[lubrigap]

Hello everyone,


I am currently stuck and seeking for help from some real professionals


I am simulating a threedimensional, unsteady and laminar hydrodynamical bearing with a field function as input for the angular velocity (local rotation rate) of the journal/shaft.
The eccentricity is constant in negative horizontal direction.


SHORT VERSION:
When simulating unsteady the pressure results are 10x the steady pressure data.
Probably a problem with the way Star-CCM+ interpolates.




LONG VERSION:
The (local) rotation rate is set by a scalar field function. Let's name it AAA.
The function says:
interpolateTable(@Table("tableTestnew"), "Time", LINEAR, "RPM", $Time)


The table (tableTestnew) consists of:
Time, RPM
0, 0
1, -1
5, -70
8, -97
9, -99
10, -100
11, -99
12, -97
15, -70
19, -1
20, 0


Now in addition to just viewing the pressure scene or plot, a report, monitor and plot were created for viewing the curse of the interpolated table.
Also annotations in the pressure scene show the current time step, solution time, pressure maximum/minimum, current rpm (made as report -> expression -> AAA), iteration, plot of AAAs course and residuals.
When setting the simulation with following criteria:
time step: 0.001s; inner iterations: 15, maximum physical time: 20s and enough maximum steps (way over 300 000)
the current rpm annotation is showing ca. 10x the rpm than it should BUT the plot (made out of the monitor made out the report) is showing the "real" interpolated data points. In addition to that the pressure is (probably) linked to the ("wrong") annotation rpm.
Images are attached




What i already found out/did:
-When simulating steady (with -100 rpm local rotation rate) the pressure results are in between ca. -1290 and + 1330 Pa.
But when simulating unsteady with rpm changing over time the pressure results are in between ca. -14000 and +14000 Pa.
-for time step 1s courant numbers go up to 70 000. but pressure results are almost the same. when setting time step to 0.001s the courant number goes max. double digits.
-regions are created correctly
-physics are set up right
-table data has been refreshed and updated
-mesh size and grid numbers are pretty good (just trust me)


and steady results are correct as they already have been compared to experimental results.






If there's anybody out there who could help in any kind of way I'd highly appreciate it as I am still a student.
Thanks in advance!










if you need more info lmk!
p { margin-bottom: 0.25cm; line-height: 115%; background: transparent }

[SESP]

Hi,

this is not easy from your post (although nicely described). My guess would be that you have somehow implemented a wrong definition of the rotation for the unsteady case. You know that for the unsteady case you need a real rotation (RBM or overset), an unsteady MRF simulation does not make too much sense... The interpolation in STAR from the tables works well, and it works well for steady-state MRF and unsteady body motion simulations. So the error is probably in the setup. Also make your you did not mix up dimensions, because your annotation should actually be consistent with your functions, so I would focus to get that clean as well to avoid any errors...

Viel Glück
Sebastian

[lubrigap]

Hey Seb,

first of all Danke !


I did find the error. It has to do with the way STAR-CCM+ automatically sets the dimensions. My imported table should be read as rpm but the software sets it as rad/s. That's the sticking point aka knackpunkt. To my knowledge there is no possibility of changing.
In the end I converted my table data to rad/s and the results were good.
But still I couldn't figure out why the plot of the angular velocity was shown in "correct" rpm but the annotations, made from the same report, showed the converted "wrong" velocity.

The weird constant came along with the ratio (about 9.55).
So that's that.



Little remark for everybody struggling:
If a problem comes up while simulating, 90% of time it's your fault. Otherwise just restart.



Mahlzeit

[SESP]

Ok, glad to hear you solved it!

To my experience, most of the CFD solvers (actually all I can think of) work with rotation rates in [rad/s]. You should be able to have the table in rpm and then declare the units in STAR as well, but probably not too relevant since its solved...

Cheers!

[cwl]

You should be able to have the table in rpm and then declare the units

Actually - rpm is a declared standard unit. Yet importing tables sometimes brings pain with units.