periodic boundary condition

Unknown

Hi all,

I want to simulate a simple flow through a fluid domain with cylindrical steel as shown in the figure. I want to use streamwise periodic bc with specified mass flow rate. I am able to select source but I am not allowed to select target (as shown in the figure). Is this because I have an steel domain in the middle?

I tried doing the same simulation without cylindrical steel (only with water domain). At this time, I am allowed to select the opposite side as target.

Does anyone have idea why this is happening? 

acupro

Prabin Pradhananga_20428 said:

I get error at the time of meshing. I am now allowed to select source and target. With streamwise pbc, I am not able to create volume mesh. 

I am just trying to simulate a streamwise periodic flow over a cylindrical fin. Should I make any modification in my setup or am I doing any error in meshing?

 

If you don't need the actual solid volume, you can delete that, so you only have the fluid volume.  Not sure why your meshing process failed.

I've attached a .hm file and a screen recording showing how to use boundary layers in conjunction with periodics in HyperWorks CFD 2022.1.  We need to define edge layers projecting onto the source face to match the normal surface boundary layer parameters on the adjacent wall boundaries.

acupro

If possible - please attach the original CAD file imported to HWCFD, along with the HyperWorks CFD file (.hm) itself.  I don't see a problem on my simple model that looks like what you have in the image.

However - the dimensions may be very different.  What are the overall sizes of that main box in the image?  (If you can attach the .hm and CAD files, we can measure.)  If the dimensions are very small, it's possible there is a tolerance issue.  But then if the same geometry works without the second volume/solid in the middle works - for same overall dimensions - it presents an odd question.

Please attach what you can.

Unknown

acupro_21778 said:

If possible - please attach the original CAD file imported to HWCFD, along with the HyperWorks CFD file (.hm) itself.  I don't see a problem on my simple model that looks like what you have in the image.

However - the dimensions may be very different.  What are the overall sizes of that main box in the image?  (If you can attach the .hm and CAD files, we can measure.)  If the dimensions are very small, it's possible there is a tolerance issue.  But then if the same geometry works without the second volume/solid in the middle works - for same overall dimensions - it presents an odd question.

Please attach what you can.

Hi acupro,

I have a very small dimension of 30mm*30mm*5mm. I am considering periodicity from the side ways.

I have attached .hm file here. I created this geometry in hwcfd itself.

And, how to change the tolerance if it is the issue?

Thanks.

acupro

Prabin Pradhananga_20428 said:

Hi acupro,

I have a very small dimension of 30mm*30mm*5mm. I am considering periodicity from the side ways.

I have attached .hm file here. I created this geometry in hwcfd itself.

And, how to change the tolerance if it is the issue?

Thanks.

Not sure why the periodics are not being found with your geometry created in HWCFD.

While I send this to the dev team - I've attached a parasolid that appears to behave as expected.

Unknown

acupro_21778 said:

Not sure why the periodics are not being found with your geometry created in HWCFD.

While I send this to the dev team - I've attached a parasolid that appears to behave as expected.

I tried to mesh with the imported geometry you provided but I am getting error.

acupro

Prabin Pradhananga_20428 said:

I tried to mesh with the imported geometry you provided but I am getting error.

Can you be more specific?  Error at what point in the process?  Meshing? Solving?

What are the details of the problem/behavior you are trying to solve?

Can you attach your updated .hm file?

Unknown

acupro_21778 said:

Can you be more specific?  Error at what point in the process?  Meshing? Solving?

What are the details of the problem/behavior you are trying to solve?

Can you attach your updated .hm file?

I get error at the time of meshing. I am now allowed to select source and target. With streamwise pbc, I am not able to create volume mesh. 

I am just trying to simulate a streamwise periodic flow over a cylindrical fin. Should I make any modification in my setup or am I doing any error in meshing?

 

acupro

Prabin Pradhananga_20428 said:

I get error at the time of meshing. I am now allowed to select source and target. With streamwise pbc, I am not able to create volume mesh. 

I am just trying to simulate a streamwise periodic flow over a cylindrical fin. Should I make any modification in my setup or am I doing any error in meshing?

 

If you don't need the actual solid volume, you can delete that, so you only have the fluid volume.  Not sure why your meshing process failed.

