Meshing or Topology generation error in TurboGrid?
 

I'm relatively new to TurboGrid, I've done some of the tutorials including the CFX tutorial on how to do a structural analysis by importing the pressure loads generated by a CFX simulation, and applying the loads induced by the rotational velocity of an impeller. I'm trying to do one of my own, using an impeller generated by some operating conditions and other information, using the Vista projects in BladeGen and exporting the project into TurboGrid to mesh.

My BladeGen project seems to go through without any problems and the export and opening in TurboGrid goes smoothly. I'm trying to roughly follow the same outline that the CFX tutorial lays out before venturing off on my own, so I'm not getting too create yet. So for now, I can generate the topology, correct the angles with no problems, and set a shroud tip since my impeller is unshrouded before I run into my problem. After I edit the mesh data, with a request for the inlet and oulet domains to be meshed as well (I used the same parameters for meshing these domains as the tutorial, so I could start playing with them afterwards to see how they affected the mesh, but for now they are the same), I try generating the mesh, and I get the following error:

ERROR There is no valid outlet domain to mesh. Move the outlet or the passage at the hub or shroud closer to the blade to create an outlet domain.

I've seen this error in one other post in the forums, but the response to it really just returns me to the same methods I'm using to setup my mesh initially. Does anyone have any suggestions for what may cause this and/or how I could go about fixing it? I would really appreciate any help offered. Thanks, so much!

Re: Meshing or Topology generation error in TurboG
 

hi turbogrid has given you the solution in the error message itself. In turbogrid the place from where the outlet and inlet domain starts is given by points ( A, R coordinates). If you double click inlet and outlet in your part list you could see this coordinates. Probably you ll have to change the A coordinate/s and bring it/them closer to the blade.

Best of luck

Re: Meshing or Topology generation error in TurboG
 

Thanks, I had tried that, and I figured out my problem not long after I posted this, I only moved one part of the outlet. I appreciate the help!

Dear jetcheve,
the solution of this problem is changing R-coordinates of "outlet" domain. The outline and the outlet coordinates can not be coincident.
Kind Regards
Patryk

Hey guys,

Im also new to turbo meshing.

Does anyone have a sort of model they follow in regards to meshing?

I notice that with mine the export points error comes up with a size factor of 1 but disappears when i make it 2. Im also a bit curious as to why some of the boxes in the red circle arent automatically ticked?

https://postimg.org/image/n0k43j1m9/

Brett, I would suggest you read through Chapter 10.5.1 The Mesh Data Objects - specifically about the Global Size Factor.
If your error goes away with a higher Global Size Factor, which makes your mesh finer, then I assume TurboGrid wasn't able to fit the coarser mesh properly to your geometry (or it didn't work with other constraints you put on your mesh such as boundary layer refinement).
Boundary layer refinement control is also an interesting chapter to read up on. I took me quite a while to understand TurboGrid's logic though ;)

The general meshing idea I follow is to have a rather coarse mesh and use local refinements via right-click on the purple topology lines --> "increase mesh refinement" by n%. With that method you will have a finer mesh where you need it and don't just "throw" more cells at the whole domain via the global size factor.

Regarding the checked boxes: I don't know the logic behind that but I assume TurboGrid doesn't show everything automatically because it would confuse you more rather than help you.

Thanks Maxim,

do you know where I can get ahold of that document? If you have it perhaps you could email it to me?

I was referring to the Ansys documentation which should be installed/on your hard drive already. Otherwise you'll find it on Ansys' customer portal

I managed to find a 2013 version of a document called Turbogrid Users guide where your chapter reference matches the one in the document so I'm assuming thats the right document. Where on the hard drive should it be? I cant seem to find it anywhere.....

standard installation path is
C:\Program Files\ANSYS Inc\v171\commonfiles\help\HelpViewer\ANSYSHelpView er.exe

or just access it from any Ansys window via Help - Help on Workbench for example.

A quick google search brought up this (I hope it's OK to post it here - copyright and stuff)
https://www.sharcnet.ca/Software/Ans...er/TGUser.html

Ah thanks Maxim,

That makes sense.

Regrettably I'm one of those people whereby if I cant print it off and have it in front of me the information just doesnt seem to sink in.

For anyone else out there interested you can get the latest full pdf version if you are an ansys customer this way. Log in:

http://support.ansys.com/docinfo.

Then

Online Documentation: Current Release - Documentation Downloads

Ansys turbo

I may have already asked this but has anyone ever had the error:

"There is no valid outlet domain to mesh"

I dont know why this keeps happening

This one....


https://postimg.org/image/j3fep9qo1/

Yes, I get this warning for both "inlet" and "outlet domain". In "Mesh Data" - "Mesh Size" all the way to the bottom, "Inlet Domain" and "Outlet Domain" are both unchecked after this warning. In your case only "outlet domain" is unchecked (see screenshot that you provided earlier). As far as I know, TurboGrid could create a mesh for inlet and outlet domains as well in case your model only has a rotor/stator included. If your inlet/outlet is right next to the blades, the solver will probably crash. We should always place our inlet/outlet further away from the area that we want to examine.

In my case, I have interfaces on both sides of the rotor and I model my inlet/outlet myself. Therefore it doesn't matter if TG cannot model the inlet/outlet domain because I don't need it to.

If you need TG to model/mesh your inlet/outlet domains, you should give TG enough space to do so. I assume the documentation has more information about that.

Hey Maxim,

These are my regions highlighted in green

https://postimg.org/image/hb4xqiz4x/

https://postimg.org/image/55476l9nl/

https://postimg.org/image/vvm0lcu3l/

Does that shed any light on things?

I _assume_ that TurboGrid is using that "block" at the inlet as inlet domain. At the outlet, TG did not create such a block.

Do you plan to simulate just the displayed region? Maybe you could try to create a bigger outlet and see if TurboGrid creates an outlet domain...

Ah, correct!

It seems TG is showing the inlet as that block

https://postimg.org/image/6hzcsjb35/

Whereas for the outlet it is just considering it a surface or plane in the passage

https://postimg.org/image/rvzwp31r5/

You can see from the box in the lop left.

I think this could be something that needs to be fixed back in Blade Gen perhaps?

Hey Maxim,

I followed the above advice and changed the outlet "section" by increasing the radial distance of the hub and shroud in the turbomesh outlet trim.

A new outlet block has been created and TG applied the interfaces correctly. I got no errors on inlet or outlet domain when I meshed it.

So it appears to me that there are 3 "blocks" (inlet, passage, outlet) within the one R1 domain and the interfaces between that and its circumferentially identical cousins are given on the LHS aswell. This lines up with an earlier tutorial video I can remember seeing. Hope this helps those above too.

https://postimg.org/image/okcpy3fif/

That looks good now. Thanks for the feedback :)
Now I hope you will get good results with your setup...

Much better,

I'm still having issues with the outlet pressure being negative for some reason.
This is causing havoc with my gas compressor macro.

Anyone else had negative pressures and how to fix this?

This might be worth a read:
http://www.cfd-online.com/Wiki/Ansys..._inaccurate.3F

I would suggest you search this forum about the problem of negative pressure and then open a new thread about this problem providing screenshots, out-file and a good description.
Otherwise this thread here gets too far off-topic now I think.

hi
I am facing a similar problem "There is no valid outlet domain to mesh. The outlet domain will be turned off" I was reading your solution but i am new to turbo grid can you guide me how I can orient my coordinates in order to solve this problem. hope to hear from you soon.