Convergence discussion

[bjorn_fallqvist]

Hi,

I have a model which does converge, but slowly. I've noticed the behaviour that at first, it converges quite quickly, but then the convergence rate rapidly drops instead.

For example:

Time        Percent     DT       L Iter. Residual
   0.000000   0.00     0.050000  1   0   0.0000E+00
   0.050000   4.55     0.050000  1   1   1.0000E+00
   0.050000   4.55     0.050000  1   2   8.1260E-02
   0.050000   4.55     0.050000  1   3   1.0256E-02c
   0.100000   9.09     0.050000  1   1   1.0000E+00
   0.100000   9.09     0.050000  1   2   4.5906E-01
   0.100000   9.09     0.050000  1   3   6.6314E-02
   0.100000   9.09     0.050000  1   4   2.3877E-02
   0.100000   9.09     0.050000  1   5   1.6093E-02c
   0.150000  13.64     0.050000  1   1   1.0000E+00
   0.150000  13.64     0.050000  1   2   4.1341E-01
   0.150000  13.64     0.050000  1   3   1.9418E-01
   0.150000  13.64     0.050000  1   4   1.2396E-01
   0.150000  13.64     0.050000  1   5   8.9698E-02
   0.150000  13.64     0.050000  1   6   5.7406E-02
   0.150000  13.64     0.050000  1   7   4.7166E-02
   0.150000  13.64     0.050000  1   8   4.2494E-02
   0.150000  13.64     0.050000  1   9   3.0608E-02
   0.150000  13.64     0.050000  1  10   3.2830E-02
   0.150000  13.64     0.050000  1  11   2.9407E-02
   0.150000  13.64     0.050000  1  12   2.3732E-02
   0.150000  13.64     0.050000  1  13   2.8896E-02
   0.150000  13.64     0.050000  1  14   2.3033E-02
   0.150000  13.64     0.050000  1  15   1.0503E-02c
   0.200000  18.18     0.050000  1   1   1.0000E+00
   0.200000  18.18     0.050000  1   2   2.3950E-01
   0.200000  18.18     0.050000  1   3   1.3407E-01
   0.200000  18.18     0.050000  1   4   1.1249E-01
   0.200000  18.18     0.050000  1   5   7.7317E-02
   0.200000  18.18     0.050000  1   6   5.6983E-02
   0.200000  18.18     0.050000  1   7   3.6821E-02
   0.200000  18.18     0.050000  1   8   3.4744E-02
   0.200000  18.18     0.050000  1   9   3.1027E-02
   0.200000  18.18     0.050000  1  10   2.1929E-02
   0.200000  18.18     0.050000  1  11   2.1361E-02
   0.200000  18.18     0.050000  1  12   1.5052E-02c
   0.250000  22.73     0.050000  1   1   1.0000E+00
   0.250000  22.73     0.050000  1   2   1.2450E-01
   0.250000  22.73     0.050000  1   3   7.3399E-02
   0.250000  22.73     0.050000  1   4   5.4359E-02
   0.250000  22.73     0.050000  1   5   4.7989E-02
   0.250000  22.73     0.050000  1   6   2.9189E-02
   0.250000  22.73     0.050000  1   7   2.8265E-02
   0.250000  22.73     0.050000  1   8   1.7900E-02c
   0.300000  27.27     0.050000  1   1   1.0000E+00
   0.300000  27.27     0.050000  1   2   1.6897E-01
   0.300000  27.27     0.050000  1   3   8.7232E-02

As you can see, for every step the residual starts to reduce rapidly, but after only a few steps, it "evens out", so to say. This is not critical, since the model does converge, it only takes a long time to solve. However, I'm interested in if you have any ideas as to what might cause this particular kind of behaviour?

I've tried fiddling with the surface contact (there are quite a few contact surfaces in the model) settings, but haven't seen any change. Any ideas?

