Overcoming Convergence Difficulties in ANSYS Workbench Mechanical, Part I: Using Newton-Raphson Residual Information

By: Ted Harris
– October 10, 2012
Categories:

image

Unable to converge.  Convergence Failure.  Failure to Converge.  Never nice words to see when you are trying to get your simulation done. 

If you’ve encountered convergence failures while running nonlinear structural analyses in ANSYS Workbench Mechanical, this two part series is for you.  What is a convergence failure?  In a nutshell it means that there is too much imbalance in the system.  The calculated reaction forces do not match the applied loads and even though the program tries hard to make changes to overcome the imbalances, it hasn’t been able to do so and stops.  If we look at the Force residuals under Solution Information, we will see that the solver has been unable to get the force convergence residual, or imbalance force, to drop below the current criterion

image

Test model example:  Newton Raphson Convergence Failure; Solution Stops

We won’t spend a lot of time here explaining the Newton-Raphson method, convergence, and residual plots here, since we wrote a Focus article back in 2002 which discusses them in more detail.  The article begins on p. 7 at this link:

/wp-content/uploads/oldblog/archive/PADT_TheFocus_08.pdf

The context of that article was Mechanical APDL, but the article is directly relevant since solving in Workbench Mechanical is done in Mechanical APDL in batch mode. 

In crayon terms, we want the purple line to drop below the blue line.  When it doesn’t and the solver is out of options to keep trying, the solution stops and we get an error message. 

Now what?  The traditional knobs to turn are to increase the number of substeps, decrease contact stiffness if contact is involved, perhaps add more points to the plasticity curve, etc.  But what if something else is the problem?  How can we identify where the problem is?

In this part I article we will discuss how to plot the Newton-Raphson residuals as contour plots to see where in the model the highest force imbalances are located.  Often this is useful information to help us figure out what is going on so we can take corrective action.  First, be aware that we must turn on the Newton-Raphson residual plots prior to solving.  That means you either have to turn them on and re-solve after a convergence failure, knowing that you’ll get the same failure again, or you need to clairvoyantly (or perhaps just prudently) turn on the residuals prior to attempting the initial solve.  Why aren’t they on all the time, you ask?  Most likely because they slow things down just a bit and also require a bit more disk space than otherwise, although if the solution runs to completion no Newton-Raphson residual plots are saved.

Here is how we turn them on.  In the Details view for the Solution Information branch, change the Newton-Raphson Residuals setting from the default of zero to a nonzero number such as 3 or 4.  That will continuously save the last 3 or 4 Newton-Raphson residual plots for viewing as contour plots after the solution has stopped due to a convergence failure.

image

After the solution has stopped, the Newton-Raphson residual plots will be available under the Solution Information branch.

image

The quantity plotted is actually the square root of the sum of the squares of the residuals in the global X, Y, and Z directions.  So, the plots don’t show us direction information, but they do show where the residuals and hence the force imbalances are the largest.  Below is an example.  The region in red shows where the residuals are the highest.  Since this is a model involving contact between two bodies, apparently the contact regions and specifically contact at the corners of the part on the left is the source of our convergence difficulties.

image

Newton-Raphson Residual Force Plot for the last attempted equilibrium iteration.

So, how do we use this information?  In this case we now suspect that the contact regions, especially at the corners of the smaller part, are the problematic areas.  Using this information we made two changes to the model. 

First, we changed the Detection Method for the contact elements from Program Controlled (at the element Gauss points) to Nodal-Normal to Target.  Many times when contact problems involve touching at corners, the robustness of the contact interface can be improved by changing the detection method from Gauss points to nodes.

Second, we reduced the contact stiffness by changing Normal Stiffness from Program Controlled (factor of 1.0) to a Manual setting of 0.2.  Reducing the contact stiffness can help with contact convergence for a lot of problems.  Too low of a stiffness value can cause problems too, but in this case the resulting penetration is still small so a value of 0.2 seems reasonable.  When in doubt, a sensitivity study can be performed whereby you make changes to the contact stiffness value while tracking your results quantities of interest.  As with most inputs you can vary, your results of interest should not be sensitive to contact stiffness.

These two changes allowed our test model to nicely converge for the full amount of load.

image

Other considerations:

The Newton-Raphson Residual plots are always displayed on the original geometry, not the deflected geometry at version 14.0 of ANSYS Mechanical.  If the deflections are large this can make it harder to ascertain what is causing the high residual values.  In those cases, it can be helpful to compare the total deformation and stress plots for the unconverged solution, along with those plots for the last converged solution, with the 1.0 true scale on the deformation active.  This will show the parts in their deflected state, and that can help in determining why the residuals are high at certain locations.

We recommend creating at least 3 residual plots (set in the details of Solution Information as described above).  Sometimes the location of the imbalance can bounce around a bit from equilibrium iteration to equilibrium iteration, so having more than one or two plots to look at can be beneficial in determining problem locations.

Conclusion

Summing it up, the Newton-Raphson residual plots are one piece of information we can use to determine why we are having convergence difficulties.  They can give us an indication of where the convergence difficulties are occurring in the model, and many times we can use that information to help us know what settings should be modified or what other changes should be made to the model to improve the convergence behavior.

In part II of this article, we’ll look at how to quickly use ANSYS Mechanical APDL to view the elements that have undergone too much deformation.

Categories

Certified Elite Channel Partner

Get Your Ansys Products & Support from the Engineers who Contribute to this Blog.

Product Development
Diamond Partner

Technical Expertise to Enable your Addictive Manufacturing Success.

PADT’s Pulse Newsletter

Keep up to date on what is going on at PADT by subscribing to our newsletter.


