Hello,
My aim is to calculate the drag coefficient (cd) for the G7 projectile at Mach 3. A drag table for this projectile can be found on this website: https://www.alternatewars.com/BBOW/Ball ... Tables.htm. Scroll a bit down.
1. Replicate the G7 with the image found on Wikipedia (https://en.wikipedia.org/wiki/Ballistic_coefficient)in the Part Design WB.
1 caliber = 10 mm
2. Add a box for the boundaries in the Part WB which surrounds the projectile. Use XOR to "fuze" the two bodies.
L = 250 mm; W = 100 mm; H = 100 mm
3. Add an analysis container in the CfdOf WB.
4. Create a mesh.
5. Add a mesh refinement.
6. Define the inlet.
Mach 3 = 1029 m/s
7. Define the outlet.
8. Define the walls.
9. Define the physics model.
10. Define the fluid - air, of course.
11. Initialise flow field.
In the end it looks like this:
12. Hit it!
My questions so far:
Is my boundary box sufficiently big enough?
Which mesh is best used for this application?
Are my settings correct to get an accurat result?
13. I used this tutorial (How to calculate aerodynamic forces with Paraview https://www.youtube.com/watch?v=J944HOj_4b0) to calculate the drag force.
14. With the force acting on the projectile it's trivial to calculate the cd (https://en.wikipedia.org/wiki/Drag_coefficient).
The problem is that this cd is wayyy too high. According to the table the cd at Mach 3 should be 0,2424.
The Freecad file with my work so far is attached.
Any constructive input would be much appreciated. Thanks!
G7 projectile at Mach 3
Moderator: oliveroxtoby
Forum rules
and Helpful information for the FEM forum
and Helpful information for the FEM forum
G7 projectile at Mach 3
- Attachments
-
- G7_2.FCStd
- (29.63 KiB) Downloaded 75 times
Last edited by S.L.App on Sun Jun 28, 2020 3:08 pm, edited 6 times in total.
Re: G7 projectile at Mach 3
Hi and welcome to the forum!
The images are not visible. Please attach them directly to the post.
The images are not visible. Please attach them directly to the post.
A Sketcher Lecture with in-depth information is available in English, auf Deutsch, en français, en español.
Re: G7 projectile at Mach 3
I forgot the images file extensions. They should work now. Thanks chrisb.
-
- Veteran
- Posts: 3158
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: G7 projectile at Mach 3
In 3D I have problems to attach boundary-layers at the projectile.
So I ran a 2D-case to get an impression. Inlet-speed 1000 m/s.
The computing domain is too small.
So I ran a 2D-case to get an impression. Inlet-speed 1000 m/s.
The computing domain is too small.
-
- Veteran
- Posts: 3158
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: G7 projectile at Mach 3
Approach with GMSH, using 1/4 model.
GMSH gives a smooth mesh, but I get 2,9 mio cells.
One iteration of Hisa needs 90 sec on my laptop with i5/16 GB. No chance...
GMSH gives a smooth mesh, but I get 2,9 mio cells.
One iteration of Hisa needs 90 sec on my laptop with i5/16 GB. No chance...
-
- Veteran
- Posts: 3158
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: G7 projectile at Mach 3
Approach with snappyHexMesh, relativly coarse mesh, 1/4-model, result:
drag-coeff cd=0,22. However, high-speed-aerodynamics is not my playground...
At S.L.App:
Check p-case-file before computing forces with paraview.
With Hisa you get the "real" pressure (not a "normalized" pressure p/rho when using simplefoam).
Do not multiply the integrated pressure field in paraview with the fluid density as described in the YT-tutorial you posted.
This would give too high drag.
Regards Thomas
drag-coeff cd=0,22. However, high-speed-aerodynamics is not my playground...
At S.L.App:
Check p-case-file before computing forces with paraview.
With Hisa you get the "real" pressure (not a "normalized" pressure p/rho when using simplefoam).
Do not multiply the integrated pressure field in paraview with the fluid density as described in the YT-tutorial you posted.
This would give too high drag.
Regards Thomas
Re: G7 projectile at Mach 3
Hello Thomas,
thank you for your time. What do you mean by "Check p-case-file before computing forces with paraview." In which file can I find the pressure?
thank you for your time. What do you mean by "Check p-case-file before computing forces with paraview." In which file can I find the pressure?
-
- Veteran
- Posts: 3158
- Joined: Sat May 20, 2017 12:06 pm
- Location: Germany
Re: G7 projectile at Mach 3
After case-writing, open p file in case/0 directory.
The [...,...,...] defines the unit e. g. pressure. Write a simplefoam case and compare. They are different.
==> compressible vs incompressible ( no rho).
Re: G7 projectile at Mach 3
Now I understand, thanks.
In this case:
m/(kg * s²)
Minus means the dimension is under the fraction line. The number is the exponent.
--------------------------------------------------------------------------------------------------------------------------------------
The biggest error seems to result from the fact that I used "walls" instead of "open - far field"
That's close enough, I guess.
I'm going to try a couple of more velocities. I wonder how it behaves in the transonic area with the "Laminar" setting.
In this case:
Code: Select all
dimensions [1 -1 -2 0 0 0 0];
Minus means the dimension is under the fraction line. The number is the exponent.
--------------------------------------------------------------------------------------------------------------------------------------
The biggest error seems to result from the fact that I used "walls" instead of "open - far field"
That's close enough, I guess.
I'm going to try a couple of more velocities. I wonder how it behaves in the transonic area with the "Laminar" setting.
- Attachments
-
- G7_3.FCStd
- (29.67 KiB) Downloaded 75 times