Simulation of Radial piston pump
 

Hello everyone,

I want to model the radial piston pump of rotating cylinder type in CFX as shown in the attached image. The cylinders are enclosed inside the rotating Rotor which rotates inside an eccentric ring. Due to the eccentric motion of rotor the cylinders volume gets increased or decreased depending upon the position of cylinder w.r.t eccentric ring. This cannot be modelled with rotating domain as the motion is not circular. How I can model the rotation of cylinders keeping into account their increasing/decreasing volume?

Thanks

Sorry I forgot to attach the image. The figure is attached with this post. Attachment 66281

immersed solids for the pistons, moving on a nicely fitted hex mesh inside the channels that get filled and emptied all the time.

It looks like this could be modelled with moving mesh. That includes the rotation and the piston motion.

Thanks for your reply.

I have till yet no experience with immersed solids but i will read about it. Can you briefly explain here what is the advantage of using immersed solid over moving mesh technique?

The clearance between Rotor( in which pistons are moving) and inlet&outlet ports is just 10 microns :(. I am not sure if CFX will be able to handle it even if i get to resolve this small region with very fine mesh?

If i choose to leave this small clearance then there will be a problem of defining the interface between moving and non-moving parts. Any suggestions?

With moving/deforming mesh, I would suggest to leave out the gap. And there won't be an interface.

The top wall will move in and out, depending on its angular position. The side walls will adapt.

In the experience I have with moving/deforming mesh, make sure the timesteps are not too large. Otherwise, the deforming mesh can't keep up the modifications, leading to bad meshes. Perform several tests first.

With immersed solids, you are just blocking off fluid elements with a secondary solid. This solid will move over the fluids elements following your prescribed motion and position.

If you have a tet mesh for fluid and a cylindrical piston blocking several tets half, you can imagine that your flow solution won't be very good. Therefore my advice is to a create hexahedral mesh for the fluid that aligns nicely with the piston. Then still, the boundary layers might not be resolved very well using immersed solids. Not as well compared to moving mesh.

In principle you can make the piston a bit smaller than the fluid channel, leaving open the small gap of 10 mu. But you need a very fine mesh if you want to resolve the flow in the gap accurate.

Bottomline, the best approach depends on which question your are trying to answer using CFD............

I didn't understand how there will be no interface for the moving mesh case? The pistons volume is getting bigger or smaller as they are rotating inside the eccentric ring, so the moving mesh will be used for the pistons as their volumes are getting bigger or smaller.

For the rotation of pistons won't i need an interface to sepratae the rotating (rotor with pistons enclosed in it) and non-rotating (shaft on which inlet and outlet ports are located) parts?

Yes you need an interface. I think the right location will be as indicated by the green circle, see my attachement.

(I thought you wanted an interface around your pistons. But neither with moving mesh nor immersed solids, you need one there. Only at the green circle.)

[QUOTE=Gert-Jan;712419]Yes you need an interface. I think the right location will be as indicated by the green circle, see my attachement.
QUOTE]

Actually the figure i attached with the post is oversized. See the actual flow model of the pump without the clearance volume between shaft and rotor.

Attachment 66315

Now if i don't consider the clearance volume, then I have the problem of defining the interface but if i consider the clearance volume then it is too small (10 microns) to be meshed. Even if i manage to mesh it i don't know if CFX will be able to handle it because of very high velocities in that region. Any further suggestions?

you can let the interface coincide with the outer wall of the chamber. It should necessarily be in the middle of the gap

sorry i didn't understand fully. How i can allow the interface to coincide with the outer wall of chamber? Inbetween the suction and delivery chambers there is a separating wall where there will be no flow if i don't consider the 10 microns gap. See the attached image where different regions are marked.

Attachment 66316

Put the interface on the circular outerwall of the pressure/suction chamber and gap. Over 360°. As a result, on the inner sideof the interface there will be fluid everywhere. On the outside of the interface, there will be alternating channels (with the piston) and wall. That's OK. CFX will find out when there is a wall, and when there is a fluid. If there is a wall, CFX will close the interface and make it wall.

thanks for your help. I cannot understand how there there will be fluid everywhere on inner side of interface? As this interface also includes the zero thickness wall which separates pressure and suction chambers (dark blue walls, also labelled in the figure attached in the above post).

This interface will be Fluid-Fluid interface?

I thought the zero thickness wall was the gap of 10 mu.
If it is a gap of 10 mu, then you have 360° liquid around. If it is a wall of zero thickness (=shell), then you cannot not include this part since CFX can't handle shell elements.

Then, for the rotating part, 2 separate surfaces (segments over ±160°) remain for the interface.

[QUOTE=Gert-Jan;712458]I thought the zero thickness wall was the gap of 10 mu.QUOTE]

No between pistons and suction port/pressure port/wall separating suction and pressure ports is a small gap of 10 mu (all around 360°) which is not included in the flow model attached in the above posts. If i include this 10 mu gap then i don't see any problem in defining the interface between rotating and non-rotating ports and separating wall.

If i leave this gap of 10 mu, can i still define the interface as the separating wall will then become part of interface? Is it somehow possible?

Your separating wall and pressure and suction chambers are fixed, in the stationary frame. The separating wall will be (almost) perpendicular to your interface. So, it won't be part of the interface.
It will be a quite complex model. I think it is wise to first create a very simple model with coarse grid. Then set it up in Pre, including all moving and stationary parts and let it run without solving the flow. Just let it rotate and see if everything behaves normal and moves in the right direction. Then turn on the flow and see if it behaves normal. Then create a better grid and solve again.

Bottomline: increase complexity step-by-step.

I am attaching the figure of new model with 10 mu gap so that you can understand what exactly I mean. If i model this extra 10 mu domain then i can define interface.

But if i leave this out then the surface connecting suction and pressure ports become zero thickness wall. My concern is, how can wall be part of Fluid-Fluid interface?

Attachment 66363

Attachment 66364

Easy to say, in the current configuration pink piston is in contact with 10 mu fluid domain but when i leave this 10 mu fluid domain then pink piston will be in contact with a wall.

As I already mentioned, you can close the gap. Then there will be a wall with zero thickness. Do not include this wall in any way in your CFD-calculation. It should be completely absent.

Then, the interfaces of your stationary domain will be the 2 round wall (±160°) of the pressure and suction chamber. The interface of the rotating domain will contain the 5 round openings to the channels where your pistons move up and down. CFX will notice by it self if these interfaces overlap or not during the rotation. If they overlap, then liquid can pass. If they don't overlap, the interface will be a wall.

Needles to say, that if the goal of your CFD-study is to the determine the flow through the gap, then you should not apply this simplification. But that depends on the question that you are trying to answer using CFD...........