[AmreD]

Hello,


I am running a flow simulation on a centrifugal compressor. This compressor uses the fluid R1233ZD. I used the Fluent beta features python code to generate a .rgp file from REFPROP and insert this material into CFX. When running the simulation, I get two issues which I think might be related.



The first is that some values are out of bounds, I know the fix to that is to increase the range of the tables in the RGP file, which I've been doing incrementally.



The second issue which seems more important is the "A wall has been placed" notice. I've gotten this and fixed it before but this time it is rather odd as the fluid specified in the notice is Air at 25C which is really strange. I am certain and I double checked that the fluid for the simulation is R1233ZD. I'm sure I didn't just add a new material without choosing it as the simulation fluid.


I've attached the CFX solver output. Unfortunately, I couldn't attach the rgp file as it is too large.



Thanks to everyone that posts questions on this forum, it's a great place!

[Opaque]

It seems you modified a previous case that used a fluid named Air at 25C, and you just replaced the material but forgot to rename the fluid.

Keep in mind that an Ansys CFX MATERIAL, is not an Ansys CFX FLUID.

A MATERIAL is the thermodynamic representation.

A FLUID is the CFD representation of a "thing" that can be made of a combination of materials, and can be modeled as a continuous, discrete, etc.

Summary: you forgot to rename the FLUID DEFINITION under DOMAIN.

[AmreD]

Originally Posted by Opaque

It seems you modified a previous case that used a fluid named Air at 25C, and you just replaced the material but forgot to rename the fluid.

Keep in mind that an Ansys CFX MATERIAL, is not an Ansys CFX FLUID.

A MATERIAL is the thermodynamic representation.

A FLUID is the CFD representation of a "thing" that can be made of a combination of materials, and can be modeled as a continuous, discrete, etc.

Summary: you forgot to rename the FLUID DEFINITION under DOMAIN.

Hello,


Thanks a lot. That was exactly the reason for the strange naming. But that is indeed all it was, the name of the fluid.

I'm still having issues with values being out of the table bounds and the wall notice but I'll try to solve those issues on my own.

[Opaque]

Originally Posted by AmreD

Hello,


Thanks a lot. That was exactly the reason for the strange naming. But that is indeed all it was, the name of the fluid.

I'm still having issues with values being out of the table bounds and the wall notice but I'll try to solve those issues on my own.

I forgot to look into the other issue.

You are using the default initialization, i.e. no information, and it is not good enough for your case.

Try setting at least:
1 - Some velocity values
2 - A Static pressure value
3 - A temperature based on the inlet total temperature, and consistent with your velocity field. say T = Ttot_inlet - magnitudeV^2 / (2*Cp)
4 - Turbulence condition identical to the inlet conditions.

You can tell the initial guess is poor by looking at the Linear Solution diagnostics:

======================================================================
 OUTER LOOP ITERATION =    1                    CPU SECONDS = 7.432E+01
 ----------------------------------------------------------------------
 |       Equation       | Rate | RMS Res | Max Res |  Linear Solution |
 +----------------------+------+---------+---------+------------------+
 | Wallscale            | 0.00 | 3.2E-04 | 4.0E-03 | 41.3  2.8E-01  ok|
 +----------------------+------+---------+---------+------------------+
 | U-Mom                | 0.00 | 3.2E-04 | 3.2E-02 |       7.2E-02  OK|
 | V-Mom                | 0.00 | 2.7E-04 | 2.2E-02 |       1.2E-01  ok|
 | W-Mom                | 0.00 | 4.9E-04 | 7.0E-02 |       3.7E-01  ok|
 | P-Mass               | 0.00 | 4.5E-04 | 1.2E-02 | 18.9  9.8E-02  OK|
 +----------------------+------+---------+---------+------------------+
 | H-Energy             | 0.00 | 4.0E-03 | 3.8E-01 |  6.0  2.5E-02  OK|
 +----------------------+------+---------+---------+------------------+
 | K-TurbKE             | 0.00 | 1.1E-01 | 7.9E-01 |  6.0  5.1E-03  OK|
 | O-TurbFreq           | 0.00 | 5.8E-02 | 1.0E+00 | 18.6  2.4E-04  OK|
 +----------------------+------+---------+---------+------------------+

You want the 18.6 number to be @9 - 12 at most for the Mom-Mass system. To do so, you may need to reduce your timescale a bit, i.e. Timescale Factor < 1

[AmreD]

Originally Posted by Opaque

I forgot to look into the other issue.

You are using the default initialization, i.e. no information, and it is not good enough for your case.

Try setting at least:
1 - Some velocity values
2 - A Static pressure value
3 - A temperature based on the inlet total temperature, and consistent with your velocity field. say T = Ttot_inlet - magnitudeV^2 / (2*Cp)
4 - Turbulence condition identical to the inlet conditions.

You can tell the initial guess is poor by looking at the Linear Solution diagnostics:

======================================================================
 OUTER LOOP ITERATION =    1                    CPU SECONDS = 7.432E+01
 ----------------------------------------------------------------------
 |       Equation       | Rate | RMS Res | Max Res |  Linear Solution |
 +----------------------+------+---------+---------+------------------+
 | Wallscale            | 0.00 | 3.2E-04 | 4.0E-03 | 41.3  2.8E-01  ok|
 +----------------------+------+---------+---------+------------------+
 | U-Mom                | 0.00 | 3.2E-04 | 3.2E-02 |       7.2E-02  OK|
 | V-Mom                | 0.00 | 2.7E-04 | 2.2E-02 |       1.2E-01  ok|
 | W-Mom                | 0.00 | 4.9E-04 | 7.0E-02 |       3.7E-01  ok|
 | P-Mass               | 0.00 | 4.5E-04 | 1.2E-02 | 18.9  9.8E-02  OK|
 +----------------------+------+---------+---------+------------------+
 | H-Energy             | 0.00 | 4.0E-03 | 3.8E-01 |  6.0  2.5E-02  OK|
 +----------------------+------+---------+---------+------------------+
 | K-TurbKE             | 0.00 | 1.1E-01 | 7.9E-01 |  6.0  5.1E-03  OK|
 | O-TurbFreq           | 0.00 | 5.8E-02 | 1.0E+00 | 18.6  2.4E-04  OK|
 +----------------------+------+---------+---------+------------------+

You want the 18.6 number to be @9 - 12 at most for the Mom-Mass system. To do so, you may need to reduce your timescale a bit, i.e. Timescale Factor < 1

Thank you very much. This is certainly helpful.

This is by far the most complex simulation I've attempted so I guess my usual plan of running an upwind scheme simulation to then use as the initial condition doesn't work for this. I'll try these options and report back.

As for the timescale, I'm already using an auto timescale at 0.1. I was taught to start small, around 0.2 and then possibly increase it as the residuals plateau. Is that reasonable?


Thanks again!