Learning Forum

[aqmalidlan]

Hello and good day to everybody.

I need help in pre pocessing the geometry of a lobe pump that i have drawn. I have little background in fluid flow analysis using schlumberger software but since im not in the industry anymore, I decided to forego with ANSYS. 

How do I prepare the model for meshing the domain for my CFD analysis later on? How do I know that the model I have contains no error?

[peteroznewman]

Hello,

You prepare the geometry by removing any unnecessary internal features. Read this discussion for an example, which has ICEM in the title, but shows ANSYS Meshing in the content. Depending on the software you choose: Fluent or CFX and the meshing approach taken to accommodate the motion of the mechanical parts, you create different bodies.  A common item is the use of a "Fill" command to fill the pump housing airspace with a solid body that represents the air.

You will know your geometry has no errors when you have created a successful Fill and have a valid mesh on those bodies.

Are you using the ANSYS Student 19.1 software? What CAD system was used to draw the lobe pump?

Regards,

Peter

[Rob]

You may also want to look at the various examples of overset meshing in documentation. Lobe pumps are not an easy piece of equipment to model as the impellers interlock meaning you need to use overset or deforming mesh: with a "normal" pump sliding mesh or moving reference frames are sufficient.  This will also affect how you build the geometry and create the mesh. 

[aqmalidlan]

 

 

Hello peteroznewman, I was planning to use Fluent for this. When I try to press Fill there is some error coming out saying there is an error with the geometry. I am using my lecturer's computer which I believe is not the Student Edition. I used solidworks to do the CAD from 3d laser scanning software. 

[aqmalidlan]

You may also want to look at the various examples of overset meshing in documentation. Lobe pumps are not an easy piece of equipment to model as the impellers interlock meaning you need to use overset or deforming mesh: with a "normal" pump sliding mesh or moving reference frames are sufficient.  This will also affect how you build the geometry and create the mesh. 

 

May I know which documentation I should refer to? 

[peteroznewman]

Hello aqmalidlan,

I am afraid your CAD geometry may be a facet representation and not a smooth surface, since it came from a 3D scanner.  That can make meshing difficult. A great deal of work must be done in a CAD system to convert the facet representation to smooth surfaces. That will result in clean geometry that is easy to mesh.  If you want to put all the SolidWorks files in a zip file, you can attach that zip file to your reply and I will take a look. After you hit the Add Post button, an Attach button will appear. There is a 120 MB file size limit on attachments.

SpaceClaim has some excellent software tools for cleaning up STL files, but it is an optional module, so I don't know if you have a license for that.  What version of ANSYS are you using?

Did you go to this link from my other discussion?  It describes using CFX to do an Immersed Body method which seems to simplify the meshing task.

Regards,

Peter

[aqmalidlan]

Hello Peter.

Im using ANSYS R19.0 . As for the CAD, I have tried to clean it. Attached along is the attachment of the said model and a powerpoint file highlighting my concern. 

Yes, I have seen the link and I have used this as a reference, but I have not yet started on meshing. So I cannot follow it yet unless the meshed domain is ready. 

 

[peteroznewman]

Hello,

I imported the STEP file into SpaceClaim 19.0 and went to Prepare, Extract Volume, I picked these surfaces:

and it created this fill:

You may want to delete the small holes in the side of the casing before you fill, or not depending on whether they are required.  I went to Repair and fixed the Split Edges.

In Meshing I tried Patch Independent mesh control first, but it left some holes...

Regards,

Peter

[aqmalidlan]

Hello Peter,

Thank you so much for the help, it is exactly what I wanted. Is there any difference in IGS and STEP files that I should take note of?

 

[peteroznewman]

Hello aqmalidlan,

SolidWorks is based on Parasolid, and so is DesignModeler, so there is no conversion errors between those systems. SpaceClaim is ACIS geometry kernel. STEP is better than IGS.

I have more to look at before the casing cavity will mesh.  The fill solid does not match the casing here

Please create a Parasolid file from SolidWorks of the Casing and Lobes assembly. Zip that file and attach it to your reply. I don't know if there is any conversion tolerance issue or not. I sometimes use my NX11 CAD system, which is Parasolid based, to edit geometry for meshing.

Regards,

Peter

 

[aqmalidlan]

Hello Peter. 

Noted on the difference between STEP and IGS. 

CUrrently I am trying to run some parameter in FLUENT as shown below. I will return back if I encounter another problem for now. Thank you so much for the help Mr Peter. 

Regards,

AqmalIdlan

[Rob]

If you click on the "Help" button in Fluent then work your way around the web support you'll find all sorts of useful stuff.  Looking at that mesh I'd advise doing some clean up or remeshing: it's not going to give a good result and you've got mesh clustered where you don't need it. 

