December 9, 2018 at 10:01 amMirghaniSubscriber
Hi Ansys Community
I am trying to run a non-linear analysis for a precast Concrete Hollow Core Slab "HCS" with topping subjected to blast loading "pressure" in ansys workbench explicit dynamics. the purpose is to determine the optimal topping thickness that could withstand the blast with some failure criteria. the model is prepared in space-claim (Line"beam" elements for Strands and topping reinf." and solid elements for concrete and supports). I used symmetry by modeling only one quartet of the HCS. CONC-35MPa material is used to model the concrete and structural steel is used to model the strands and topping reinf. Any Help or suggestion with the following will be highly appreciated.
* Version used: Ansys Workbench 19.2
2. How to Apply the following
a. the pre-stressing force on the strands in an explicit dynamic analysis "Prestressing-longer term event, followed by a blast Pressures-short term event. Any Initial Conditions required??
b. How to apply the blast pressure?? Directly on the slab surface. when to use the blast load by the means of a detonation point with TNT material specified in the engineering data.
4. Which material model better simulates the concrete in this case "Blast" (RHT Concrete strenght/CONC-35MPa or another concrete model may be more suitable).
5. With an end time of 0.005 the full simulation solution is reached. "What is the rule of thump for calculating a suitable end time for the blast"??
The attached file include all the snaps of the model.
thanks in advance
December 15, 2018 at 4:36 am
December 15, 2018 at 1:05 pmMirghaniSubscriber
I managed to run the analysis to completion with an end time of 0.08 seconds. To overcome the issue of the "Time step too small" in explicit dynamics, I changed the mesh and make it more uniform with no elements too small than others. In general I think the solution of this type of problem is to check the mesh for any small elements that could affect the run time because the run time in explicit dynamics depends directly on the element size, the smaller the element the higher the probability of this error.
January 17, 2019 at 8:27 pmMissy JiAnsys Employee
Q: How to deal with ""Program terminated -time step too small"" error message? "
In ANSYS Explicit "Analysis settings", Step controls section, there is a field called "minimum time step", this is the minimum time step allowed in the Explicit analysis, If set to Program Controlled, the value will be chosen as 1/10th the initial time step. If the current time drops below this value the analysis will stop.
You can always decrease the minimum time step to continue the calculation. After loading your problem, go to "Analysis settings", select Timestep Options. Change the Minimum Time Step to a very small number, for example, 1e-15, your simulation will continue with the small time step. And the simulaiton might take a long time to the completion.
The variables affecting the time step are the smallest cell size, gap size, velocity, and sound speed. For Lagrangian type parts, you need to examine the geometry of the parts to see if there are distorted cells.
For Lagrangian type parts, you need to examine the geometry of the parts to see if there are distorted cells. So when you say the error messages, examine the time step contours, find out where are the distorted elements, get a better mesh quality might help increase the time step. To have timestep plotted from the graphics area, you can insert an user defined results, (see attached image), use the expression "TIMESTEP" to request timestep contours, then you could have an idea on where those small time step occurs.
Mass scaling is another way to improve the time steps.
I would suggest to have a uniform and good quality mesh to start. However, during the projectile impact problems, there would be distorted elements, they will not provide stiffness to the simulaiton, so you could also remove those elements away from the calculation by using erosion, there are multiple criterias to remove elements, you can set them from Analysis settings, Erosion controls section, you can use material failure, geometric strain limit to remove highly distorted elements.
Erosion is a numerical mechanism for the automatic removal (deletion) of elements during a simulation.
Removes very distorted elements before they become inverted (degenerate).
Ensures time step remains reasonably large.
Ensures solutions can continue to the End Time.
Can be used to allow simulation of material fracture, cutting and penetration.
November 22, 2019 at 2:53 pmyousafSubscriber
Do you know how to run 3D in autodyn
- You must be logged in to reply to this topic.
Simulation World 2022
Earth Rescue – An Ansys Online Series
- How to calculate the residual stress on a coating by Vickers indentation?
- Errors – Reinforced Concrete Beam
- Solver Pivot Warning in Beam Element Model
- 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
- Large deflection
- Colors and Mesh Display