Setting up contact in WB environment

[maheshh]

I have worked with contacts (mostly small displacement) in the classic environment and have recently moved to WB. There seems to be something that I am doing wrong as none of my contacts seem to work (althought these problems I am working on are large displacement). So I setup a simple 2-link problem to see if my contact is even working. Imagine a steel chain with multiple links. Take any two links as the scope of the problem. Not fix one link (fixed support) and apply longitudinal force on the other.

I have tried to setup the contact two ways:
1) just select the interacting faces on the links. Set one link as contact and the other as target.
2) select one body as contact and the otehr body as target (all faces on both the bodies).

But my links never seem to interact. What could be wrong>? Is there a way to expeort a .inp file from WB environment so that I can post it here?

Thanks,
MAhesh

 

[maheshh]

how can i post text attachements here? the inp file is too large to paste

Thanks
mahesh

 

[maheshh]

I have attached pictures for a simple test case that I am trying to run. Am not sure why there is no contact interaction. Can somebody point out how to setup the contact? Or what is it that I may be doing wrong?

Environment:

http://farm1.static.flickr.com/237/455829357_0de43206ae_o.jpg

Contact:

http://farm1.static.flickr.com/169/455829371_c4756053f7_o.jpg

Deformation:

http://farm1.static.flickr.com/178/455829405_1595638144_o.jpg

 

[cbrn]

Hi,
maybe the contact is not closed at the start of the analysis: in this case, make sure that you set "each equilibrium iteration" under the "update stiffness" option.

Regards

 

[maheshh]

But if the analysis is set for large displacement, should it matter whether the contact is closed or not?

For example in another simulation, I have a complex mechanism where two parts are almost 5 mm apart at teh start, and over the period of the movement of another part, one of the parts will travel 5 mm and touch the other. In this case I have about 20 different contacts out of which at least 3 will always be open at the start. How will Ansys handle this?

Thanks,
Mahesh

 

[cbrn]

Hi,
I recognize that this kind of analysis can become extremely tricky. In your simplified example of the two plates, I'd set a surface / surface contact (not a body / body one), frictional, mu=0.2 (this is for contact between two pieces of steel, you may or not be interested in friction...), symmetric (or asymm if you can properly identify a contact and a target), trim contact -> program controlled, augmented Lagrange, tolerance -> program controlled, interface -> Add offset, no ramping, offset=0, normal stiffness -> program controlled, update stiffness -> each equilibrium iteration (this is EXTREMELY important in order for the contact not to be "missed"), pinball -> program controlled, time step controls -> predict for impact.
In the analysis settings: 1 Step, auto time stepping -> ON (this is also very important), substeps: initial 10, min 10, max 100 (adjust numbers as desired, but ensure you will have a sub "near" to the "impact" of the two bodies).

With these settings, I produced the correct solution for your example, so there is no reason why it shouldn't work with your "complex" model (OK, likely you will have to repeat the analysis until you find the correct combination of settings). The fact I used v.11 instead of v.10 is unrelevant: these settings are the same in v.10.

Hope this helps...

Regards

 

[doatis]

What you set the solver to include large deformation, that will increase the pinball radius (unless you've specified it manually). Whenever I have an initially open contact set, I use the automatic time stepping to control how 'fast' the parts come into contact. If your time stepping is too large, odds are your parts will "fly" through eachother.

In v11, they have added a Contact Tool that you can insert into the 'Contact' branch. You can then solve for initial status. This is the same as issuing the cncheck,all in ANSYS Classic. You can then go through and double check that any and all gaps are where they should be, and the value is correct.

Your complicated model should solve, but will take longer because of all the additional contact and increased model size. You can try increasing the pinball radius to be your gap size, which will in turn perform near-field calculations earlier...meaning slower solve time. It's always a give and take =)

I would use cbrn's contact settings (augmented Lagrange, updated each iteration, etc.), since those are what I use whenever I have 'troublesome' contact problems. The rest is fine tuning it to work for your application.

