# rasidual in each cell, location of the cells with maximum residuals

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

 November 28, 2013, 09:48 rasidual in each cell, location of the cells with maximum residuals #1 New Member   Join Date: Oct 2013 Posts: 21 Rep Power: 6 Hi, is there any posibility to show me the positions of the cells, which have the highest residuals? I couldn't find something in the manual... THX!

 November 28, 2013, 10:23 #2 Member   Join Date: Jul 2013 Posts: 49 Rep Power: 6 One thing you can do, is create a user-defined field function which correspond to your model. If you are using an incompressible, then = 0 Therefore, if you create a field function which is div(V), it should show values near 0 in each cell. The value I suggest you display will not be the same as residuals, but at least it can show you what part of the domain is less precise. You can also create field-function for momentum equations, and eventually energy and turbulence, if you want to. ebringley likes this.

 November 28, 2013, 11:48 residuals #3 Member   allan thomson Join Date: Mar 2009 Location: scotland Posts: 40 Rep Power: 10 Hi There is an easier way. If you're using the segregated solver then: solver -> segregated flow-> check the temporary storage retained box in the expert properties window and run for 1 iteration. The momentum residuals will be written out to field functions. azt crevoise and Alex C. like this.

 November 29, 2013, 05:53 #4 New Member   Join Date: Oct 2013 Posts: 21 Rep Power: 6 ok thx... now i've got field functions with the residuals... but how can i see the distribution over the cells... a scalar scene didn't show anything...

 November 29, 2013, 08:57 stuff #5 Member   allan thomson Join Date: Mar 2009 Location: scotland Posts: 40 Rep Power: 10 Hi you should be able to plot these as a scalar field. you can createa report that gives you the max and min values. You can then create a threshold with say the top 10% and bottom 10% value and plot this. That's how you do it. azt

 November 29, 2013, 10:18 #6 New Member   Join Date: Oct 2013 Posts: 21 Rep Power: 6 hm... i don't get any scalar-field plots. i created a new scalar scene. Under displayers/Scalar 1, I added (under Parts) my fluid region. Under scalar field, i choose a Residual-field-function and nothing is happening. It seems that this values are empty... because it does not show any Min/Max Values. edit: i forgot to say, that i am using a cluster... so on my desktop-pc, the values are available... is there any way to save the field functions in the .sim file? there is another question: some residuals are negative... is there a way to get the values of residuals, which are displayed in the residual-plot?

 November 30, 2013, 05:17 stuf #7 Member   allan thomson Join Date: Mar 2009 Location: scotland Posts: 40 Rep Power: 10 hi you can't save temporary storage stuff to the sim file, which is a real pain. However you can write out the scaler field to a table file, and read it in later on. azt

 December 2, 2013, 06:33 #8 New Member   Join Date: Oct 2013 Posts: 21 Rep Power: 6 hi, thx! can you give me a short instruction, how to write out a scalar field to a table file?

 December 3, 2013, 07:26 #9 Member   allan thomson Join Date: Mar 2009 Location: scotland Posts: 40 Rep Power: 10 hi tools -> tables -> right click -> new table -> xyz internal table chose parts and scalars you want to export then right click -> extract then right click export Read this file in later and create a field function using the function InterpolatePositionTable see help for syntax azt

 December 10, 2013, 09:48 #10 New Member   Join Date: Oct 2013 Posts: 21 Rep Power: 6 sorry for my late answer! i will try it, thx!

 August 24, 2016, 18:17 #11 New Member   Join Date: Aug 2016 Posts: 5 Rep Power: 3 Sry for this post. After I read aztīs answer I thought this option for temporary storage retained is only available for segregated and posted my question. But you can use it for coupled or turbulence solvers, too. I wanted to delete my post, but couldnt find a way to do it.

 Thread Tools Display Modes Linear Mode

 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 OffTrackbacks are On Pingbacks are On Refbacks are On Forum Rules

 Similar Threads Thread Thread Starter Forum Replies Last Post rietuk STAR-CCM+ 8 February 27, 2013 05:50 vainilreb OpenFOAM Native Meshers: snappyHexMesh and Others 1 February 14, 2013 05:44 lentschi OpenFOAM Meshing & Mesh Conversion 1 March 9, 2011 05:49 unoder OpenFOAM Installation 11 January 30, 2008 21:30 zonexo Main CFD Forum 13 September 9, 2005 02:00

All times are GMT -4. The time now is 05:55.