Ansys frictional contact - convergence problem

[zizou]

Hi, I am writing to you to ask for help.
I have a problem with the contact "Frictional". I'll show you screenshots of my settings and program the console errors. Everything will be shown in the screenshots. The problem is that between the beams and the top element and the bottom element is Frictional which causes a lack of convergence. I do not know how to deal with all of this, especially since this is a problem in my thesis. I need to find out what are the internal forces in the joints of these elements.

Model presents powered support, and support beams represent an extreme variant of contact with rocks.

here are screens:
http://postimg.org/image/n525lay2t/
http://postimg.org/image/9qp2p9ret/
http://postimg.org/image/lej4jtgjp/
http://postimg.org/image/iunhppszp/
http://postimg.org/image/lngp9qtc5/
http://postimg.org/image/f8d2zbx8l/
http://postimg.org/image/vw96fkhdx/
http://postimg.org/image/f5xsq8iyt/
http://postimg.org/image/gv6vyayo5/
http://postimg.org/image/57cu3r9j9/
http://postimg.org/image/71polhwjp/
http://postimg.org/image/di38pbuh1/

 

[Greg Bernhardt]

I'm sorry you are not generating any responses at the moment. Is there any additional information you can share with us? Any new findings?

 

[koolraj09]

Hi,
As a first step you can try bonding the contacts instead of frictional. If results look ok...then you might switch on the frictional settings. Try "weak springs" option while attempting a frictional run...

 

[zizou]

when i use bonded contact everythink looks ok. i get results, anyone happy. but... could it be "update stiffness" set on "never" cause the problem with convergence ? i will try set "update stiffness" to "each iteration" and will see if it works.

 

[zizou]

how to change integration function to full integration ? is this about changing frictional to bonded ?

 

[Mech_Engineer]

I'm not on as much as I would like these days, but I just randomly stopped by and saw this post. In case you haven't received the feedback you need, I'll give you the same advice I've posted in the past:

• Pay Close attention to your mesh density in the sheet metal being bent, as well as in the contact conditions that are moving it. The mesh should be of similar size on both sides of the contact, you can use a "contact condition mesh refinement" to make sure this happens.
• Make sure you use an "Augmented Lagrange" formulation for the contacts between the sheet metal and press. This formulation will work best with sliding conditions.
• As a start, make the contact condition between the sheet metal and press frictionless. Once you get it to converge, then you can think about considering friction.
• Make sure your contact condition forces update every substep, and split your problem into MANY substeps (on the order of 100).
• Make sure you have accurate material data for your sheet metal, especially into the plastic deformation region which you'll be probing specifically.
• Remove the "frictionless supports" which are nonlinear boundary conditions that I suspect will cause you undue grief, and replace them with fixed displacement conditions (0 displacement in axis perpendicular to surface).

That's a good start anyway... I'm not sure of your limitations using ANSYS Academic (the mesh is limited to what, 10K nodes or something?), but hopefully this will start getting you in the ballpark.

Generally speaking a lot of this advice is relevant to you as well. Split your problem into lots of small substeps (or even outright load steps), make sure the contacts updates every substep, and pay close attention to your boundary conditions. Good luck.

 

[zizou]

Hi, thanks for your all replies, i found a way to converge - i add normal stiffness with 0,1 value to all contacts, even to bonded. I really don't knew if it was exactly this setting because i change a lot other values, but i think it was the certain setting. Thans again a lot!