September 10, 2022 at 9:44 pmhelen.durandSubscriber
What is the difference between a single frame and multiframe restart in ANSYS transient structural?
Using inserted command objects, I want to change the material type (MPCHG) and use element birth and death (EKILL and EALIVE) between each loadstep. Do I want to use single frame or multiframe restarts?
I found some resources on single and multiframe restarts, but it's still not clear to me which to use:
September 14, 2022 at 6:18 pmSean HarveyAnsys Employee
You can change material properties between load steps by using the ‘MPCHG’ command with certain limitations such as material properties cannot be changed from linear to nonlinear, or from one nonlinear option to another. So for this, you don't need restart.
Ekill and ealive also do not need restarts and they are natively exposed inside Mechanical if you are using Mechanical that is.
Single frame restart is the original method of restarting in APDL. In fact if you are in MAPDL, you solve a load step, then add some loads, and solve again, you are using a single frame restart. There are all the files such as esav,full,db, etc. needed to do this. You may have seen input files for mapdl that have multiple solve commands. That doc you shared is a good resource that if you are using mechanical, it will naturally set the model up for multiframe restarts. With multiframe, we can have multiple points, but there are some limitations as listed in that help doc.
So, in your case, you can use single frame restart and just put in mpchg in a command object, and use ekill and alive natively. The code provided to delete the rdb and turn of restarts should not be necessary if you go to Analysis Settings> Restart Controls> Generate Restart Points to No.
MPCHG is valid in /solu, so you don't need to even leave /solu to go to /prep7
Keep in mind Mechanical deletes the single frame restart files (and other files) by default after the solve, and you can change this under Analysis Settings > Analysis Data Management> Delete Unneeded files to No
September 23, 2022 at 2:02 amhelen.durandSubscriber
Thank you for the detailed reply! This is extremely helpful. I just have a couple of follow up questions:
What do you mean by using ekill and ealive "natively" in transient structural?
Is there a way to change between two nonlinear materials? For example, is it possible to change some elements from one nonlinear material to another nonlinear material at the end of each load step using command objects?
September 23, 2022 at 9:54 pmSean HarveyAnsys Employee
See the screenshot below. It is in the Mechanical UI as an option as shown.
I answered on the other thread but I can repeat it here for the benefit of others.
MPCHG command allows you to change from one nonlinear material to another, but it does not support if there are different options.
per the help doc on MPCHG "Changes the material number of the specified element. Between load steps in SOLUTION, material properties cannot be changed from linear to nonlinear, or from one nonlinear option to another."
So you can't switch the type of plasticity model, etc. If you do, you will get an error like this.
*** FATAL *** CP = 191.328 TIME= 14:33:48
Change a nonlinear material model, 2, to another nonlinear material
model, 1, is not allowed for element type 186.
- You must be logged in to reply to this topic.
Simulation World 2022
Check out more than 70 different sessions now available on demand. Get inspired as you hear from visionary companies, leading researchers and educators from around the globe on a variety of topics from life-saving improvements in healthcare, to bold new realities of space travel. Take a leap of certainty and check out a session today here.
Earth Rescue – An Ansys Online Series
The climate crisis is here. But so is the human ingenuity to fight it. Earth Rescue reveals what visionary companies are doing today to engineer radical new ideas in the fight against climate change. Click here to watch the first episode.
Subscribe to the Ansys Blog to get great new content about the power of simulation delivered right to your email on a weekly basis. With content from Ansys experts, partners and customers you will learn about product development advances, thought leadership and trends and tips to better use Ansys tools. Sign up here.
- How to calculate the residual stress on a coating by Vickers indentation?
- Solver Pivot Warning in Beam Element Model
- Errors – Reinforced Concrete Beam
- An Unknown error occurred during solution. Check the Solver Output…..
- The solver engine was unable to converge on a solution for the nonlinear problem as constrained.
- whether have the difference between using contact and target bodies
- Massive amount of memory (RAM) required for solve
- Cannot apply load on node
- Saving & sharing of Working project files in .wbpz format
- Colors and Mesh Display