## General Mechanical

#### pressure load that depends of the contact between solids

• Mattias Scheffler
Subscriber

Hello,

I am running a transient, axisymmetric simulation with pressure loads and contacts between 2 deformable solids.

What I am currently using is a ramped pressure step that is applied on a surface (see first attachment).

However, I would like this pressure to drop locally to zero where the surface is in contact (see 2nd attachment). Ideally, the transition between the "nominal" pressure and zero pressure would be smooth. Of course, the load has to be updated at each time step.

My first guess would be to compute the distance between the surfaces for each node and compare it to a treshold. Unfortunately, I have very little experience with APDL and user defined functions so I do not know where to start.

I would like to know if there is a relatively simple way to implement this, or a good tutorial that I could use as a basis to build my feature.

Best,

• peteroznewman
Subscriber

Hello Mattias,

You will find this tutorial shows you how to do what you want.

https://courses.ansys.com/index.php/courses/structures-in-industrial-equipments/lessons/analysis-of-an-o-ring-seal-lesson-3/

Regards,

• Mattias Scheffler
Subscriber

Thank you for the link. Unfortunately, this tutorial does not include any pressure load. However, i did look at some other O ring studies like this one :

https://tarkka.co/2019/04/11/overview-of-hyperelastic-fea-of-o-ring/

It uses what is called a fluid pressure penetration load. It is a pressure that spread from defined start points, unless contact is active. Some documentation exist in the "contact technology guide"

It can be applied by using the APDL command SFE. I am using this snippet to apply the load on the surface (named selection "pressure") from the start points (in named selection "StartPoints") :

kbc,0 ! I want this pressure to be ramped
cmsel,s,Pressure
esln,s,1
esel,r,type,,cid_1
sfe,all,1,pres,,6e5
ALLSEL

cmsel,s,StartPoint
esln
csel,r,type,cid_1
sfe,all,2,pres,,6e5
ALLSEL

On overall it is working neatly. One problem remains : My flexible body has some self contact (not shown in the previous figures). It is defined separately from the contact with the other body. Fluid pressure start from this self contact although it is not specified as a starting point. I will update this post if I find the answer.

• peteroznewman
Subscriber

I'm glad you found a good tutorial.  I meant to send you this link which has the APDL code for fluid pressure in part 3.

#### (3) O-ring seal with fluid pressure

https://courses.ansys.com/index.php/courses/structural-nonlinearity/lessons/homework-quizzes-simulation-examples-nonlinearity-lesson-4/

If you can show an image of the self contact, that would be helpful. Why don't you want the pressure removed from the region of self contact?

• Mattias Scheffler
Subscriber

Here is a picture of fluid pressure where arrows indicate the location of the start point and the self contact area. Pressure should propagate from left to right as elements get out of contact. However, pressure is also applied on the right area directly at the start, which should not happen (because no start points are located there).

I did plot the fluid pressure with only contact between solids selected, which gives the result that I want :

Then I switched to self contact and I do get this :

I think that the commands "cmsel,s,Pressure" and "esel,r,type,,cid_1" select all the contact elements that are in the "pressure" named selection. To solve my issue, I should only select the correct contact elements.