Altair RISE

A program to recognize and reward our most engaged community members

Nominate Yourself Now!

Is there way way to restart a transient time marching solution with the last step from a steady state solution

Hi,

I am trying to run a transient time marching propeller analysis in AcuSolve. To save run time, I would like to run a steady state analysis without propeller mesh motion first and then use its last state to run a transient analysis with propeller mesh motion. I tried this but got a message saying no restart file exists. Any help on switching between steady and transient would be much appreciate.

Find more posts tagged with

AcuSolve

English

v2022.1

Accepted answers

All comments

acupro

The restart approach does require having a restart output set for the problem/run indicated in the RESTART command. Having a nodal output set is not enough, there needs to be a restart output set. By default, both nodal and restart outputs are written when the job does a clean stop.

Beyond that, it also depends on the setup of the initial steady state run. Are you doing that with a reference frame to approximate the flow established by the rotating propeller - or is the initial run simply to establish something of a 'surrounding' flowfield, with no accounting yet for the rotation?

I think new in 2022.1, you can blend reference frame and mesh motion, so possibly do all in one run. This uses multiplier functions to ramp down the application of the reference frame, and ramp up the application of the mesh motion - also using a multiplier function to yield larger time increments when the reference frame is applied, and smaller more physical time increments when the mesh motion is applied. In HyperWorks CFD this would be Motion > Rotation > Hybrid, but it doesn't write the information exactly correct, so may require manual-editing of the input file. (This will be corrected in the 2022.2 release.) I've attached a sample input file for this approach.

HydridMMO_Corrected.inp

M_22487

Thanks for the prompt reply.

I did have a clean stop on the steady state solution, so by default both nodal and restarts outputs should be written (cos i am able to re-start another steady state using last state). Not sure why its not re-starting with switch to transient.

I am using mesh motion and not reference frame. I have run a transient analysis and seems to work well. Just trying to reduce run time by using a steady condition as initial start for transient and before starting the rotation of the propeller.

I am also in the process of increasing the time step until a flow field is established (using transient) but it seems that the time step variable function is unnecessarily complicated to input. Why not just allow the user to input a time step v time function. There are so many fields to fill in for a simple task and am not sure how the function gets me what I want.

I did not see the attachment from your last reply, also if you can point me to an example on how to input a variable time step would be much appreciated.

thanks. have a great weekend.

acupro

Thanks for the prompt reply.

I did have a clean stop on the steady state solution, so by default both nodal and restarts outputs should be written (cos i am able to re-start another steady state using last state). Not sure why its not re-starting with switch to transient.

I am using mesh motion and not reference frame. I have run a transient analysis and seems to work well. Just trying to reduce run time by using a steady condition as initial start for transient and before starting the rotation of the propeller.

I am also in the process of increasing the time step until a flow field is established (using transient) but it seems that the time step variable function is unnecessarily complicated to input. Why not just allow the user to input a time step v time function. There are so many fields to fill in for a simple task and am not sure how the function gets me what I want.

I did not see the attachment from your last reply, also if you can point me to an example on how to input a variable time step would be much appreciated.

thanks. have a great weekend.

If you get a response via email, you probably won't get the attachment. If you're in the Community portal, you should be able to see the attachment in my previous response.

Which interface are you using - SimLab, HyperWorks CFD, etc?

The number of nodes cannot change with the restart.

Are you able to attach the .inp files for the steady state and transient (restart) runs - as well as the .Log file for the transient?

You can indicate time-increment as a function of time through a multiplier function (as in the previous attachment I hope you can locate above).

TIME_INCREMENT {

initial_time_increment = 0.001
multiplier_function = "Rotational - hybrid - Time Increment"
}

MULTIPLIER_FUNCTION( "Rotational - hybrid - Time Increment" ) {
type = piecewise_linear
curve_fit_variable = time_step
curve_fit_values = { 0, 1e10;
20, 1;
50, 1;
10000, 1; }
}

So from time step = 0 to time step = 20, the multiplier on the initial time increment of 0.001 ramps down linearly from 1e10 to 1.0 (meaning the time increment goes from 1e7 to 0.001), then the multiplier stays at 1 from that point on (meaning the time increment stays at 0.001).