Hope this helps,
Doug

 

[maheshh]

I was not able to find the option:

time step controls -> predict for impact.


anywhere.

Can somebody point me to this setting in the WB 10.0 environment?

Thanks,
Mahesh

 

[maheshh]

Still no luck with contact interaction. I have tried out the settings for contact that have been suggested here. The only setting I was not able to find on the WB environment was:
time step controls -> predict for impact.

Thanks
Mahesh

 

[cbrn]

Hi,
I'm very sorry I confused you: I forgot that the timestep control (typical of Classical environment since at least v.8...) has been introduced in WB only in v.11, so in v.10 you won't find the "predict for impact" option. You will have to tune the analysis timesteps by yourself.

Regards

 

[maheshh]

In any case, I was not able to get the contacts to interact with all the settings that you mentioned (except the predict for contact). So I think "predict for contact" setting is very important.

I just received a copy of version 11 from Ansys and I will be installing it soon. I will keep you guys updated whether I get lucky with version 11.

Thanks for all the help.

MAhesh

 

[cbrn]

Hi,
well, "predict for contact" is very important in order to save a lot of pre-calculation, but I believe that it should be possible to live without it: in fact, in the example of the chain, you would have to calculate by yourself the timestamps at which the chain rollers would impact the teeths of the driving wheel. Then, you would have to set up an analysis with a STEP at least at each of your calculated timestamps (plus, eventually, some intermediate ones if it makes sense for some reason). These "impact-possible" steps should be allowed to subdivide in substeps.
But, of course, if you can upgrade to v.11 it should be better (anyway, don't expect it to solve it 100% automatically! ;-) ). Another thing: you're one of the firsts I "hear" in this forum who will soon upgrade to v.11, so I take the opportunity to warn you: v.11 has some REGRESSIONS with respect to v.10 (and at least one of them is, in my opinion, extremely severe), so be cautious if you find behaviours very different from what you expect to be correct.

Regards

 

[maheshh]

I thought that if I use an unreasonably high number of substeps for a static nonlinear contact problem, I should not have to calculate the exact substep when the contact occurs. In any case the complex problem that I am trying to solve, the metal components are already in contact so there is no need to calculate. I still have problem setting up the contact.

In any case, if you can help me understand how to do the # of substep calculations I would appreciate it.
Environment:

http://farm1.static.flickr.com/237/455829357_0de43206ae_o.jpg

Contact:

http://farm1.static.flickr.com/169/455829371_c4756053f7_o.jpg

Deformation:

http://farm1.static.flickr.com/178/455829405_1595638144_o.jpg

The problem of two cantilever beams that I had posted before can be used as a example. I have a gap of I think 2 mm between the beams and one beam is loaded with 5 N downward force. I tried setting contacts using body-body or face-face, and used 100 substeps (updating stiffness each equilibrium step) but still there was not interaction between the contacts.

Thanks,
Mahesh

 

[doatis]

Is this a 2D or 3D analysis? Looking at the pictures, it looks like a 2D analysis defined with surface to surface contact. You need to use edge-edge contact for 2D models.

Sorry if you already knew this.


Doug

 

[maheshh]

Doug,

It is a 3D problem.

 

[cbrn]

Hi,
I keep on not understanding... I retried the "two-beams" example in v.10 and it works perfectly! Settings are:
CONTACT REGION:
frictionless, face-face, asymmetric (the Contact is on the "forced" beam), augmented Lagrange, add offset -> 0, update stiffness each equilibrium iteration, sphere of influence -> radius, radius of sphere -> <slightly more than the initial distance btw contact and target>
SOLUTION:
1 step, direct solver, weak springs off, large displacements, ato time steps ON, initial number of substeps 10, min number 10, max number 50.

When you review the results, BE CAREFUL to set the displacements' multiplier to 1 (real scale), otherwise you will see the "forced" plate pass through the other because the displacement differences will also be scaled!!!

Regards