I've attached a .hm file and a screen recording showing how to use boundary layers in conjunction with periodics in HyperWorks CFD 2022.1.  We need to define edge layers projecting onto the source face to match the normal surface boundary layer parameters on the adjacent wall boundaries.

Unknown

acupro_21778 said:

If you don't need the actual solid volume, you can delete that, so you only have the fluid volume.  Not sure why your meshing process failed.

I've attached a .hm file and a screen recording showing how to use boundary layers in conjunction with periodics in HyperWorks CFD 2022.1.  We need to define edge layers projecting onto the source face to match the normal surface boundary layer parameters on the adjacent wall boundaries.

Just a quick question:

What is pressure offset and what is its unit?

Is it different from pressure gradient?

Do I need to mandatorily define both mass flow rate and pressure offset?

I checked the .inp file. How to find out surface set for source and target?

acupro

Prabin Pradhananga_20428 said:

Just a quick question:

What is pressure offset and what is its unit?

Is it different from pressure gradient?

Do I need to mandatorily define both mass flow rate and pressure offset?

I checked the .inp file. How to find out surface set for source and target?

I'm assuming you are referring to the information you are seeing in the Periodic BC commands in the input file.

If I understand your case correctly, you want velocity, turbulence, to be 'periodic' - so the same value on the upstream and downstream matching nodes.  The pressure difference is unknown - the periodic condition for pressure is thus single unknown offset - AcuSolve will determine the pressure difference between the upstream/downstream matching nodes to balance everything else.  That would be the typical setup.

Per the above, you would only specify the overall flow rate, and AcuSolve will determine the velocity field, and pressure offset between inlet and outlet.

I haven't gone into the details yet in HyperWorks CFD, but I would expect the source used when defining the Periodic sets is the same in the input file.  I could suggest creating Surface Monitors - one for what you used as the source face, and another for what you used as the target.

Unknown

acupro_21778 said:

I'm assuming you are referring to the information you are seeing in the Periodic BC commands in the input file.

If I understand your case correctly, you want velocity, turbulence, to be 'periodic' - so the same value on the upstream and downstream matching nodes.  The pressure difference is unknown - the periodic condition for pressure is thus single unknown offset - AcuSolve will determine the pressure difference between the upstream/downstream matching nodes to balance everything else.  That would be the typical setup.

Per the above, you would only specify the overall flow rate, and AcuSolve will determine the velocity field, and pressure offset between inlet and outlet.

I haven't gone into the details yet in HyperWorks CFD, but I would expect the source used when defining the Periodic sets is the same in the input file.  I could suggest creating Surface Monitors - one for what you used as the source face, and another for what you used as the target.

Thanks for your explanation!

You said the pressure difference is unknown - the periodic condition for pressure is thus single unknown offset. Then, why is there pressure offset? What happens if i specify pressure offset? 

Also, what is this thermal forcing mechanism (constant heat flux/constant temperature)?

Thanks!

acupro

Prabin Pradhananga_20428 said:

Thanks for your explanation!

You said the pressure difference is unknown - the periodic condition for pressure is thus single unknown offset. Then, why is there pressure offset? What happens if i specify pressure offset? 

Also, what is this thermal forcing mechanism (constant heat flux/constant temperature)?

Thanks!

It looks like the dev team needs to take another look at these panels for Periodic BCs.  They don't seem consistent with the input file itself - where single unknown offset should be the condition for pressure in your case.  It may write both single unknown offset, and constant value.  But with type = single_unknown_offset, the constant value will be ignored.

Thermal periodicity is a bit more difficult to determine.  The simplest periodic conditions are for boundaries that are either constant temperature or constant heat flux.  One will yield temperature PBC type single unknown offset and the other will yield temperature PBD type single unknown ratio.  I believe the wall with fixed temperatures matches with single temperature PBC type single unknown ratio.  You can check that after you write the input file.

In other words, if your solid is kept at a constant temperature (really only need the boundary - not the actual volume) the PBC for temperature would be Constant Temperature in the GUI, and should yield single unknown ratio in the input file.  If your solid has a heat source instead (or the surface has constant heat flux), then it would likely write single unknown offset in the input file.