CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > Siemens > STAR-CCM+

Star-CCM+ | interpolation bugs

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 7, 2021, 10:26
Default Star-CCM+ | interpolation bugs
  #1
New Member
 
Join Date: Apr 2021
Posts: 2
Rep Power: 0
lubrigap is on a distinguished road
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 }
Attached Images
File Type: jpg 01.jpg (109.6 KB, 3 views)
File Type: jpg 02.jpg (109.5 KB, 2 views)
lubrigap is offline   Reply With Quote

Old   April 12, 2021, 10:03
Default
  #2
New Member
 
Join Date: Mar 2011
Posts: 17
Rep Power: 13
SESP is on a distinguished road
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
SESP is offline   Reply With Quote

Old   April 14, 2021, 08:44
Lightbulb
  #3
New Member
 
Join Date: Apr 2021
Posts: 2
Rep Power: 0
lubrigap is on a distinguished road
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 \frac{rpm}{rad/s} 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
lubrigap is offline   Reply With Quote

Old   April 15, 2021, 04:50
Default
  #4
New Member
 
Join Date: Mar 2011
Posts: 17
Rep Power: 13
SESP is on a distinguished road
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!
SESP is offline   Reply With Quote

Old   April 15, 2021, 10:10
Default
  #5
cwl
Senior Member
 
Chaotic Water
Join Date: Jul 2012
Location: Elgrin Fau
Posts: 251
Rep Power: 13
cwl is on a distinguished road
Quote:
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.
cwl is offline   Reply With Quote

Reply

Tags
annotations, bug, error, i dont even know man, interpolate

Thread Tools Search this Thread
Search this Thread:

Advanced Search
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are Off
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
problem when imported geometry from 3D CAD to star ccm, TAREK GANAT STAR-CCM+ 1 May 21, 2013 22:15
[Commercial meshers] Using starToFoam clo OpenFOAM Meshing & Mesh Conversion 33 September 26, 2012 04:04
[Other] StarToFoam error Kart OpenFOAM Meshing & Mesh Conversion 1 February 4, 2010 04:38
error in star ccm maurizio Siemens 3 October 16, 2007 05:17
[Commercial meshers] Trimmed cell and embedded refinement mesh conversion issues michele OpenFOAM Meshing & Mesh Conversion 2 July 15, 2005 04:15


All times are GMT -4. The time now is 12:42.