'Gill Static Pressure Inlet' simulation project by burble


I created a new simulation project called 'Gill Static Pressure Inlet':

This inlets correct static pressure errors in barometric measurements.

More of my public projects can be found here.


@burble - interesting model. What type of analysis are you looking to run?



I am hoping to verify proper deceleration of the airflow between the disks. The purpose of the Gill inlet is to reduce barometric pressure measurement errors due to air velocity. My application is MAVs, where the altimeter is barometric. Due to aerodynamic effects, there can be significant altitude errors and consequently, undesirable flight characteristics.

Since we are on the subject, you might be able to point me in the right direction. My simulation efforts stalled when I was unable to select the mesh that I generated with SimScale to use for analysis. Any idea why this would happen?

Thanks and best regards,

Chris Hardwick


Hi Chris @burble,

sounds interesting. So am I right that the air is entering through the big hole and then leaving the device in radial direction? Could you maybe provide a quick drawing of where is fluid coming in and where it is leaving again? That way I probably also could provide a better hint for meshing.

Regarding your current simulation setup: You have not generated a mesh yet, you only created the mesh setup. So there is no valid mesh you can assign to your simulation yet.

You generate a mesh by defining a mesh operation that shall be used to generate it (see screenshot). I’m happy to suggest a mesh operation as soon as I know where things are flowing :smile:!





Thanks for the mesh explanation. As I’m a simulation noob, I could use some coaching in the process.

The quick explanation of the Gill inlet function in this application is that the device is positioned horizontally in some free-stream flow. Air enters between the plates, around the perimeter. The device is circular, so that airflow in any direction in the horizontal plane can be accommodated. The barometric pressure is then sampled through a small hole in the center. In situ, this device would be mounted on the top of a tube that places it outside of the aircraft’s pressure gradient. The purpose is to compensate for altitude errors caused by that pressure gradient. A conventional, forward-flying aircraft uses a pitot tube for this purpose. However, a multirotor aircraft can move in any axis.




Chris @burble,

ah - thanks for the explanation, I think I understood it now better. One thing that’s still not clear to me is where exactly you’ll sample the pressure? That would be good to know for a proper boundary condition assignment.

However based on that info the meshing and simulation process got clearer. There are different options how you can create a proper mesh for that simulation. The best way would be if you’d have a CAD model of the actual air domain, so basically the negative of the device. That way mesh setup would be straightforward. But one can also set up a mesh with the positive model with certain limitations. Let me quickly set up a demo.


Chris @burble,

ran a quick test analysis of your model. The mesh is too coarse to capture the flow in the small channel accurately but it serves as a proof of concept: The fluid is assumed to be incompressible, flowing with 1 m/s from the left. The bottom of the vertical “channel” or “pipe” is closed - is this correct or can air flow through there?

What I was wondering:

  • What’s the dimension of the device? In my sim it’s not roughly 6cm big? Is that dimension correct?
  • What flow speed are you expecting? Everything below Mach Number of ~0.3 can be assumed incompressible?

You can find the project here: https://www.simscale.com/projects/dheiny/gill_static_pressure_inlet



Fascinating! Thank you for the sim!

The pressure analysis looks spot on. The pressure should be neutral at the center inlet port. You are correct in that the tube is essentially plugged.

I don’t understand the U analyses. Are these a velocity gradient?

The target is neutral pressure at the inlet up to around 20m/s.

The inlet diameter is 40mm at present. None of the dims are fixed. This design can be modified to achieve the desired result.

I need to learn how you set up and ran the sim.

Thanks again!


Hmm, a negative model. I’ll see what I can produce.



the U color plot shows the magnitude of the velocity vector. I simulated the device in an airflow of 1 m/s from the left. The blue region on the right shows the vortex/turbulent wake behind the device.

Regarding the negative model: Actually it worked well also with the positive model, so you can stay with that one. One question though: Does the air flow until level A or B of the device (see sketch):

The reason I ask is that the way I ran the simulation, the distance between the device and the lower wall of the mesh is very short (see sketch below). In the real world there would be air, right?

So it might make sense if you upload both the device + the long pipe/beam it is attached to. That way the lower wall of the mesh could be set farer away from the device.




Ah, I see. Yes, the device would normally be mounted on a hollow mast. Everything above the flange below B would be in freestream air. That might have an impact on velocities near the ‘front’ of the disk. For reference, the air pressure would be sampled at the end of a tube that would be connected to the bottom of the mast.

I’ll upload an assembly model that includes the mast.



@burble - if the pressure is sampled at the bottom of that tube, then I think it might be even more important to have the attached mast in the simulation as well. From a meshing workflow perspective, that will not make anything more complex but it will give more accurate results.



Thanks much for your work on this sim. I really appreciate your time to help me get started. I’m hoping that I can ask for a bit more guidance. I have been trying to get a useful sim, partly using your copy of my project as an example, and partly trial and error. I think I’m close, but still missing something. My sim doesn’t seem to contain any pressure or velocity data; or I don’t know how to view it.

