turn on suggestions

Auto-suggest helps you quickly narrow down your search results by suggesting possible matches as you type.

Showing results for

- Navigation
- Simcenter
- Forums
- Blogs
- Knowledge Bases

- Siemens PLM Community
- Simcenter
- 3D Simulation - NX Nastran Forum
- Unclear "USER WARNING MESSAGE 3000 (CNTITER2)"

Options

- Subscribe to RSS Feed
- Mark Topic as New
- Mark Topic as Read
- Float this Topic for Current User
- Bookmark
- Subscribe
- Printer Friendly Page

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 10:47 AM

Hello Experts,

I solve a really big model with

- contact(Set to Zero)

initial: a) no gap

b) gap - realized with negative region offset,

- glueing,

- CBEAMS with PINFLAGS,

- CBUSH, CTETRA, CHEXA, CTRIA6,

- RBE2 RBE3,

- ...

in NX10 using iterative elemental solver for static analysis (SOL101).

Most of my contacts are centering seats in a flanged structure. As the structure is also connected with shear pins these contact definitions don't need to have contact because of their initial gap and the lack of large forces to overcome the gap. I do not know if its a problem for solver.

Because of security instructions of our firm I'm not allowed to post the model here and I have no time to strip it down. But may be its not necessary.

Here my problem - I've always got the following USER WARNING at the beginning of contact iteration in force loop 1

^^^Begin Contact Iterations for Subcase Number 1

^^^Contact Iteration Number 1

^^^Number of inactive contacts: 0

^^^Number of active open contacts: 464680

^^^Number of sticking contacts: 0

^^^Number of sliding contacts: 35133

^^^Begin Contact Force Iteration

^^^ Force loop: 1*** USER WARNING MESSAGE 3000 (CNTITER2)ITERATIVE SOLUTION FAILED TO CONVERGE IN 1000 ITERATIONS. FINAL ERROR WAS 1.543E-07.CHECK RESULTS FOR ACCURACY.

^^^ Force loop: 2

But finally every time the contact iteration converges:

^^^ Force loop: 3

^^^ Force loop: 4

...

...

...

^^^Contact Iteration Number 16

^^^Number of contact status changes: 83 (NCHG: 26)

^^^Number of inactive contacts: 498494

^^^Number of sticking contacts: 0

^^^Number of sliding contacts: 1319

^^^Begin Contact Force Iteration

^^^ Force loop: 1

^^^ Force loop: 2

^^^ Force loop: 3

^^^ Force loop: 4

^^^ Force loop: 5

^^^Contact force convergence ratio: 8.796551E-03 (CTOL: 1.000000E-02)

^^^Final contact status at convergence

^^^Number of contact status changes: 25 (NCHG: 26)

^^^Number of inactive contacts: 498517

^^^Number of sticking contacts: 0

^^^Number of sliding contacts: 1296

^^^Contact iteration converged

Now I do not know if I can trust my solution resluts. They appear in a correct way.

Can I ignore that warning?

I 've had a similar model in NX8.5.2 but there was no such warning. Does it depend on NX10?

Any suggestion can help!

With best regard, Michael

Labels:

21 REPLIES

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 11:24 AM

What other warning messages do you get before this warning?

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 11:44 AM

AM,

I have only one additional warning

*** USER WARNING MESSAGE 3000 (CNTITER)

THE USE OF CTRIA6, CQUAD8 OR RBE2 ELEMENTS IN THE ELEMENT BASED ITERATIVE

SOLVER REQUIRES THE USE OF THE PARAMETERS AUTOSPC AND ELITASPC.

WITHOUT THESE PARAMETERS, A SINGULAR MATRIX MAY OCCUR.

and my dat-File contains those parameters

$* PARAM CARDS

$*

PARAM AUTOMPC YESPARAM AUTOSPC YESPARAM ELITASPC YES

PARAM K6ROT100.0000

PARAM MAXRATIO1.000+12

PARAM OIBULK YES

PARAM OMACHPR YES

PARAM POST -2

PARAM POSTEXT YES

PARAM PRGPST NO

PARAM UNITSYS MN-MM

Did you have such a behavior, too?

What's your opinion?

Best wishes, Michael

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 11:48 AM

You need to set the parameters:

ELITASPC to YES

AUTOSPC to YES

Here's an explanation from the docs for ELITASPC:

Set to YES to perform the autospc in the element iterative solver. Normally the element iterative solver does not perform an autospc function as it is usually not necessary. For solid elements, the rotational dofs are eliminated directly. If K6ROT is specified for linear shell elements, there is no issue either. But for CQUAD8 and CTRIA6 elements and possibly other special cases, the autospc function is required. The drawback of this option is that it requires the assembly of the KGG matrix which is used in the autospc and this can have a significant impact on performance. This parameter will also generate the rigid body mass properties.

If MPCFORCES output is requested, this parameter will automatically be set to YES since a partition of the assembled stiffness matrix is needed for the calculation of the mpc forces.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 11:53 AM

AM,

as I told you, those Parameters are set (see below).

Michael

as I told you, those Parameters are set (see below).

Michael

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 12:09 PM

Sorry, I missed that, and I hope others can give you more advice.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 12:12 PM - edited 04-21-2017 12:22 PM

I hope so, too.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-21-2017 09:52 PM

MiDi1791 wrote:

Hello Experts,

I solve a really big model with

- contact(Set to Zero)

initial: a) no gap

b) gap - realized with negative region offset,

- glueing,

- CBEAMS with PINFLAGS,

- CBUSH, CTETRA, CHEXA, CTRIA6,

- RBE2 RBE3,

- ...

in NX10 using iterative elemental solver for static analysis (SOL101).

Most of my contacts are centering seats in a flanged structure. As the structure is also connected with shear pins these contact definitions don't need to have contact because of their initial gap and the lack of large forces to overcome the gap. I do not know if its a problem for solver.

Because of security instructions of our firm I'm not allowed to post the model here and I have no time to strip it down. But may be its not necessary.

Here my problem - I've always got the following USER WARNING at the beginning of contact iteration in force loop 1

^^^Begin Contact Iterations for Subcase Number 1

^^^Contact Iteration Number 1

^^^Number of inactive contacts: 0

^^^Number of active open contacts: 464680

^^^Number of sticking contacts: 0

^^^Number of sliding contacts: 35133

^^^Begin Contact Force Iteration

^^^ Force loop: 1*** USER WARNING MESSAGE 3000 (CNTITER2)ITERATIVE SOLUTION FAILED TO CONVERGE IN 1000 ITERATIONS. FINAL ERROR WAS 1.543E-07.CHECK RESULTS FOR ACCURACY.

^^^ Force loop: 2

But finally every time the contact iteration converges:

^^^ Force loop: 3

^^^ Force loop: 4

...

...

...

^^^Contact Iteration Number 16

^^^Number of contact status changes: 83 (NCHG: 26)

^^^Number of inactive contacts: 498494

^^^Number of sticking contacts: 0

^^^Number of sliding contacts: 1319

^^^Begin Contact Force Iteration

^^^ Force loop: 1

^^^ Force loop: 2

^^^ Force loop: 3

^^^ Force loop: 4

^^^ Force loop: 5

^^^Contact force convergence ratio: 8.796551E-03 (CTOL: 1.000000E-02)

^^^Final contact status at convergence

^^^Number of contact status changes: 25 (NCHG: 26)

^^^Number of inactive contacts: 498517

^^^Number of sticking contacts: 0

^^^Number of sliding contacts: 1296

^^^Contact iteration converged

Now I do not know if I can trust my solution resluts. They appear in a correct way.

Can I ignore that warning?

I 've had a similar model in NX8.5.2 but there was no such warning. Does it depend on NX10?

Any suggestion can help!

With best regard, Michael

It happens all the time with the iterative solver... 1.5E-07 isn't that bad, really, the default is 1E-8... I'd ignore the error.

That being said, have you tried the sparse solver? And since you mentionned it's a big model maybe use CNTASET to get a subset of the matrix solved during contact iterations, this should go a lot faster.

