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...........

ok but if I don't include the connecting wall then the mesh of suction and pressure sides will be totally disconnected from eachother and the interface side of stationary parts will be discontinous from eachother. Can CFX handle this?

Also as per my understanding the interface should be exactly same on both the sides?

the pump has already been designed and working. Purpose is to get the simulation model of pump so that the effect of variation of different parameters on pressure delivered by the pump can be studied e.g increasing no. of pistons.

Yes. No problem

No, not necessary. Certainly, if you have a coarse mesh on either side, it will affect your solution. Therefore, you could perform some tests to check their influence.

thanks for your help. I will try this and will share the results.

One more thing. If i include the connecting wall between suction and pressure ports and just consider it as a part of interface on both sides of interface, will it gonna work?

For the interface model which model i can use? When I am using the transient-rotor stator I am getting the following error as seen in the figure attached with the post.

Attachment 66470

Any idea?

Turn on the expert parameter?

Even with frozen Rotor it's not working because I think the pistons are not getting the right motion.

For the mesh motion i have defined 5 local coordinate systems at the interface surface of each piston as seen in the figure1. I set to rotate the local coordinate frame at the same rotational speed so that I can easily define the displacement of each piston in each local coordinate system (e.g. for local coordinate system of piston1 as seen in figure 2) . But when i define the rotational speed of local coordinate system then i can't access this coordinate system under the boundary condition panel as seen in figure 3. In such a case how i can refer the local coordinate system for definition of Mesh displacement?

Attachment 66476 Attachment 66477 Attachment 66478

Just a simple question. When I load the mesh in CFX then CFX automatically places Global coordinate system centre at the centre of body as shown by the red dot in the attached figure. Attachment 66501

I am asking this because I don't know the location of Global coordinate system and I am just specifying 'Global Y' as rotation axis.

I know it is possible with immersed solids. I can share an example which is different but contains the similar settings.
I don't know with moving mesh. Maybe there is a limitation on moving mesh in combination with a rotating domain. I doubt it, but if you want to be sure I would ask the Support for an example.

I don't understand this. If I am correct, CFX creates the Global Axis on the origin (0,0,0). As a check, you can always create a monitoring point with certain coordinates to find where you are in the geometry.

I have use moving mesh and TRS to model rotary sliding valves many times and it works fine for me. But I do not use moving mesh and rotating frames of reference on the same domain. I have a domain either moving mesh or rotating frame of reference, but not both.

Yes please share the example.

If the geomtery is not centered around Global axis (0,0,0) then is there a way to move the mesh to centre in CFX or i have to go back and reorient it in meshing module?

The second option is to define the rotation axis using Two Points Option i.e. Rotation axis from and Rotation axis to...but i am not sure what is meant by this? Do you have any idea or example?

I am not sure if I place a local coordinate system on a rotating face then the local coordinate system will rotate with it not?

If domain is rotating and i also specify a rotation for local coordinate system then this coordinate system is no more available under the boundary conditions tab as shown in the picture in the above posts. I asked the support guy but he was not sure about it and he said that he will tell me later.

Certainly you can move the mesh in Pre. Go to the mesh i nhe top of your tree and use your RMB for option to translate, scale, rotate or mirror it.

Just define two points, e.g. [0,0,0] and [0,1,0] to rotate around the line through those points (the y-axis in this example). But you can use any number. CFX is flexible.......

There is also an option to create a coordinate frame based on the normal of a surface. Convenient if you don't know its, center.
Remember you can find coordinates using the creation of monitor points.

That is why I advised to create a very simple geometry and calculate the movements of all objects without calculating the flow. To first find out how everything behaves and moves like you want. Start simple..........

I had this example in mind, showing the use of multiple coordinate systems in 1 simulation. It shows the movement of rotating immersed solids in a rotating domain. There is no flow. I hope it helps.

Can't upload it somehow. You can download it here: https://we.tl/t-jk5dTykpvB

Hi,

thanks a lot for your reply. I will look at your example.

I am facing another problem. The pistons are getting the right movement but the interface side which is on the rotating domain side, is also moving. Although i have defined the 'Mesh Motion' to 'Stationary' on this side of interface but still the mesh is moving. This can be identified by the figures attached with the post.

Attachment 66590

Attachment 66591

The reason which came to my mind is that it is not a wall but a fluid interface, so the mesh nodes on interface are also moving but not exactly as the pistons. Any idea how i can keep the mesh on this interface as stationary?

I don't have a lot experience with deforming mesh.

Please post an image which shows clearly which domains are rotating and which are moving mesh, and for the moving mesh domain clearly show your different boundary patches and the moving mesh boundary conditions you applied to them.