Would you be willing to take a look? https://www.simscale.com/workbench?publiclink=24ef29bc-4da3-4d73-b456-02f17bb55757

Best regards,



@burble - sure, I’ll take a more detailed look later today! On the first glance, you did not only upload a model of the air domain around the device but also the device itself, which is typically only necessary if you want to simulate both (e.g. heat transfer through both domains). So the air CAD model would be enough. But I’ll take a closer look later.



so now I had a closer look at your project. Great work in the simulation setup - I didn’t find any issues/mistakes there so that one should be good to go! The reason why you’re getting wrong/strange result is the generated mesh or more precisely the combination of your CAD model and your choice of mesh generation approach. But it’ll be easy to fix, so let’s have a closer look:

The CAD model you uploaded was an assembly made up of 4 parts. The first part is a simple box/enclosure (note that this is a full volume body).

And placed within this box, intersecting with the box, the 3 parts of the actual assembly:

You now meshed these 4 parts with the auto-mesher, that will generate a volume mesh for each of these parts. But this means that we’ll end up with overlapping/intersecting meshes since the parts in this assembly are already intersecting and the volume mesher will not change anything. So with your simulation setup you then assigned a material to the box part but this part does not know anything of the 3 other parts which is why you get unexpected results.

What we actually want are the pressure and velocity values around the 3 parts of the device, right? That’s the tricky part about CAD preparation for flow simulation, that most of the time you’re not modeling/designing the flow domain but the part that implicitly defines the flow domain. That’s the part where you need to get you’re head around in the beginning, but once that got clear, the mesh-gen and sim-setup will become much easier, promised ;)!

So there are now two different options how to get a valid mesh of the flow domain around the object:

1. Upload a CAD model of the actual flow domain: In your case that’s pretty simple: As you already put a box around the device, you simply need to subtract the device from the box and there you go: A CAD model of the flow domain, that you now can start meshing.

Please note the difference: You uploaded a model where the device was intersecting with the box (so they occupied the same space):

I subtracted the 3 parts from the enclosure box:

The advantage of this approach is that you can model your flow domain arbitrarily complex. So say you’d like not to put the device into a box-like enclosure but a sphere-like one, you could simply do that. The disadvantage is that it requires a bit more CAD work.

2. Upload only the positive CAD model and use external-flow mesh operation: In the second approach you do upload the positive of the CAD model and use the Automatic snappyHexMesh for external flow mesh operation.

This operation first puts a Cartesian box around your object and then meshes everything around your object. So it basically does the boolean operation of cutting the object from the box for you.

Disadvantage of this method is that it only works for Cartesian/box-like enclosures of objects which is the case in your application.

I’m running 2 quick mesh tests over in my copy of the project: https://www.simscale.com/projects/burble/gill_static_pressure_inlet

Hope I could help.

BTW: Are you planning on manufacturing the device at some point?




Quick additional note: It’s actually quite an interesting application for meshing as it has this very small channel in the middle of the device. Here it’s crucial that the mesh has enough cells, otherwise this very small channel will be artificially blocked. Check out the first mesh that was generated (finer meshes already running):

Here the small channel in the very middle has only 2 cells across the diameter. If you’d now assign a no-slip wall to the walls here, this would mean there wouldn’t be any cells where the flow could go through. So I just kicked of a finer mesh, let’s see how that looks.



Thank you very much for the detailed walk-through. You’ve clarified few things for me.

I thought that I had created a solid model, enclosed by a surface model. Now that you’ve shown me the preferred method, I’ll go that way.





glad I could help. One question regarding the device itself: What’s the reason that the channel is so small + long? I did understand correctly that the pressure is probed at the bottom of the long channel, right? So is there a specific reason for this (from a CFD perspective) “extreme” dimensions?



There isn’t a scientific reason for the tiny hole. It was an assumption on my part that the hole should be small, not knowing that it could present a challenge in simulation. If the disks do their job, and pressure is neutral at that orifice, then the hole could be larger. However, a transient sim might be in order, to verify that rapid air velocity changes don’t impart the pressure reading with a larger hole.

In answer to a question that I missed earlier, I don’t know if volume manufacturing is my path for this part. I might 3D print a few for my own use. I might make the CAD available to the open-source UAV community that I’ve been working with. Several of us have been working independently on resolving an aerodynamic problem with the barometric altimeter that we use in our drones.





It looks like my trial and error approach to learning how to perform a fluid analysis on my part has resulted in exceeding my computational quota.

I thank you very much for your help on this project. I think the service that SimScale provides is a fantastic idea and fills a big niche. Your individual assistance has been outstanding.

There have been many designs over the last several years wherein I would have benefited a great deal from ability to simulate, but the tools are far out of reach. Your service brings the tools within reach for a great many people; hacks like myself, and real engineers alike.