By submitting this form, you are consenting to receive marketing emails from: Phoenix Analysis and Design Technologies, 7755 S. Research Dr., Tempe, AZ, 85284, https://www.padtinc.com. You can revoke your consent to receive emails at any time by using the SafeUnsubscribe® link, found at the bottom of every email. Emails are serviced by Constant Contact

Share this post:

Share on twitter
Share on facebook
Share on linkedin
Share on pinterest

Upcoming Events

09/21/2022

ExperienceIT NM 2022

09/21/2022

Additive Updates in Ansys 2022 R2 - Webinar

09/14/2022

Rocky Mountain Life Sciences Investor & Partnering Conference

09/08/2022

Ansys Optics Simulation User Group Meeting - Virtual

09/08/2022

Ansys Optics Simulation User Group Meeting

09/07/2022

SI & PI Updates in Ansys 2022 R2 - Webinar

08/31/2022

Simulation Best Practices for Developing Medical Devices - Webinar

08/24/2022

Mechanical Updates in Ansys 2022 R2 - Webinar

08/10/2022

Tucson after5 Tech Mixer: Ruda-Cardinal

08/05/2022

Flagstaff Tech Tour, 2022

08/02/2022

2022 CEO Leadership Retreat

08/01/2022

2022 CEO Leadership Retreat

07/27/2022

Thermal Integrity Updates in Ansys 2022 R1 - Webinar

07/20/2022

Simulation Best Practices for the Pharmaceutical Industry - Webinar

07/14/2022

NCMS Technology Showcase: Corpus Christi Army Depot

07/13/2022

NCMS Technology Showcase: Corpus Christi Army Depot

07/13/2022

Additive & Structural Optimization Updates in Ansys 2022 R1 - Webinar

07/07/2022

Arizona AADM Conference, 2022

06/29/2022

LS-DYNA Updates & Advancements in Ansys 2022 R1 - Webinar

06/23/2022

Simulation Best Practices for Wind Turbine Design - Webinar

06/15/2022

MAPDL Updates & Advancements in Ansys 2022 R1 - Webinar

06/01/2022

Mechanical Updates in Ansys 2022 R1 - pt. 2 Webinar

05/26/2022

Modelling liquid cryogenic rocket engines in Flownex - Webinar

05/25/2022

SMR & Advanced Reactor 2022

05/25/2022

05/24/2022

SMR & Advanced Reactor 2022

05/19/2022

RAPID + tct 2022

05/19/2022

Venture Cafe Roundtable: AI & Healthcare

05/18/2022

Tucson after5 Tech Mixer: World View

05/18/2022

RAPID + tct 2022

More Info

05/18/2022

Signal & Power Integrity Updates in Ansys 2022 R1 - Webinar

05/18/2022

Simulation World 2022

05/17/2022

RAPID + tct 2022

05/11/2022

Experience Stratasys Manufacturing Virtual Event

05/04/2022

Mechanical Meshing Updates in Ansys 2022 R1 - Webinar

04/27/2022

04/22/2022

12TH ANNUAL TUCSON GOLF TOURNAMENT

04/21/2022

04/20/2022

Additional Fluids Updates in Ansys 2022 R1

04/20/2022

Experience Stratasys Tour – Tempe Arizona

04/18/2022

Experience Stratasys Tour - Flagstaff Arizona

04/14/2022

D&M West | MD&M West

04/13/2022

D&M West | MD&M West

04/13/2022

Experience Stratasys Tour - Albuquerque New Mexico

04/12/2022

D&M West | MD&M West

04/12/2022

Experience Stratasys Tour - Los Alamos New Mexico

04/12/2022

Optimizing Engineering Workflows f​​​​or Propulsion System Design

04/07/2022

Experience Stratasys Tour - Austin Texas

04/07/2022

37th Space Symposium - Arizona Space Industry

04/06/2022

Transforming Digital Engineering with Ansys Discovery 2022 R1

04/06/2022

37th Space Symposium - Arizona Space Industry

04/05/2022

37th Space Symposium - Arizona Space Industry

04/04/2022

37th Space Symposium - Arizona Space Industry

03/30/2022

Simulation Best Practices for Vehicle Engineering - Webinar

03/23/2022

03/23/2022

High & Low Frequency Electromagnetics Updates in Ansys 2022 R1

02/24/2022

Arizona Technology Council After 5 Tech Mixer "Pandemic Pivot Pizza Pa

02/23/2022

SciTech Festival: Spend an Hour with 3D Printing Experts

02/11/2022

Webinar: Mechanical overview for Ansys 2022 R1

More Info

02/09/2022

Webinar: Product Development 101 (FAKE)

02/08/2022

Webinar: Navigating the Additive Landscape

01/27/2022

Arizona Technology Council 1st Quarter VIP Tech Mixer

More Info

01/26/2022

Simulation Best Practices for Gas Turbine Design & Development - Webin

More Info

01/19/2022

Arizona Photonics Days

More Info

11/04/2021

ExperienceIT, New Mexico

More Info

11/03/2021

Additive Manufacturing & Structural Optimization in Ansys 2021 R2 - We

More Info

11/03/2021

Optics Valley Technical Series: The Future of Simulation in the Optics

More Info

11/02/2021

SBIR Liftoff AZTC Virtual Breakfast Series

More Info

10/10/2021

Stratasys Mobile Truck Stop - Tucson Arizona

More Info

Search in PADT site

Contact Us

Most of our customers receive their support over the phone or via email. Customers who are close by can also set up a face-to-face appointment with one of our engineers.

For most locations, simply contact us: