

Best wishes.

Michael

Betreff: Model different tensile and compression behavior

Builder
Builder

Hello,

Thank you again. Here are my comments:

1. O know how the unloading occurs in the two cases. My problem is that I only impose a prescribed displacement of type: 0,0;  1, 60 and the NELAST do not converge. I do not do any unloading!

 

3. What do you understant by "softening contact behavior"?

 

6. I am using ATS. I have also tried 0,0; 0.75,45; 1,20. In this case, I get the 20 mm deformation, but very quick. It do not looks like it calculates for 45 and then unloads!!!

 

I will try to use higher order elements

Regards

Ionut

 

Betreff: Model different tensile and compression behavior

Builder
Builder

I have once again tried the sequence: 0,0; 0.75,45mm; 1,20mm. It looks like it calculates only from 0 to 20, ignoring 45mm! I am totally confused.

Ionut

Betreff: Model different tensile and compression behavior

Hi,

 

With reference to your analysis, try to reduce the load increments, your problems may come from too large diferences between the subsequent steps.

 

If you would like to get rid of elements which exceeded certain strain (last point of your stress-strain curve) read about XTCURVE entry in NXSTRAT:

 

XTCURVE:

Indicates whether the table in TABLES1 entry is extended by linear extrapolation of the two last points. (Integer; Default = 1) 0 – Table is not extended. This option may be used to allow element rupture at the last specified strain value. 1 – Table is extended Note: XTCURVE is only applicable for the multilinear-plastic material model.

Betreff: Model different tensile and compression behavior

Legend
Legend

Hi,

 

what happens if you adapt your global time step parameters to simulate a total time range from 0 to 0.75 s without changing your enforced displacement control ({0.0,0.0}; {0.75,45.0}; {1.0,20.0}).

I would expect a total displacement of 45 mm. Is that true?

 

Best wisches,

Michael

Betreff: Model different tensile and compression behavior

The SOL106/601 is a static solution, so there is no influence whether you will simulate your loads in 1sec or 20sec. The results will be exactly the same. Important is to specify your enforced displacement / force within the same 'time' as it is specified in NXSTRAT.

incrementation of the load is dependent on the time step you will specify in NXSTRAT and the incrementation strategy (ATS... etc).

 

Here you have quite good explanation: SOL 601-106