Tube inside tube contact

andyecho

Hi
my first post
I'm trying to model a square tube inside a tube with a load on the outside tube and displacement supports at either end
modelled in freecad then partioned in salome to allow me to extract faces

contact faces defined - stiffness = 10 x 200 / 0.004 = 500000 Gpa

however when I run I'm getting "Number of contact spring elements=0"

result is as a cantilever beam with no restiction from the inside tube

Sure it's probably something simple - this is my first go at contact

Mecway 12 with Paradiso solver

Any pointers please

Victor

A couple of problems:

A ) The contact won't be working because one surface is on the outside of the outer tube, instead of the inside.

It probably happened because when you select a surface in the geometry view, it only allows one side to be chosen, even if it looks like both. That's currently a limitation that often causes this kind of problem, unfortunately.

It can take a bit of gymnastics to change and it will lose associativity with the CAD model. If you don't mind allowing contact on the entire length of the tube, then:
1) Right click the Partition_1 component and click Hide all but this.
2) Click the Partition_1 component to select all its elements.
3) Edit -> Select faces
4) Edit -> Invert selection
5) Right click Components & Materials and click Show all.
6) Use the selected inside faces in the contact or put them into a named selection.

It might be slow to solve because of the large contact surface. If you want to limit it to the short section, perhaps use the Cutting Plane slider to hide the rest of it and select the faces manually.

B ) Both parts are insufficiently constrained to prevent rigid body motion, so that could cause it to fail. Perhaps change the displacement constraints to fixed support if that's appropriate.


C ) I notice the Partition-1 is linear elements. It's usually better for accuracy, speed, and contact convergence to use quadratic elements. It's OK to leave it how it is though.

andyecho

Victor

Thanks, I think I could have looked at this for ages and not spotted the incorrect surface. I got a smaller version to work first time with the displacement support. I used linear elements to reduce solution time.
Running the final version with quadratic element groups extracted using salome - to allow better component definition - the displacement correection and residual force seesaw after 15 iterations no solution after 60. Is this generally due to excess stiffness

Victor

I'm not sure what the convergence graph looks like for excess contact stiffness, but it could be that. However, the contact stiffness here looks reasonable (10 E/t).

Did you add more constraints to both parts? If not, then I wouldn't expect to get a correct static solution since the bending force and frictionless sliding may tend to push the two tubes apart. If you do need to allow the ends to slide a little, you can constrain them through weak springs such as elastic support.

The next version (13) will allow selecting the back faces of surfaces in the geometry so this kind of thing will be much easier.

Victor

I've tried to solve it and, like you say, it still didn't work. It does look like the contact stiffness might be the issue because it can solve with small loads before contact occurs. I got it working on a with a coarse mesh by making these changes:

• Turned on quasi-static
  
• Changed force from -6250 to -6250*t^3. This keeps it very low when the contact first occurs while still ending up with the same final force.
  
• Increased the maximum number of iterations from 60 to 100 by adding the following to CCX -> custom model definition:
  

*CONTROLS,PARAMETERS=CONTACT
,,,100