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

CFX error (Overflow) with particular user defined material

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

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

Reply
 
LinkBack Thread Tools Search this Thread Display Modes
Old   April 9, 2020, 10:26
Default CFX error (Overflow) with particular user defined material
  #1
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 5
UsamaQ is on a distinguished road
Hello everyone,

I previously posted about getting this error in CFX everytime when I try to run simulation with user defined material.
I checked the FAQ section regarding this error and checked everything. I then tried to run the simulation with defualt material Air and it converged. So, basically my setup is okay because it converged.

Now moving on to next step, i checked the material properties as if they are correct and I am using Refprop and the values are fine.

But the error still persists, its been 4 weeks I am stuck at this point and cannot proceed further. Can someone help me?

I can provide files too if needed.

Using ANSYS 19.2.
UsamaQ is offline   Reply With Quote

Old   April 9, 2020, 15:18
Default
  #2
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,741
Rep Power: 25
Gert-Jan will become famous soon enough
I would start with uploading your complete output file. Not only small parts as in the previous posts. So we can check your setup and where the error occurs.
UsamaQ likes this.
Gert-Jan is offline   Reply With Quote

Old   April 9, 2020, 21:22
Default
  #3
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,363
Rep Power: 139
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
Please post your output file as Gert-Jan requests.

Don't forget that most of the simple build in materials (eg the default air model) are very numerically stable. This means they should converge quickly and easily. But if your material model is unstable (which looks highly likely), even if it is correct, the simulation will diverge with a floating point error. It is normal to have to take measures to improve numerical stability when you use complex custom material models.
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 10, 2020, 05:44
Default
  #4
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 5
UsamaQ is on a distinguished road
Hello,

Thank you for reply.

I have attached the output file.
Attached Files
File Type: txt output.txt (135.7 KB, 3 views)
UsamaQ is offline   Reply With Quote

Old   April 10, 2020, 06:03
Default
  #5
Senior Member
 
Gert-Jan
Join Date: Oct 2012
Location: Europe
Posts: 1,741
Rep Power: 25
Gert-Jan will become famous soon enough
Advice 0: Simplify. Go 2-3 steps back.
Advice 1: start with a simple geometry, something like a pipe. And test your material there first in the range of pressures and temperatures that you expect. If it works there, then you can progress to more complicated setups like your geometry.
Advice 2: Use more significant numbers in polynomial coefficients. If you have something like a*T^5 it makes quite a difference if a is 0.002 [K^-5] or 0.002049 [K^-5]. (Double precision won't save you). Test your polynimial equations over and over and over in a spreadsheet. Make sure the numbers are realistic.
Advice 3: start with a lower rotational speed. You can always increase speed on a restart. If you want to get to the top, don't jump, but climb, or crawl.
Advice 4: You use a pitch of 1. That means 360. Then, don't use a pitch, but just automatic.
UsamaQ likes this.
Gert-Jan is offline   Reply With Quote

Old   April 10, 2020, 06:23
Default
  #6
Super Moderator
 
Glenn Horrocks
Join Date: Mar 2009
Location: Sydney, Australia
Posts: 17,363
Rep Power: 139
ghorrocks is just really niceghorrocks is just really niceghorrocks is just really niceghorrocks is just really nice
I have given it a quick look. An obvious major problem is the out of bounds error in pressure vs enthalpy. You will need to fix this by the methods it describes as it will never converge when your material properties are being clipped.

You are also getting speeds of Mach 11 on the first time step - this is likely linked to the clipping.

Once you have fixed the clipping problem you should look at the comments listed in the FAQ. They describe the things you should consider as a first try to get convergence.
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 10, 2020, 07:49
Default
  #7
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 5
UsamaQ is on a distinguished road
Thank You. I will try to do that step by step.
UsamaQ is offline   Reply With Quote

Old   April 10, 2020, 12:04
Default
  #8
Senior Member
 
Join Date: Jun 2009
Posts: 1,688
Rep Power: 29
Opaque will become famous soon enough
May I ask the rotational speed in layman units, ie. RPM?

Your setup is at 50 000 [rad s^-1] --> 477 000+ [rpm]

I do not think the model will ever converge using a timescale of 2E-5 [min], which means the impeller basically turned more than 1 [rev] in a single timestep.
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 10, 2020, 12:18
Default
  #9
Member
 
Join Date: Mar 2020
Posts: 33
Rep Power: 5
UsamaQ is on a distinguished road
Thank you @Opaque for highlighting that silly mistake. I didn't see it was set to 50000 rad/s. It is 50000 RPM and now i see It didn't show the same error. Thank you everyone. I hope it will work fine now.

Will let you know if something happened.
UsamaQ is offline   Reply With Quote

Reply

Tags
cfd, cfx, error, overflow, turbomachinery

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
How to use user code in CFX Ugee CFX 7 January 22, 2020 16:48
User Defined Material Equation - Error message .bastian CFX 4 July 30, 2018 09:49
How to define function for material properties in CFX? Hamda CFX 3 July 29, 2018 06:09
Adding new fluid material in workbench and using it in cfx nirajpandya ANSYS 1 May 7, 2014 05:35
CFD Short Course & CFX User Day Chris Reeves CFX 0 September 11, 2000 08:53


All times are GMT -4. The time now is 13:41.