Engine-design: air intake

[thschrader]

Hello everyone!

There is a discussion in the german forum about designing
the air intake of a four-stroke Audi racing engine.
https://forum.freecadweb.org/viewtopic. ... 6&start=90
https://forum.freecadweb.org/viewtopic. ... 5&start=70

At the moment we use simplefoam-solver with steady/single-phase/incompressible option.
Does it makes sense to use the new Hisa-solver for such a problem?
Would be nice to see a pressure-wave / temperature-distribution running
through the engine.

At full-throttle the engine runs at 7500 rpm.
Stroke 92,8 mm, drilling 84 mm.
This gives an average mass-flow (inlet condition) of 31 grams air/sec.
The average air speed is approx 20 m/s, max piston speed is 73 m/s,
That are obviously not high-mach numbers.

When having a look at fvSchemes, there is the word „rPseudoDeltaT“.
Is Hisa a „pseudo-transient“-method? If so, how must I interpret the iteration-steps?
@Oliver: a tutorial about hisa would be sooo nice.

Comments/ideas welcome.
Thomas

air_intake.JPG (89.44 KiB) Viewed 2428 times

hisa_case.JPG (24.11 KiB) Viewed 2428 times

[oliveroxtoby]

The average air speed is approx 20 m/s, max piston speed is 73 m/s,
That are obviously not high-mach numbers.

As a density-based solver, HiSA is best used at Mach numbers > 0.3. A pressure-based compressible solver such as rhoSimpleFoam/rhoPimpleFoam would probably be best here.

When having a look at fvSchemes, there is the word „rPseudoDeltaT“.
Is Hisa a „pseudo-transient“-method? If so, how must I interpret the iteration-steps?
@Oliver: a tutorial about hisa would be sooo nice.

Dual timestepping with local timestepping is used to converge the steady state solution. The pseudo-timestep used for this has no relation to actual time and is automatically computed to converge as quickly as possible.

There are some example cases in the source - see hisa.gitlab.io

[thschrader]

There are some example cases in the source - see hisa.gitlab.io

Hello Oliver,
sorry, I have overlooked the Hisa-tutorials on gitlab.

I am trying to rebuild the basic-finner tutorial with FC.
http://hisa.gitlab.io/archive/asc/basic ... inner.html

How can I generate the nice mesh (or a mesh closed to this)
you used in the tutorial? I have set a basic element-size of 300 mm
(the cube in the corner) and 3 refinement boxes (refinement level 0,5 each box)
and at least a surface refinement of 0,2 with 5 boundary layers. As a start.
Meshing works, but the boundary-layers are located wrong.
According to the uav-tutorial: must I first set the surface refinement of
the body and after that the volume refinement? Is there a special order needed
of the mesh-refinement objects in the model tree?
I used a finner with a diameter of 200 mm and the dimensions
from the tutorial.

I downloaded the shockTube tutorial from gitlab and did a run with
bluecfd. No problems.

Air intake Audi-engine and my wrong thoughts about using Hisa:
At 7500 rpm the piston needs 0,004 seconds from the upper dead-point
to the lower dead- point („loading“-phase). Can the air follow this movement?
At atmospheric pressure of 100 kPa and a „vacuum“ in the cylinder
the air would fill the vacuum with approx 400 m/s. But the max piston speed is
at 70 m/s, the air cant be faster. This gives a Mach-number of 0,2,
I think for a non-scientific approach the use of simpleFoam solver is ok.
Thomas

mesh_finner_tutorial.JPG (123.94 KiB) Viewed 2353 times

meshRefinement.JPG (110.59 KiB) Viewed 2353 times

cfmesh-finner.JPG (80.83 KiB) Viewed 2353 times

boundary_layer.JPG (101.43 KiB) Viewed 2353 times

[oliveroxtoby]

I am trying to rebuild the basic-finner tutorial with FC.
http://hisa.gitlab.io/archive/asc/basic ... inner.html

How can I generate the nice mesh (or a mesh closed to this)
you used in the tutorial? I have set a basic element-size of 300 mm
(the cube in the corner) and 3 refinement boxes (refinement level 0,5 each box)
and at least a surface refinement of 0,2 with 5 boundary layers. As a start.
Meshing works, but the boundary-layers are located wrong.

The mesh shown was generated with different meshing tool to cfMesh (Hexpress Hybrid I think). However your mesh looks OK to me. Have you tried selecting the symmetry plane and un-setting boundary layers on that patch?

According to the uav-tutorial: must I first set the surface refinement of
the body and after that the volume refinement? Is there a special order needed
of the mesh-refinement objects in the model tree?
I used a finner with a diameter of 200 mm and the dimensions
from the tutorial.

No special order needed.

[thschrader]

Have you tried selecting the symmetry plane and un-setting boundary layers on that patch?

No, how can I do this in the GUI?

I have the same problem when using a cylinder. The boundary layer elements
are located correct, when the cylinder is as long (or longer) than the cube.
When the cylinder is inside the cube, the boundary elements are located wrong.
I experimented hours but cant find the reason.

meshTest.FCStd

(13.95 KiB) Downloaded 66 times

cyl1.JPG (39.65 KiB) Viewed 2262 times

boundary_layer_ok.JPG (237.85 KiB) Viewed 2262 times

boundary_layer_wrong.JPG (193.25 KiB) Viewed 2262 times

[oliveroxtoby]

Have you tried selecting the symmetry plane and un-setting boundary layers on that patch?

No, how can I do this in the GUI?

I was thinking you could add the symmetry face as a refinement region and unselect boundary layers (or set them to 1), but I don't think that will make a difference.

I have the same problem when using a cylinder. The boundary layer elements
are located correct, when the cylinder is as long (or longer) than the cube.
When the cylinder is inside the cube, the boundary elements are located wrong.
I experimented hours but cant find the reason.

Try removing and re-adding the references in the mesh region object - if the geometry changes, the numbering will change. The cylinder works OK for me. However, cfMesh will often continue boundary layers onto adjacent patches (probably depending on feature angle), so this behaviour might be unavoidable depending on geometry.

Screenshot from 2018-10-11 22-50-13.png (266.71 KiB) Viewed 2241 times

[cansf]

Hello,

I want to ask a question about pseudo-transient approach.

I'm trying to solve a nozzle analysis at supersonic conditions in a steady state approach but I don't know if I can turn pseudo-transient option off.

I couldn't turn it off in Freecad.

Best regards.