Surface contact

[pugAA]

Hello,

I'm working with a model that has a lot of elements in surface contact and that means

very long computational time.

I activated the option " Contact Element Updating" to speed the calculations, but the

problem is that I have a very large surface with many elements.

How can I divide this big surface (automatically generated in the mesh process) in 5

or 6 smaller surfaces. Will I reduce simulation's time in this way? (I think smaller

surfaces, less elements in contact and the processor will recognize the correct

surface in contact each time).

Thank you for your feedback.

[S.LI]

Dividing a big surface to several smaller one is definitely helpful to reduce computations.

If the model is drawn by hand, you can select lines on the surface and modify their attributes to another surface (the new one).

If the model is from CAD, I guess you'd better change surface number in your CAD model, otherwise there will be a warning message.

[zhuangs]

Though this is an old topic, I still want to provide some comments and advice here.  I don't think it is a good and practical  idea to split a large surface to a few small surfaces to save CPU time for MES contact:

(1)          The first issue is that this idea results in redundant surfaces which might the user does not want but cannot be deleted.  Some users here asked how to remove them.

(2)          The second issue is that this idea cannot effectively save CPU time.

 If there is no memory issue (not enough memory),  the following procedure can greatly save CPU time for your current model:

(1)          Please check which contact updating method is used.  If "Never" is used, this might be the reason that makes your simulation slow.  Then please check the "Maximum initial distance” for each contact pair.  If “zero” is used (and if you are using version 2011 or earlier versions), then this is exactly the reason.

(2)          Please switch to use “Automatic” contact updating, if there is kind of large relative motion (compared with mesh size) between the two surface in a contact pair.  But if the relative motion is tiny, “Never” contact updating with a small ‘Maximum initial distance” rather than zero for each contact pair will be better.

By the way, we do some improvements in version 2012:

(1)          “Automatic” contact updating will always be default for a new defined contact model no matter how you define contact pairs.

(2)          If "Never" contact updating is used, and if the user does not define the "Maximum initial distance” with default of zero, a value based on mesh size rather than an infinite value is set for calculating contact element.

Note that "Never" contact updating is always to be used for contact with small relative motion.  Otherwise, "Automatic" is recommended.

[bjorn_fallqvist]

I would recommend that you rather split the surface in CAD, if it is a CAD model. Otherwise, you could always modify the attributes of the lines themselves, and "repair" the old surface with new lines, I guess. It kind of depends on the model.

[northtown]

I have the same question. If I use bonded, the simulation will be completed in 4-5 hours; if any kind of surface contact was used, the simulation becomes very very slow, it only completed 2-3 % after continue running 3 days (over 70 hours). How many hours did this simulation take?

[S.LI]

---

@northtown wrote:

I have the same question. If I use bonded, the simulation will be completed in 4-5 hours; if any kind of surface contact was

The real meaning behind "bonded" is "no contact", at least "simplifed surface-to-surface contact". Since it knows the surface pairs are bonded together, solver won't consider contact updating, surface movement etc. So this saves a lot of simulation time.

used, the simulation becomes very very slow, it only completed 2-3 % after continue running 3 days (over 70 hours). How many hours did this simulation take?

So far, we don't have any accurate estimate on the simulation time for a general contact problem. As mentioned in above messages, some option changes might be helpful on this, but no guarantee.

---

[zhuangs]

For your case,  it is not usual if "surface contact" only completes 2-3% in 70 hours while "Bond" completes 100% in 4-5%, even though we know "Bonded" should run faster than "Surface contact".

If "Bonded" is used for a contact pair, if you run the model or only "check" the mpdel, the preprocessor will combine the nodes on the two sunrfaces, which means the two parts share the same nodes on the contact area.

For your case with "Surface contact", there are a few things that might result in slow convergence, divergence or slow simulation speed:

(1) "Contact updating":  If "Never" is used, you can either switch it to "Automatic" or define a reasonable value rahter than 0 for each contact pair (if the relavtive motion is small, try to use a value of 2 times of mesh size)

(2) "Large displacement": For surface contact, "Large displacement" is always recommended for all the part which have this option.

(3) "Contact (Defualt: Bonded)":  If you don't need bond some parts when you use "Surface contact", set the default as "free/no contact".  "Bonded" option currently results in some unnecessary bonding when there is "Surface contact".

(4) Contact stiffness and contact distance:  Disable "adaptive contact stiffness option" first, and then try to use "user-defined" contact stiffness as recommended by the document.

-Shoubing

---

@northtown wrote:

I have the same question. If I use bonded, the simulation will be completed in 4-5 hours; if any kind of surface contact was used, the simulation becomes very very slow, it only completed 2-3 % after continue running 3 days (over 70 hours). How many hours did this simulation take?

---