Cancel
Showing results for 
Search instead for 
Did you mean: 

Solution 601,106

Builder
Builder

Hello,

I am struggling  with the following problem:

I am trying to model, using sol 601/106 the flattening of a pipe (see the attached file pipe.jpg ). The problem is that although I am increassing the time interval of the applied displacement, I always get practically the same results (see file pipe2.jpg). It is like NX stops in the same place. I also mention that I do not receive any message about errors!

Many thnaks

IL

9 REPLIES

Betreff: Solution 601,106

Legend
Legend

Hi,

 

I think you have to describe something more of our problem, because if something is wrong, the question ist, what do you want to do, what is the way you choose to solve our problem, what kind of results do you expect and THEN what is wrong, therefore here some questions to help to encircle the problem.

1. What ist the enforced displacement or load, do yout put on your model?

2. What kind of solution sheme did you use?

- Case Control => Strategy parameters: default, ATS, TLA, TLA-S

3. Which way to define the time characterisitc did you choose?

- Case Control => Time Step definition: TimeSteps

4. What is the method to define your time dependent enforced displacements?

5. Do you expect large deformations or strains and did you activate the right parameter option?

6. What kind of contact parameter did you select?

7. Did you already tried to solve it in SOL101?

 

May be it helps yourself to get more information about your problem.

 

Greetings,

Michael

Betreff: Solution 601,106

Builder
Builder
Dear Michael,
Thank you for you answer. Here are my answers to your questions:
1. I wand to simulate the flattening of a pipe. In order to do that, I have
prescribed displacements on the rigid upper body (modeleld with shell
elements) - see displacements.jpg
[image: Inline image 1]
2. I am using ATS
3. Here I use Case control -> Time steps intervals -> Number of time steps:
10000, Time increment 0.01 (to cover a maximum of 100 seconds)
4. I am using a table, starting at 0 seconds, with 0 displacement, and
reaching 50 mm at a time that I am still looking for
5. I am using large strain approach
Hoping my answer helped you understand my problem
Sincerely yours
Ionut


--

Betreff: Solution 601,106

Builder
Builder

Dear Michael,

Thank you for you answer. Here are my answers to your questions:
1. I wand to simulate the flattening of a pipe. In order to do that, I have prescribed displacements on the rigid upper body (modeleld with shell elements) - see displacements.jpg bellow:
Inline image 1
2. I am using ATS
3. Here I use Case control -> Time steps intervals -> Number of time steps: 10000, Time increment 0.01 (to cover a maximum of 100 seconds)
4. I am using a table, starting at 0 seconds, with 0 displacement, and reaching 50 mm at a time that I am still looking for 
5. I am using large strain approach
6. For the contact, see the attached file (contact.png). The settings are used for both contacts, the top and bottom one
7. No, I did not tried to solve the problem with solution 101
Kind regards
Ionut

Betreff: Solution 601,106

Legend
Legend
Hi,

all right. I think you do not understand the meaning of time in your
problem correctly.

In your case and Solution 601, 106 span of time is not so relevant.
If you want to press down the tube you have to define a time period in
which you want to do it so.
That means you have to build a time table as a collection of pairs of time
step and enforced displacement value to describe a time characteristic for
your problem.

You try an analysis with 10’000 time steps which is for a first check
really much. Anyway, if you have a time increment of 0.01s to reach 100 s I
think the enforced displacement shall reach may be a quarter of the
diameter of the tube.
Therefore your time table can be:

0, 0
100, 1

That time table you can use in your displacement definition an for
magnitude you use d/4.

Then after 100 sec your displacement will be d/4.
May be reduce your DeltaT and your number of time incrementation (time
steps).
If your solution works try to increase maximum deformation and all the
other time parameters. The time table can be unchanged if total time as the
product of time increment and time steps does not change, too.

Try this way. You will find after solving for all your time steps your
desired results.

Best whishes.
Michael

Betreff: Solution 601,106

Builder
Builder

Dear Michael,

Sorry for replying so late.

Regarding the enforced displacement and the time table, if I correctly understood, you suggested that the table acts like a multiplyer of a displacement. I have used Enforced displacement (see Enforced1 and 2) and it seems that the table provides absolute values (expressed in mm). Am I wrong?

Apart from that, when running the analysis, I am using the general settings:

- Number of time steps:10000

- Time increment:0.01

- Skip factor for output:1

With these, using the following settings for the enforced displacements, I got:

1. Time 0,0;100,1 -> max displacement: .01

2. Time 0,0;100,5 -> max displacement: .05

3. Time 0,0;10,1 -> max displacement: .1

4. Time 0,0;10,5 -> max displacement: .5

 

With - Number of time steps:1000 (the rest unchanged) and Time 0,0;10,5 -> max displacement was also: .5

I a confused!

many thanks in advance

Ionut

 

PS. I have also attached the f06 file for the last case

 

 

Betreff: Solution 601,106

Phenom
Phenom
Are you not trying to enforce a 50mm! So it does not matter whether you are applying in 1s or 10000s. I am assuming here a non linear static analysis. So "time" is pseudo-time. not real time. The analysis will stop once the 50mm enforced disp has been reached (assuming it can).
Production: NX9.0.3.4, NX10.0.2.6
Development: VB.NET (amateur level !)

Betreff: Solution 601,106

Builder
Builder

Dear Michael,

With your help I managed to get a solution. Thank you. Now I have two other questions:

1. Is it possible to define some sort of a sensor to stop the analysis when the stress in a certain point (node) reached a certain value?

2. How can I control the way elements where the stress exceeds the strength limit behave?

Many thanks in advance

IL

Betreff: Solution 601,106

Legend
Legend

Hello IL,

 

that are two very interesting questions but I 'm not able to answer in a meaningful way.

I suggest you post these questions as a new thread.

 

As a hint for q2, may be it helps:

To control the nonlinear behaviour of elements you can set different yielt function criterias i.g. in description for MATS1. May be its what you look for.

 

Best wishes,

Michael

 

Betreff: Solution 601,106

Siemens Phenom Siemens Phenom
Siemens Phenom

There is no ability to stop a SOL 601 solution based on a stress limit.

 

By default, multilinear plastic material properties defined via MATS1/TABLES1 will be extrapolated beyond the last point defined in the table. If you set XTCURVE=1 on NXSTRAT, elements exceeding the last strain value in the table data will be considered ruptured and will be removed from the solution.