You don’t wanna step to this: Breaking down Loadsteps and Substeps in ANSYS Mechanical

By: Doug Oatis
– November 8, 2011
Categories:

Did you know Warren G is still alive?!?  I obviously confused Nate Dogg with Warren G.  How embarrassing.  Anyways, on to the topic at hand…regulators, mount up.

Nate Dogg and Warren G using ANSYS…what’s next?

So what exactly is the difference between a load-step and a sub-step?  A load-step should be thought of as a set of constraints/loads that are being solved for while the sub-steps are how you transition from one loading environment to the next. 

Blue = Sub-step, Red = Load-step
Solved for loading

So as shown in the graph above, at time=1 (for a static run time is meaningless, think of it more as a % of applied load where 1=100%) the applied load is 10 pounds.  Since it’s the first load-step, all applied values are ramped from 0 (by default), and there are 10-equal interval sub-steps that allow the solver to get from 0 to 10.  For load-step 2, which has an end time of 2 (load-steps must have increasing end-times), only 4 sub-steps that get progressively larger were used.  We’ll get into how that works, but the important take-away is that load-step 2 starts at the end of load-step1. 

Within Mechanical, you define both load-step and sub-step controls in the ‘Analysis Settings’.

Red = Load-step, Blue = Sub-step

By default the number of steps in an environment is 1, and the solver has control over how the loads are ramped.  As soon as you increase the number of steps you will see this reflected in the ‘Tabular Data’ window for any applied load or constraint.

Single Load-step Defined
Two Load-steps Defined

When you first start defining the load for a multi-load-step analysis, Mechanical assumes that the loading will remain constant for all subsequent steps.  This is indicated by an ‘=’ sign shown in the tabular data.

Mechanical assumes a constant value for LS2

So after you’ve gone through and defined an assembly loading process, large deflection plastic analysis to determine permanent set, or whatever else your heart desires…you can go back to define how the loads are ramped from one step to the next. 

Toggling the ‘Auto Time Stepping’ to ‘On’ gives you even more options.

Auto Time Step = On

You have the ability to define the ramping controls either by number of sub-steps or time.  Both represent the same thing, just presented through a different paradigm.

Not to be confused with a pair-of-dimes…(I’ll be here all night, make sure you tip the wait staff)

Before I get into the difference between sub-step and time, I’ll touch on the Initial/Minimum/Maximum values (note the following explanation is valid for the sub-step paradigm).  The initial value is the initial ramping value used to start off the current load step.  If the solver was able to converge easily, it can increase the load increment until it hits the ‘minimum’ sub-step value.  If the sub-step was difficult to solve, or did not solve at all, the solver can reduce the increment and try again. 

Assuming the end time of the load step is 1, here are equivalent sub-step controls (sub-step vs time) listed next to what the actual load increments are:

Equivalent Settings Assuming End Time=1, Actual Load increments shown on right

One thing to note is that if you were to change the end time from 1 to 2, the sub-step-method would still ramp by the exact same amount for each sub-step whereas the time-method would ramp it slower.  Obviously if you are running a transient analysis these controls become very important as they determine what response frequencies you’ll pickup from your structure.  The documentation recommends a time-step size of (1/20*f), where f is the highest frequency assumed to contribute to the response.  If your time-steps are too large, you’ll miss the higher frequency content that could be more damaging.

So now you’re probably thinking “great, so now what?”.  First…watch that tone mister.  Second, this should be one of the first places you should turn when you run into model convergence issues.  If a model is poorly constrained you can run a first load-step with additional constraints and then ‘release’ it once the model has converged.  If you have a model held in place purely by contact you can run an initial no-applied-load-step to allow the contacts to ‘settle down’ and properly engage.  If you have a model that fails due to excessive distortion or accumulated plastic strain you can increase the number of sub-steps to ramp the loads slower.  Or you could use this information to create some fairly complex loading environments.

I’ll be going over all of this information and more (activating/deactivating loads, command snippet use, etc) in the upcoming PADT Webinar being held on November 17th.  Hope to see you there.

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

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: