Cancel
Showing results for
Did you mean:
Highlighted

ADVENCED SIMULAITON "DYNAMIC" PRESS FIT SIMULATION

Experimenter

Hi to everybody :-)
I am new of this forum but I hope that someone can help me. I would to study a dynamic deformation of hole and pin when the last one go inside.

It is possible with Non Linear Advanced solution to study it? My target is to see how the pin and the hole deform.

I created a mesh for both of 0.1 size, I assigned the material ( plastic ), I fixed the hole and I assigned a enforced displacement of 0,5mm to the pin to allow the traslation. How can I go on now? I have to create a "mesh meting" between them? According to you can I see a "dynamic" deformation of hole and pin´s mesh during taslation of the pin.

Thank you very much  if you give me some suggestions!!

2 REPLIES

Re: ADVENCED SIMULAITON "DYNAMIC" PRESS FIT SIMULATION

Creator

Hello,

your request seems to me suitable SOL 601 (-106 or -129).

As you wrote, you defined enforced displacement 0.5mm. So I reccomend yout o define this displacement in a tab, a displacement vs time, f.e.:

0 0

100 0.5

wher 100 is final time 100 secounds.

And define total time for SOL 601 100s with some increment, something like 5s, 1s...

Define proper parameters (Large displacement, ATS, Line search etc.).

Question is if you really want to simulate dynamic press fit - in this case it would be in SOL601-129, where 1 secound is not just a lenght of step but real time. If you simulate the press fit is time-independent (no inertia efffect, static friction only etc.), then SOL601-106 is enough.

Another option may be explicit SOL 701 but I would not start with it, let it as a backup

Good luck, Jan

Betreff: ADVENCED SIMULAITON "DYNAMIC" PRESS FIT SIMULATION

Phenom

Domenico1987,

additionally you have to define a contact definition between the partners. Source region / Target region have to be large enough to get the complete motion of pin fullfilled.

In Contact parameters you have to define large displacements and in SOL601 you have to activate large displacement and large strains.

NXSTRAT is the keyword you have to deal with STRATEGY PARAMETERS in Case Control.

ATS should be a good choice for automatic incrementation scheme (AUTO) for solution algorithm because time increment can be adopted to reqirements of solution.

If you are interested in the deformation states between 0 mm and maximum enforced displacement it would be good to define a time dependend enforced displacement as a table field and in TIME STEP INTERVALS a time table with an inital time increment of 1s and 100 Steps. Than you will get 100 intermediate steps from 1s to 100s.

As you could expect huge transfomation in local area it would be good to allow ATS to lower dot time increment drastically with having al large value for Smallest Time Step Size Number (ATSSUBD).

Keep in mind that SOL 601 is ADINA and not NASTRAN and there are a lot of other opportunities to improve solution.

Its not so easy to get a good result as you maybe expect. Therefore keep stamina.