Supersonic CFD with FreeCAD!

[Buckeye]

The CfdOF workbench in FreeCAD includes the density-based compressible solver, HiSA, developed for transonic and supersonic flows. I am not experienced in compressible flow CFD, so I am learning as I go. The documentation discusses two validation test cases, the Army-Navy Basic Finner (ANF) and the Air Force Modified Finner (AFF). I built the ANF using the Rocket Workbench. The domain boundaries were prescribed as far-field with freestream conditions at 50 calibers away from the rocket body. I simulated a steady-state Mach 1.5 in this first go around. For y+=1 across the range of speeds I plan on testing, the first layer was 500 nm. Wow!



The initial mesh was about 1.7M cells. The meshing options include a shockwave adaptive refinement during the solve, which is way cool! After solution refinement, mesh size increased to 2.4M cells.



The solution is well-converged after 800 iterations or so. Wall time was about 8 hours on 4 cores. CD = 0.68, which is right in line with the wind tunnel and free flight data. Nice! I will do a complete speed sweep.



The compressible solver was no more difficult to set up in FreeCAD and seems just as robust as the incompressible. This really opens up CFD as an accurate hobby tool for drag, lift, center of pressure, etc. across all regimes of model rocketry. Really awesome freeware!

 

[2-0turbo]

That is really amazing! I plan on following your work to see how this progresses. I don't have the time to invest right now in this, so I hope to learn from what you're doing. Is the model you ran essentially in coast right now? Or is the motor burning? It appears that base drag is present and large, indicating that perhaps this is just after motor burnout. Thanks.

 

[dvdsnyd]

@Buckeye,
Really cool stuff!
I've been really following FreeCAD as of late. I REALLY want to make the plunge. I've tried a few other times. It's JUST SO CLUNKY, when compared to SolidWorks, which I use at work, and Fusion360, which I've used for close to 6-8 years now.
This work and your other CFD thread makes it more enticing, that's for sure.
Are you using FreeCAD to model parts as well?

Did I understand you right, it took your computer 8 hours to plug through the algorithm and solver?

Dave

 

[Buckeye]

That is really amazing! I plan on following your work to see how this progresses. I don't have the time to invest right now in this, so I hope to learn from what you're doing. Is the model you ran essentially in coast right now? Or is the motor burning? It appears that base drag is present and large, indicating that perhaps this is just after motor burnout. Thanks.

Yes, coasting. Motor and its burn is not simulated here.

 

[Buckeye]

@Buckeye,
Really cool stuff!
I've been really following FreeCAD as of late. I REALLY want to make the plunge. I've tried a few other times. It's JUST SO CLUNKY, when compared to SolidWorks, which I use at work, and Fusion360, which I've used for close to 6-8 years now.
This work and your other CFD thread makes it more enticing, that's for sure.
Are you using FreeCAD to model parts as well?

Did I understand you right, it took your computer 8 hours to plug through the algorithm and solver?

Dave

Yeah, I don't care for the CAD part of FreeCAD either, but the seamless integration of the CFD workbench (and other workbenches) makes it worthwhile.

I am building all the 3/4 FNC rockets for CFD testing using the parametric "Rocket" workbench. It is awesome for building nosecones and fincans. You can import other CAD models and meshes into FreeCAD if you prefer to design in another software.

Yes, 8 hours to solve on my home computer, which is a function of the mesh size and desired convergence. I am zeroing in on a good balance for me. The compressible algorithm is also solving for T and rho, which you don't worry about in isothermal incompressible simulation, so it takes longer.

 

[GlenP]

Very cool, nice job! Can you make another similar Mach contour plot at an offset Y<>0 XZ-plane roughly in the mid span station of a fin? Just curious.

 

[Buckeye]

Very cool, nice job! Can you make another similar Mach contour plot at an offset Y<>0 XZ-plane roughly in the mid span station of a fin? Just curious.

Here is a y-slice through the midspan of the fin nearest you. Does it look reasonable?

 

[GlenP]

Here is a y-slice through the midspan of the fin nearest you. Does it look reasonable?

View attachment 637582

Reasonable? It looks awesome!

There are some textbook oblique shock equations for 2D flow that you can use for comparison, just for fun, as well as 3D conical theoretical solutions, without friction, but would give a pretty good estimate of the shock wave angle and Mach number change across the shocks at the nose and over the fins.

 

[kjhambrick]

Here is a y-slice through the midspan of the fin nearest you. Does it look reasonable?

<<snip>>

Holy cow, yes !

My calibrated eyeball says that is definitely a 41.8 degree Mach cone

Great work !

Thanks for the inspiration, @Buckeye !

-- kjh

 

[GlenP]

You can also look at the mesh in that offset plane to see the solution adaptive refinement at work along the fin shockwaves.

You could maybe try out different supersonic airfoils for your fins, like wedge, diamond, bi-wedge/flat (Nike Smoke type), if you are curious, you may already be planning trade studies like this of your own after these standard validation test models.

Wedge is typically most stable, but also higher drag, so a drag comparison of wedge and diamond of the same thickness might be interesting.

Thank you for expanding and sharing the body of knowledge!

 

[aerostadt]

Technically, shock waves do not go all the way through the boundary layer, because somewhere in the boundary layer the flow goes subsonic. I don't know if the fidelity of the current analysis is that comprehensive. Years ago in my aerospace life, I ran Fluent in a very zoomed-in CFD model of a carbon phenolic nozzle and sure enough the CFD model showed the shock waves coming down to the top of the BL.

 

[Buckeye]

You can also look at the mesh in that offset plane to see the solution adaptive refinement at work along the fin shockwaves.

You could maybe try out different supersonic airfoils for your fins, like wedge, diamond, bi-wedge/flat (Nike Smoke type), if you are curious, you may already be planning trade studies like this of your own after these standard validation test models.

Wedge is typically most stable, but also higher drag, so a drag comparison of wedge and diamond of the same thickness might be interesting.

Thank you for expanding and sharing the body of knowledge!

Sounds like you have experience in this field. CFD or other analysis methods?

Yeah, I will probably next work on the Air Force Finner model, which is a double wedge and also ogive nosecone.

I don't have any trade-off studies at the moment. I just enjoy building and analyzing CFD models, demonstrating the capability, and comparing results with the prior art. I think CFD is now a feasible tool for the model rocket simulation toolbox for those looking to go to the next level.

 

[GlenP]

Not so much recently, but I studied similar such methods in school some years ago.

 

[Buckeye]

Here is a speed sweep of drag coefficient with my model (blue x's) plotted over published data of the ANF. The free flight and wind tunnel experiments from DRDC are plotted in circles. CFD analysis from other authors are shown in triangles.

The FreeCAD CfdOF results agree nicely except for the first point at M = 0.5. Not sure what is going on here. Maybe this case is pushing the compressible limit of the HiSA solver. Still, damn good for a CFD model that would be considered pretty coarse at just 2M cells. I would be confident in building a CD vs. Mach curve in CFD for trajectory analysis.



I built the ANF model in RASAero and plotted its drag vs. the CFD model.

 

[Buckeye]

Velocity slices:



Mach 1 isosurfaces: