CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > Software User Forums > ANSYS > CFX

CFX error

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

Like Tree5Likes
  • 1 Post By AtoHM
  • 1 Post By ghorrocks
  • 1 Post By Gert-Jan
  • 1 Post By Opaque
  • 1 Post By Opaque

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 18, 2020, 11:09
Default CFX error
  #1
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 6
UsamaQ is on a distinguished road
Hello everyone,

I am trying to run simulation of compressor but I am getting error again and again, I have checked boundary conditions, changed time scale, model everything but the solution is diverging. Can someone please look at output file and tell me what is wrong. I have checked CFX wiki but still couldnt solve the issue.

Thank you
Attached Files
File Type: txt output.txt (68.3 KB, 5 views)
UsamaQ is offline   Reply With Quote

Old   April 18, 2020, 12:04
Default
  #2
Senior Member
 
M
Join Date: Dec 2017
Posts: 658
Rep Power: 12
AtoHM is on a distinguished road
Something is at least wrong with your mesh, look at the expansion ratios it shows in the Mesh Statistics section. And your Mach number is skyrocketting, its related I guess.
UsamaQ likes this.
AtoHM is offline   Reply With Quote

Old   April 18, 2020, 18:33
Default
  #3
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 6
UsamaQ is on a distinguished road
Hey. Thank you. I believe this is due to the mesh because I checked antoher converged solution of kinda same geomtry but less than 1000 expansion ratios. I will try to improve mesh. Will let you know
UsamaQ is offline   Reply With Quote

Old   April 19, 2020, 00:10
Default
  #4
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,746
Rep Power: 143
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
The rapidly diverging Mach number means that the FAQ on floating point error is relevant here (it is a very similar problem): https://www.cfd-online.com/Wiki/Ansy...do_about_it.3F

* The mesh quality issue is very important, definitely need to improve that.
* You have viscous work turned on. Unless you need it turn it off.
* Are you sure the flow is not choked?
* As the FAQ says, the first things you try in this case are: double precision numerics, smaller time step, improve mesh quality, better initial conditions.
UsamaQ likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
ghorrocks is offline   Reply With Quote

Old   April 20, 2020, 04:00
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,837
Rep Power: 27
Gert-Jan will become famous soon enough
Another 50 cents:
You have challenging boundary conditions. And you use them all starting from iteration 1, without any initial guess.
I would start with a lower massflow and rotational speed. Get it converged and then restart with tougher settings. Do it over and over, until you get where you want to be.

Although CFX can be quite forgiven for bad mesh and tough boundary conditions, I think you push it too far. You want to be on top of a mountain and try to jump to get there at once. But you need to climb and take a rest a few times.
UsamaQ likes this.
Gert-Jan is offline   Reply With Quote

Old   April 20, 2020, 18:14
Default
  #6
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 6
UsamaQ is on a distinguished road
Thank you so much guys. I refined the mesh, reduced mass flow rate and velocity and it finally converged. One thing is still confusing me, the direction of rotational velocity. I have attached the image, can you please tell me for clockwise rotation about z-axis (from the top view), should input velocity be positive or negative? How can I check it in post?
Attached Images
File Type: png Capture.PNG (37.4 KB, 11 views)
UsamaQ is offline   Reply With Quote

Old   April 20, 2020, 21:15
Default
  #7
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
Your last question is ill-posed. You are showing the impeller, and a coordinate frame in a viewer, but you have not explicitly stated/described nor shown which direction for the axis you selected.

You can still in the domain models panel select -Z as the axis, and any answer to your question will be wrong or right.

For anyone to help, you need to state the direction of the axis by either showing the panel, or indicating which axis direction you have selected.

Hope the above helps,
UsamaQ likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   April 21, 2020, 13:14
Default
  #8
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 6
UsamaQ is on a distinguished road
Hello. Sorry for the missing information. I selected the positive Z-axis (axis 1.3) as axis of rotation.
UsamaQ is offline   Reply With Quote

Old   April 21, 2020, 14:41
Default
  #9
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
For a compressor, the impeller must rotate from the Y-axis towards (using the shortest angle) the X-axis; therefore, then you must set a negative value for the angular velocity in the panel.
UsamaQ likes this.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Old   April 21, 2020, 14:55
Default
  #10
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 6
UsamaQ is on a distinguished road
Thank You. I already set negative value. was just need confirmation if doing it right or not.
UsamaQ is offline   Reply With Quote

Old   April 23, 2020, 11:13
Default
  #11
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 6
UsamaQ is on a distinguished road
Hey Guys, I am facing aproblem regarding inflation layer. I am trying to place inflation layers around blades by appropriate first layer thickness (y plus 1), the inflation layer is generated but the mesh quality decreases and Aspect ratio + Expansion ratios becomes very high. This is causing the solver to diverge.

How can I solve this issue? If I remove inflation layers, the solution converges.
UsamaQ is offline   Reply With Quote

Old   April 23, 2020, 12:51
Default
  #12
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,837
Rep Power: 27
Gert-Jan will become famous soon enough
Go to ANSYS' Mesh & Geometry forum and add a few pictures. Otherwise people can't help at all.
Gert-Jan is offline   Reply With Quote

Old   April 23, 2020, 13:11
Default
  #13
Senior Member
 
Join Date: Jun 2009
Posts: 1,825
Rep Power: 33
Opaque will become famous soon enough
"boundary layer" meshes have very high aspect ratio. That is the norm.

Once your aspect ratio goes above 1000, you should use the double precision solver, and also beware that you are resolving additional features you did not capture with the coarser meshes.

As Gert-Jan suggested, a picture is worth a thousand words.
__________________
Note: I do not answer CFD questions by PM. CFD questions should be posted on the forum.
Opaque is offline   Reply With Quote

Reply

Tags
ansys, cfx, error, turbo machinery

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
Compile calcMassFlowC aurore OpenFOAM Programming & Development 13 March 23, 2018 07:43
[swak4Foam] GroovyBC the dynamic cousin of funkySetFields that lives on the suburb of the mesh gschaider OpenFOAM Community Contributions 300 October 29, 2014 18:00
Undeclared Identifier Errof UDF SteveGoat Fluent UDF and Scheme Programming 7 October 15, 2014 07:11
How to install CGNS under windows xp? lzgwhy Main CFD Forum 1 January 11, 2011 18:44
Compiling problems with hello worldC fw407 OpenFOAM Installation 21 January 6, 2008 17:38


All times are GMT -4. The time now is 15:24.