[aqmalidlan]

Dear Mr Peter and Mr Rwoolhou, 

The suction for this pump im doing is sucking atmospheric air and discharging at a certain rate. For now I'm just trying to see if the flow is flowing correctly. 

Firstly, as for the suction, I noticed I could not select type of flow rate as m3/h but instead only mass flow rate (kg/s) in the inlet BC type. How do select the inlet and outlet to flow rate (m3/h) instead of mass flow rate(kg/s)? Is the direction of flowing from top to bottom is set by a constant value of 1 on the x-component? And where do I input the discharge pressure value for the

Secondly, in some specification sheet I saw, do I need to input the value for this simulation based on operating condition or designed condition?

Thirdly, I would mesh with the lobe later on since now I would want to see the flow if there is no lobe inside. And Mr Rwoolhu, which part of the mesh that you saw that needed clean up? my experience is meshing is still a novice as I cannot determine by visual inspection that my mesh needs reworks. 

Fourth, In a way, you are right Mr Rwoolhu, the meshing is terrible. how do I optimise the meshes?

Looking forward for your reply.

[peteroznewman]

Hello aqmalidlan,

I am a novice at CFD but have learned a few things that I will share and hope they are correct.

You say the pump "sucks atmospheric air", which means that the inlet should have a pressure boundary condition of 0 Pa pressure.

The outlet has a defined flow rate, which means the solver will compute the pressure required to achieve that flow rate and provide that as a result, which means you can't specify the outlet pressure.

I don't know if a volume flow rate can be specified, but if you multiply the value you want by the density, then you have the mass flow rate. Yes, you understand the x,y,z components correctly.

I believe rwoolhou was referring to the very small elements that formed along the line where the cylindrical portion of the housing transitions into the funnel to the inlet and outlet openings.  When I first attempted to mesh the casing airspace, I tried "patch independent" meshing (that failed), which means it would build elements without strictly following every surface patch. The geometry has a long thin sliver of a surface that causes lots of small elements to be created in a place where there are not expected to be large gradients in the flow field, so that is a waste of elements.

Regards,
Peter

[aqmalidlan]

Hello Peter, 

No worries as I am a novice too when it come to other than black oil model. I lack a lot of experience and knowledge in regards to pumps. 

Yes, the purpose of this pump is just to transfer air into a barrel. I have set the inlet pressure BC at 0 Pa and as calculated the mass flow rate is 0.94kg/s based on the flow rate spec of 4695m3/h. I have entered these value into inlet.

As for the outlet, I have set the same mass flow rate outlet to 0.94kg/s too. And when I try to run the simulation, I have this weird not converging graphs. I also attached the log in this reply as well for reference. 

Correct me if I'm wrong but it doesnt look right. I really appreciate your help Mr Peter. As for the meshing, I forgot how to change the shape as I think the meshing doesnt look right. 

Looking forward for your reply.

Regards,

Aqmal

[Rob]

OK, there are a few problems here. 

Please look at the help resources on the Community landing page & ANSYS Documentation re the meshing. I think Virtual Topology should resolve the issue with the small faces on the mesh.

For the boundary conditions we can't set the flow rate on the inlet and outlet at the same time. This causes problems with the numerics as you'll always see a slight difference in the solver: as Peter said set the inlet pressure as zero and if it's incompressible gas (liquid?) I'd set the outlet with a negative velocity.

Note, I can't go into much detail as ANSYS staff are limited in what we can share on a public forum. 

 

[peteroznewman]

If the flow inlet and outlet direction is generally along the Z axis, are inlet mass flows positive and outlet mass flows negative by definition?  So a -1 would be put into the Z component for an outlet even though the mass is moving in the +1 direction. I'm sure I could look for this in the help, but it's an easy question to ask, thanks rwoolhou.

[Rob]

A velocity (or mass flow) inlet will by default have an inward vector normal to the boundary, and setting a positive flow value will add mass to the domain. 

A mass flow outlet has an outward vector so a positive flow value will remove mass from the domain. 

If you want flow at an angle, then there is a component option so you can do this too. 

 

One trick with Fluent is to open the panel of interest and click on it's help button. Rather than going to the index, each panel has an entry in the User's Guide where we explain what it does and provide links to other sections as needed. 

[aqmalidlan]

What do you guys mean when you guys mentioned help resource on community landing page? So I should set the output as negative instead of positive? 

[Rob]

There are some support resources here   https://www.ansys.com/en-gb/academic/free-student-products/support-resources  plus the documentation which contains some videos as well as the theory etc. 

For your model you either need to push flow in and let it leave through a pressure boundary OR have a pressure boundary and suck it out the other end. Have a look at Chapter 6 of the Fluent User's Guide: click on "Help" in the boundary conditions panel and navigate via the menu on the left side of the pop up window/browser. 