Thanks,

Björn

[xli]

The number of a converged nonlinear iterations really reflects the nonlinearity of your model. But that nonlinearity usually contains many facts, such as material properties, geometry, contact, and various numberical approximations in the model etc. Generally as a transient nonlinear analysis package, MES always started from "rest" state, i.e.everything are guessed as zero. So this is generally far from true balanced state of your model, so model generally take more iteration in the 1st convergence step. It is a "transient" period. This is one explaination I can give.

-xli

[bjorn_fallqvist]

Hmm, ok....must be something I've overlooked. It shouldn't have that much of a non-linear behaviour...

Thanks.

[zhuangs]

Before we discuss about contact setting, the following procesures might help:

1. If "Static stress with NLM" is used, switch to "MES with NLM",
2. If there is any part having element definition with an analysis type of "small displacement", change all to "Large displacement".
3. If "MES with NLM" is used, more possible constraints and boundary conditions can help.

-Shoubing

[zhuangs]

Now we might discuss the contact setting, as for your question "I've tried fiddling with the surface contact (there are quite a few contact surfaces in the model) settings, but haven't seen any change. Any ideas?".  Before that, I would like first to know:

1. what kind of contact method for the contact pairs? frictionless, frictional or others?
2. whether the user-specified contact stiffness is activated? If yes, what is the value?

By the way, even though there is no nonlinear material models (Material Nonlinearity), there might be Geometric Nonlinearity, which can be resulting from contact, large displacement, etc.

-Shoubing

[bjorn_fallqvist]

I'm using a MES solver. I've had lots of difficulties with the regular NLM solver, so I avoid using it.

The contact is frictionless surface contact. I deactivated the adaptive contact stiffness setting, and am instead using my own value. This is set to 100 000N/mm and 250 000 N/mm for primary and secondary stiffness, respectively. I am unsure if this is correct since the material used in the contact is concrete, quite a soft material. I'm using a contact tolerance of 0.001mm, which I've used in models with forces of similar magnitudes earlier.

But, if I reduce the contact stiffness I get large penetration instead, and that's not desirable. Funny enough, I get both penetration and chatter at the same time. Aren't chatter a sign of too high contact stiffness and penetration a sign of too low contact stiffness? I'm not really sure how to handle this.

By the way, I have also tried re-meshing the model, and this refinemene does seem to help a little bit, despite the model getting bigger. Interesting. I guess this helps with the chatter problem?

Thanks

Björn

[zhuangs]

Hi Bjorn,

You are right to deactivate the adaptive contact stiffness setting.

Basically for penalty method, a larger stiffness results in a slower convergence, while a smaller stiffness results in a larger penetration.   But some contact models converge slow evne though the contact stiffness is small, since some typical material models and complicated geometry make convergence difficult.

For the log file of your model you attached, lots of iteration might result from too large contact stiffness (as you mention that concrete is used.).   Considering F=K*D, let's reduce K (contact stiffness) and enlarge D (contact distance).  Use 1/10 of the smaller modulus of the material in the contact pair as K, and enlarge D to adjust the penetration.  You might deactivate the user-defined contact distance.

-Shoubing

---

@bjorn_fallqvist wrote:

I'm using a MES solver. I've had lots of difficulties with the regular NLM solver, so I avoid using it.

The contact is frictionless surface contact. I deactivated the adaptive contact stiffness setting, and am instead using my own value. This is set to 100 000N/mm and 250 000 N/mm for primary and secondary stiffness, respectively. I am unsure if this is correct since the material used in the contact is concrete, quite a soft material. I'm using a contact tolerance of 0.001mm, which I've used in models with forces of similar magnitudes earlier.

But, if I reduce the contact stiffness I get large penetration instead, and that's not desirable. Funny enough, I get both penetration and chatter at the same time. Aren't chatter a sign of too high contact stiffness and penetration a sign of too low contact stiffness? I'm not really sure how to handle this.

By the way, I have also tried re-meshing the model, and this refinemene does seem to help a little bit, despite the model getting bigger. Interesting. I guess this helps with the chatter problem?

