Hi,
Am currently working on a model which includes culverts.
As part of the study I am investigating the influence of the culverts on water exchange which is modelled using a conservative tracer. My understanding is that the culverts would conserve the tracer mass, however, I can clearly see in the results that transport of the tracer between the source and sink sides of the culvert is not working correctly. It seems that the source of the culvert has a difference tracer concentration to the sink side.
As you can see in the attached figures, tracer is initialized to a value of 100 on either side of the culvert. A few time steps later, the tracer concentration is significantly reduced suggesting that the culvert source has a tracer concentration below 100 (perhaps 0).
Has anybody experienced this before?
Many thanks,
[name removed]
Hi [name removed]
I agree that culverts should conserve tracer and in your case it’s not seems to be the case…
I have in mind a case where we had problems with the tracer numbering dur to a bug few years ago.
For me this was corrected but maybe you use an old version?
By the way, you could easily check by using 2 tracers (one with 100, the second with 200) and see if the problem exists for both…
Hope this helps
Hi [name removed],
Thanks for the quick response. I’m currently on the latest V8P4 version so that shouldn’t be an issue. I am however using a computation restart file to initialize the tracer concentration so am wondering if this has anything to do with it.
Will try to include another tracer over the same area but different number to see if that resolves the issue.
[name removed]
Hi [name removed],
Changing the tracer number doesn’t seem to influence the results. In this case I modelled the same initial tracer concentration but using TR3 instead of TR1. Am trying to write the tracer concentration outputs for one of these culvert nodes to understand what is going on.
[name removed]
So have spent the day trying to debug the issue inside BUSE and DIFSOU but cannot figure out what is going on.
Have confirmed that all I1 and I2 nodes are correct etc. I’ve attached my .CAS file and culverts file for further debugging if anyone is interested in taking a look. Unfortunately I need to deliver this study quite soon and wasn’t expecting to run into something like this.
If anyone has a clue what might be going on would be really much appreciated if you could reach out to me.
Many thanks,
[name removed]
NISI_PRODUC_FLUSH_004.cas (6.99 KB)
01_Temporary_EastLink_Culverts.txt (32.2 KB)
Did you tried with option for culvert 1?
You confirm the discharge computation is OK?
Hi [name removed],
Will run a test with Opt 1 but the computed flows with Opt 2 appear to be correct. Attached is a timeseries of TELEMAC computed total flow rates (summed over all culverts) through the causeway section previously shown.
Also shown is the total flow rate estimated using the same [name removed] eqns. but using water levels extracted from a model run excluding the culverts. I attribute the reduction in computed flow due to the likely reduction in head once the culverts are in place.
Will get back to you once I have some results with Opt 1.
Regards,
Thanks for the clarifications.
According to these results, I agree switching to opt 1 will not solve the problem
Maybe a final test could be to run in sequential rather in parallel
Regards
Unfortunately sequential doesn’t change the results either.
Been using single core while trying to debug the issue today.
And with a limited number of culvert?
Hello [name removed],
Sorry, it seems that you have found a bug dealing with culverts and LIPS.
Can you try to change the advection scheme and switch LIPS to NERD e.g. (13).
I have tried with TELEMAC-2D test case siphon and it seems to better work.
In addition to tracers, you may also need to change LIPS for velocity components, I have not tried.
Unfortunately, our LIPS scheme specialist will not be able to answer for months and it may take me some times to understand what the issue is with LIPS (and not in a close future).
Hope this helps,
[name removed]
Looking into the source code of DIFSOU.f on line 329 or 332 I cannot quite work something out.
Writing the value of MASSOU(ITRAC) immediately after it is defined for a source point along the culvert I am getting an output value of zero. However, computing the actual mass of tracer according to the below I am getting a non-zero value
DT*DBUS(I)*BUS%ADR(ITRAC)%P%R(NBUSE+I)
Not really understanding why this is happening as my Fortran skills are limited, although if it is indeed zero then I would assume that no tracer mass but an increase in cell volume may cause such an unrealistic dilution.
Hi [name removed],
Thanks for your response - didn’t catch it before my last reply.
Will try with the NERD scheme for advection of velocities and tracers. I guess a ‘SCHEME FOR ADVECTION OF VELOCITIES’ = 1 would be required to avoid LIPS?
Do you know if there is any major difference between scheme 13 or 14 as I haven’t used them a whole lot?
Hi [name removed],
Can confirm the tracer transport is working correctly now with Scheme 13
Thanks very to both yourself and [name removed] for the assistance in debugging this.
Regards,
1 Like
Yes, I would use characteristics (= 1) if LIPS does not work for velocities.
If I remember, schemes 13 and 14 can give different results if there are dry areas. I have not investigated deeply but I think there are not so many basic differences of implementation.
Hope this helps,
[name removed]
Hi [name removed] and [name removed],
Was wondering if either of you had carried out any sensitivity analysis on the model calculated flow rates relative to the cell size at the upstream and downstream nodes before?
What I am seeing is that the model calculated flow rates are substantially smaller than those I estimated by hand using the same [name removed] equations but using modelled water levels without the culverts in place.
It seems that for my larger culverts, changes to the water levels locally at the culvert nodes are more pronounced which may be artificially influencing the head. I can imagine that with larger cell volumes changes to the WL at the culvert nodes would be less pronounced.
[name removed]
Hi [name removed]
No sensitivity analysis conducted on my side but totally agree with your analysis.
The culvert functionality had been developed to take into account the effect of existing and potentially in charge connections in the flow when those structures are smaller than the mesh size without refining the model.
Small structure implicitly means small discharge then small velocities and by consequence allow to consider free surface as head…
Using this capability in case of large structure could leads to erroneous results due to violation of these assumptions.
In case of significant velocity there is probably some adaptation to envisage (enlarge artificially the structure, modify buse.f file to use head instead of free surface)
Hope this helps
Hi [name removed],
Thanks - once I have some time I may try to modify BUSE.f to take water levels from nodes 1 or 2 points away from the culvert node and see if that improves the results.
Alternatively, as you mentioned, artificially increasing the culvert size may work, however its difficult to know a priori what flow rate to be targeting.
[name removed]
Hi,
Just wondering whether there has been any progress in addressing this bug in recent updates? I wasn’t able to see any updates on the GitLab change logs so assume that nobody has had an opportunity to address it at this stage.
It would be great to be able to use the PSI LIPS scheme for advection of tracers when applying culverts as the alternative schemes are rather diffusive.
[name removed]