 

[aqmalidlan]

and also how do i make the lobe as a mesh as well like the one in the tutorial? i noticed the tutorial mentioned is using cfx5 format file?

because i want to extract the volume for the space between the lobe and the casing. 

[DrAmine]

Hi,

Are you willing to use Fluent or CFX? To which tutorial are you referring? To this one: https://www.youtube.com/watch?v=yoUHuRf9h8w

In CFX there is option of modeling solid regions as immersed parts in fluid domain and this solid bodies might move rigidly.  The immersed solid should be entirely contained in the fluid domain and is not allowed to intersect any fluid boundaries. 

[aqmalidlan]

Is there a difference between CFX and Fluent for doing this?

There is a tutorial, https://fetchcfd.com/view-project/730 that i am referring to, that I want to make my model like in the tutorial. 

As per Mr Abenhadj, the analysis that I want to do is pretty much like the one in the video. Can someone help guide me as I am not familiar with Fluent.

[peteroznewman]

That tutorial is for CFX.

I did extract the volume inside the casing, without the lobes and I found a defect mentioned above. I can try the Virtual Topology method to make a better mesh.

You also must mesh each lobe individually, which is what CFX wants for the Immersed Body method. I can't recall if you provided lobe geometry.

[aqmalidlan]

Dear Peter, before this I have followed the tutorial, but yea, it was in CFX as opposed to Fluent.Can you teach me how to run the virtual topology for a better mesh? 

So extracting the volume for the lobe individually doesnt make it into meshing? 

And yes I haven't provide because I was refining it. Attached herewith is the said geometry. 

[Rob]

I'd advise building a 2d model for use with the Fluent Overset mesh as you need to comply with some fairly tight mesh constraints: the Student & Teaching licences won't allow the cell count that you'll need. 

[aqmalidlan]

2d model? 

[Rob]

2 dimensional, ie take a slice through the centre plane of the domain. 

[aqmalidlan]

My lecturer knows a friend who have access to the full license, is it possible to be done if I use their workstation to get this simulation done?

[Rob]

It should be possible, but the mesh count will be very high. We're currently working on the Overset tools to further improve them. 2d models work well, but 3d tend to need very high cell counts. For a student project I'd suggest 2d to start with and then extend to 3d once you've got the model working. 

[aqmalidlan]

I have tried following the tutorial, but somehow I wonder why the outlet velocity is lower than the inlet velocity. And I have set the direction to be blown from top to bottom, and the lobe direction. But somehow it leaks also towards the inside of the lobe. What did I do wrong here?

And shouldnt the particle be flowing around the lobe instead of inside the solid lobe? and seems there is a lot of turbulence

[DrAmine]

Check the limitations of the Immersed Solid modeling in CFX (especially regarding tracking of particles). Regarding the velocity plot you need to debug it as we do not know the settings and boundaries you applied here. 

[aqmalidlan]

how do i debug it?

[Rob]

Not sure how you've managed to do that. Please upload the project archive so someone can have a look. Note, I can't as ANSYS staff cannot work on cases in this way: it's one of several constraints we need to follow on a public forum. 

[aqmalidlan]

Not sure how you've managed to do that. Please upload the project archive so someone can have a look. Note, I can't as ANSYS staff cannot work on cases in this way: it's one of several constraints we need to follow on a public forum. 

 

How do i save the project archive? I see, is there anybody that can help me with this, as I have to understood it would against the rules. 

[Rob]

In Workbench, under the File menu there is an option for Save Archive. If you can attach that or the RES file (CFX) here then someone in the community may be able to help: as mentioned ANSYS staff cannot open the files. 

[peteroznewman]

Details on saving an archive.

[aqmalidlan]

I couldnt get it to compress to 120mb because it a 2gb files. Btw, attached is the google drive link to it. 

https://drive.google.com/open?id=1lJIDevwarMiy7DEL0rxa90ZDUikm0fM_

[aqmalidlan]

 Hello and Good Morning All,

From this simulation I wanted to know the volume of air that the blower is pushing. So after doing the solution in CFX Pre, I entered the expression = volumeAve(Velocity)@Inlet or Outlet, but it is spitting out the ERROR The following unrecognised name was referenced: velocity (on 'Inlet').

What did I do wrong here? I wanted to know the volume of the air at both inlet and outlet in m3/h, how do I do that? I have set the Inlet to be Boundary Details of a mass flow rate (kg/s) instead of volume (m3/h). My Outlet to be Boundary Details is average static pressure of 1 atm.

How do I fix everything in this simulation to show volume of air in m3/h instead of kg/s?