Heat flux distribution plot

Feroz

I have a log file showing various contour plots. I am mainly looking at the temperature distribution. Is there a way to get a heat flux distribution contour plot? 

acupro

You can get heat flux contours on surfaces.

Step1 - Make sure you activate (set to a non-zero value) for either nodal_output_frequency or nodal_output_time_interval for the Surface Output on the surfaces where you want heat flux contours.

1A - For surfaces with Boundary Conditions applied - click the 'pencil' to the right of 'Create Linked Surface Output' to see the Nodal output entries

Step2 - In post-processing you need to enable the read of extended output, as nodal heat flux becomes part of extended nodal output.  Or - if translating to other formats for reading, make sure you add the flag for extended output.

acupro

You can get heat flux contours on surfaces.

Step1 - Make sure you activate (set to a non-zero value) for either nodal_output_frequency or nodal_output_time_interval for the Surface Output on the surfaces where you want heat flux contours.

1A - For surfaces with Boundary Conditions applied - click the 'pencil' to the right of 'Create Linked Surface Output' to see the Nodal output entries

Step2 - In post-processing you need to enable the read of extended output, as nodal heat flux becomes part of extended nodal output.  Or - if translating to other formats for reading, make sure you add the flag for extended output.

Feroz

acupro_21778 said:

You can get heat flux contours on surfaces.

Step1 - Make sure you activate (set to a non-zero value) for either nodal_output_frequency or nodal_output_time_interval for the Surface Output on the surfaces where you want heat flux contours.

1A - For surfaces with Boundary Conditions applied - click the 'pencil' to the right of 'Create Linked Surface Output' to see the Nodal output entries

Step2 - In post-processing you need to enable the read of extended output, as nodal heat flux becomes part of extended nodal output.  Or - if translating to other formats for reading, make sure you add the flag for extended output.

Hi, thanks for the answer. But i am a little confused still. 

So i select a BC and check the linked surface output settings. Are these the expected settings to enable this?

Regarding step 2, does this only work in Hyperworks CFD, or Hyperview? 

acupro

Feroz said:

Hi, thanks for the answer. But i am a little confused still. 

So i select a BC and check the linked surface output settings. Are these the expected settings to enable this?

Regarding step 2, does this only work in Hyperworks CFD, or Hyperview? 

By default, the surface has Integrated and Statistics output every time step.  (You'll see these in the Plot tool in HyperWorks CFD - or in the older AcuProbe tool.)

If you want to see the nodal heat flux on the surface within the post-processing (HyperWorks CFD Post or HyperView) you'll need to set the 'Nodal' entry to a non-zero value.  If you're running a steady-state case, and only looking at the last time step in Post, you can use the same large number as is the typical value for the overall Nodal output.  For example, if you set Output Frequencies / Nodal to 1000 - it will write the additional Nodal output on that surface every 1000 time steps, or when the job does a clean stop (either reaches the convergence level, or a user-activated stop).  If you're running transient, and writing the main Nodal output every 10 time steps, for example, then you would also set Output Frequencies / Nodal to that same 10.

In HyperView click on Reader Options > AcuSolve Result Reader and set Extended Nodal Output to Yes.  (This is if you point to the .Log file to load the results.)

Feroz

acupro_21778 said:

By default, the surface has Integrated and Statistics output every time step.  (You'll see these in the Plot tool in HyperWorks CFD - or in the older AcuProbe tool.)

If you want to see the nodal heat flux on the surface within the post-processing (HyperWorks CFD Post or HyperView) you'll need to set the 'Nodal' entry to a non-zero value.  If you're running a steady-state case, and only looking at the last time step in Post, you can use the same large number as is the typical value for the overall Nodal output.  For example, if you set Output Frequencies / Nodal to 1000 - it will write the additional Nodal output on that surface every 1000 time steps, or when the job does a clean stop (either reaches the convergence level, or a user-activated stop).  If you're running transient, and writing the main Nodal output every 10 time steps, for example, then you would also set Output Frequencies / Nodal to that same 10.

In HyperView click on Reader Options > AcuSolve Result Reader and set Extended Nodal Output to Yes.  (This is if you point to the .Log file to load the results.)

Hello, apologies for the late reply. 

I tried this method. I set a few probe, surface and volume monitors with non-zero nodal outputs. Then I ran my simulation as usual. 

When i opened my log file in hyperview i could see my temperature distribution plot as usual. Then i selected "Reader Options" and chose "Acusolve result reader" and selected "Apply".

I received a warning noting: "the data type of grad_incident_radiation, 1, is not supported"

Now my results have disappeared. 

Do you have any insights on this? 

acupro

Feroz said:

Hello, apologies for the late reply. 

I tried this method. I set a few probe, surface and volume monitors with non-zero nodal outputs. Then I ran my simulation as usual. 

When i opened my log file in hyperview i could see my temperature distribution plot as usual. Then i selected "Reader Options" and chose "Acusolve result reader" and selected "Apply".

I received a warning noting: "the data type of grad_incident_radiation, 1, is not supported"

Now my results have disappeared. 

Do you have any insights on this? 

The HyperView direct reader (through .Log file) may not be 100%, depending somewhat on the version.  You can also try converting/translating the AcuSolve results to H3D format.

acuTrans -out -extout -to info -pb <problem_name>

will give you the available variables, then you can translate your desired variables using the -outv option:

acuTrans -out -extout -to h3d -outv velocity,heat_flux,velocity_magnitude

The comma-separated list are the variables you want, based on those available from the first command above