Thanks

Björn

---

[bjorn_fallqvist]

I think I found the error. At a corner, the vertices that were supposed to become several nodes due to contact didn't become several nodes. The program kept them snapped together...so what I had was a huge contact surface with only a few corner nodes still snapped together, where I'm guessing there would be a lot of local load transfer and possible non-linear effects.

I have had this problem before, that the surfaces do not come apart as they should due to "diagonal" surfaces still having their nodes snapped together, but that wasn't the first thing I thought off now. I manually moved the nodes a few mm to the side to avoid this, and now it runs much much better (and faster!).

Thanks!

[zhuangs]

I see.  You might use "Bonded" as default in FEA Editor.  Now this is kind of issue from mesh about "Bonded".  I got some contact models from AEs or customers with the same issue.  I have already reported this issye to our mesh developers.

In this case, I usually add some pairs with "Free/no contact" for the neighboring surfaces, if there are lots of surfaces to be bonded and "Bonded" have to be the default.  However, if "Bonded" as default  is not necessary, you can set the default as "Free/no contact", and you can set some pairs with "Bonded" if a few surfaces are needed to be bonded.  While it is also an idea to make a small gap.

-Shoubing

[xli]

Shoubing,

Well, that may not be an issue but a better understanding of the logic to set up part connections. In FEA editor's contact pair GUI:

There is a global setting for any possible pair in the model, which default is set as bonded. You can also build up individule part/surface connection pairs and set them as what you want. Those individule settings will over-write the global setting. And then all other possible connections will use the global default setting unless you set it yourself!

For example in follwing four parts model,

    o---------oo--------- o

     |     P1    | |     P2      |

     |             | |               |

    o---------oo--------- o

    o---------oo--------- o

     |     P3    | |    P4       |

     |             | |               |

    o---------oo--------- o

Say you want to build up contact pairs P1&P2, P1&P3,P2&P4,and P3&P4, and have that four pair defined. But using default global settings may end up the node of P1 and the node P4 snapped as well the node P2 collapsed with P3 nodes. So a good approach is set the global setting as Free, and the four individule contact pairs will give correct modeling.

Because the global setting now is free. If the model has somewhere parts needs to be connected, then you need to create corresponding individule pair to bonned them.

-xli 

[bjorn_fallqvist]

Yeah, I know that I can set the surfaces as free, but there are simply too many combinations that might create this problem, and that's why I chose the other approach. Likewise, there are too many areas supposed to be bonded to eachother to make it feasible to create the bonded contacts by hand.

At least it seems to run a little nicer now, although my previous post was maybe a bit premature (it's still taking a long time, but not as long).

[zhuangs]

You are right.  it is hard to manually set up these pairs for model with too many bonded areas.  This is also my concern.  I know this case should not be a user issue, and it should deserve some improvement.

For the running without bonded issue, I would recommend some setting changes based on my previous replys about contact stiffness and contact distance.

If the model is too large, you can share it for investigation if you would like to.

-Shoubing

---

@bjorn_fallqvist wrote:

Yeah, I know that I can set the surfaces as free, but there are simply too many combinations that might create this problem, and that's why I chose the other approach. Likewise, there are too many areas supposed to be bonded to eachother to make it feasible to create the bonded contacts by hand.

At least it seems to run a little nicer now, although my previous post was maybe a bit premature (it's still taking a long time, but not as long).

---

[bjorn_fallqvist]

Shoubing,

If you'd like to take a look at the model, I'd really appreciate it. I uploaded an archive of it on sendspace.com:

http://www.sendspace.com/file/3b1i2u

It seems like the model converged well only initially. 😞

[Joey.X]

To avoid the tedious work of manually set up contact pairs, there is an option at importing CAD model.

In CAD import options, go to "global" tab, turn on "Automatically generate contact pairs"(Default is Off). After CAD import, user will see all contact pairs under the Feaeditor/TreeView/Contact.

[bjorn_fallqvist]

Thanks for the tip. I know the setting's there, I've just decided not to use it because I'm usually comfortable with the parts by default being bonded.

It seems increasing the contact tolerance also improved the convergence rate. Now it's down to 14-15 hours instead of 30. Thanks for all your input, people. 🙂