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-22-2017 02:46 PM

TenTechLLC,

thank you for answering.

Normally I don't use the iterative element solver. I also use the standard solver and I think it's the Sparse solver. But because of the huge amount of solid elements, 90 % of my structure with 3'000'000 grid points, NX advices the iterative elemental solver and I did obey.

Can you describe the system parameter CNTASET in your circumstances? I found very interesting facts about condensation but also that it's not usable for iterative solver. All other restrictions are not relevant for me.

https://docs.plm.automation.siemens.com/tdoc/nx/10

If I switch to sparse solver and matrix condensation can you estimate the influence on calulation time?

- For one loadcase the calculation lasts round about 5 hours with 15 contact iterations and 10 force loops in average for every iteration step. (I use a system with 190 GB RAM on Win7-64 bit with 24 hyperthreaded cores. The CPU load changes between 4 % and 80 %.)

Restrictions when PARAM,CNTASET,YES is defined

- If multiple subcases exist, the same contact set and the same constraint set must be used

by all subcases. This can be achieved by including the BCSET and SPC case control commands

in the global subcase. If the subcases use different contact and constraint sets, the software

will continue without the A-set reduction.

- If multiple subcases exist, only a single constraint set can exist, and the SPC case control

command must be in the global subcase.

- Bolt preload conditions are not supported.- The iterative solver is not supported.

- You cannot select additional degrees of freedom with the ASET bulk entry to include in

the Kaa matrix. The software determines all A-set and O-set degrees of freedom.

- The dynamic solutions 103, 111, or 112 are not supported.

Best wishes, Michael

- Mark as New
- Bookmark
- Subscribe
- Subscribe to RSS Feed
- Highlight
- Email to a Friend
- Report Inappropriate Content

04-22-2017 04:52 PM

MiDi1791 wrote:

TenTechLLC,

thank you for answering.

Normally I don't use the iterative element solver. I also use the standard solver and I think it's the Sparse solver. But because of the huge amount of solid elements, 90 % of my structure with 3'000'000 grid points, NX advices the iterative elemental solver and I did obey.

Can you describe the system parameter CNTASET in your circumstances? I found very interesting facts about condensation but also that it's not usable for iterative solver. All other restrictions are not relevant for me.

https://docs.plm.automation.siemens.com/tdoc/nx/10

/nx_help/#uid:id1369966

If I switch to sparse solver and matrix condensation can you estimate the influence on calulation time?

- For one loadcase the calculation lasts round about 5 hours with 15 contact iterations and 10 force loops in average for every iteration step. (I use a system with 190 GB RAM on Win7-64 bit with 24 hyperthreaded cores. The CPU load changes between 4 % and 80 %.)

Restrictions when PARAM,CNTASET,YES is defined

- If multiple subcases exist, the same contact set and the same constraint set must be used

by all subcases. This can be achieved by including the BCSET and SPC case control commands

in the global subcase. If the subcases use different contact and constraint sets, the software

will continue without the A-set reduction.

- If multiple subcases exist, only a single constraint set can exist, and the SPC case control

command must be in the global subcase.

- Bolt preload conditions are not supported.- The iterative solver is not supported.

- You cannot select additional degrees of freedom with the ASET bulk entry to include in

the Kaa matrix. The software determines all A-set and O-set degrees of freedom.

- The dynamic solutions 103, 111, or 112 are not supported.

Best wishes, Michael

The iterative solver is not supported, correct. Honnestly, I'm not convinced that the iterative solver would work best anyway since you need 15 iterations to converge, the sparse solver might. NX isn't really checking if you have contact or not before it "suggests" the iterative solver, it's just looking at the solid elements count relative to all elements in the model...

Based on your description of your model, it looks like the vast majority of your model is not involved in the contact definition. That means CTNASET would probably speed up the solve tremendously as the iteration will use a subset of the stiffness matrix. This should work very well for you.

Follow Siemens PLM Software

© 2017 Siemens Product Lifecycle Management Software Inc