CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   Pointwise & Gridgen (http://www.cfd-online.com/Forums/pointwise/)
-   -   Pointwise to Fluent problem (http://www.cfd-online.com/Forums/pointwise/95388-pointwise-fluent-problem.html)

scottmichaels December 15, 2011 08:59

Pointwise to Fluent problem
 
Hi all,
I'm using Pointwise 16.4 to mesh a simple 2D half cylinder in a structured rectangular grid. After completing the mesh, setting the boundaries and volume conditions, i export as a CAS file, but when I try to read this in Fluent I always get an error saying "Build Grid: Aborted due to critical error". I believe this is happening because in my volume conditions I'm defining my single fluid as 3 domains, which should be in a 2D block, but I can't find an option to create a 2D block! A really simple issue but I'm tearing my hair out so if someone can point me in the right direction it would be greatly appreciated!
Scott

cnsidero December 15, 2011 11:44

Quote:

Originally Posted by scottmichaels (Post 335937)
Hi all,
I'm using Pointwise 16.4 to mesh a simple 2D half cylinder in a structured rectangular grid. After completing the mesh, setting the boundaries and volume conditions, i export as a CAS file, but when I try to read this in Fluent I always get an error saying "Build Grid: Aborted due to critical error". I believe this is happening because in my volume conditions I'm defining my single fluid as 3 domains, which should be in a 2D block, but I can't find an option to create a 2D block! A really simple issue but I'm tearing my hair out so if someone can point me in the right direction it would be greatly appreciated!
Scott

Scott,

First make sure you have set the dimension type in Pointwise to 2D (CAE > Set Dimension > 2D). Next, I believe 2D meshes need to be in the XY plane, so make sure your domains are in the XY plane. Last, to ensure the cell orientations are correct, the domain normals need to be pointing in the +Z direction. To check/modify the orientation, select all of your domains and go to Edit > Orient. If some are pointing in the -Z, select only those and reverse their orientation. If you have structured domains, you will want the k coordinate pointing in the +Z direction.

The last step is usually the cause of 2D meshes not working in Fluent.

Let me know if that helps, Chris

scottmichaels December 15, 2011 14:10

Thanks Chris!
I know for certain that your first two points are not my problem, however I'm having trouble checking the 3rd. When I select one of my domains and click edit > orient, firstly there appears to be no mention of whether it is pointed in the Z/-Z direction, and secondly the white domain overlaps the i/j/k labels so I can't see them!
Thanks for your help
Scott

cnsidero December 15, 2011 15:21

1 Attachment(s)
Quote:

Originally Posted by scottmichaels (Post 335979)
Thanks Chris!
I know for certain that your first two points are not my problem, however I'm having trouble checking the 3rd. When I select one of my domains and click edit > orient, firstly there appears to be no mention of whether it is pointed in the Z/-Z direction, and secondly the white domain overlaps the i/j/k labels so I can't see them!
Thanks for your help
Scott

Scott,

OK, it sounds like you have all structured domains. If so, you're right - you can't see any normal arrows. In a 2D structured domain it will only show the I and J topological directions - the K is implied and determined by I and J.

Refer to the attached image for the followin explaination.

I have two domains selected in Edit > Orient. The top one has the correct orientation such the (implied) K direction is pointing out of the screen. I determine this by applying the right-hand rule with the red (I direction) and yellow (J direction) arrows. You can see they begin in the top right corner; therefore using the right-hand rule, +K will be out of the screen.

The bottom one has the incorrect orientation. The I and J directions begin in the bottom right corner but using the right-hand rule the +K direction would be into the screen. So there's two ways it can be corrected. Either reverse the I direction or reverse the J direction. Then the orientation of +K will out of the screen.

An easy way to ensure they're all correctly oriented is to pick (or modify) the orientation of one domain so it's correct, set it as the master (Set Master), select all of the domains and click Align to align them to the one you set as the master.

A little confusing at the beginning but once you get the hang of it, it's no longer an issue.

cnsidero December 15, 2011 15:56

Quote:

Originally Posted by scottmichaels (Post 335979)
secondly the white domain overlaps the i/j/k labels so I can't see them

My tip here is while in Edit > Orient, you can select/deselect as needed to make it clearer to work on them.

scottmichaels December 15, 2011 16:47

Hi Chris,
Thanks so much for your help, one of my domains was indeed oriented wrong and fixing it has solved my issues! And your instructions were very clear btw ;)
Scott

cnsidero December 15, 2011 17:31

No problem. Good to hear that fixed your problem.

daenerys December 19, 2014 10:58

4 Attachment(s)
Hi, bringing back forgotten memories...

I have the same problem. I'm using Pointwise to mesh a certain Geometry (attached), I chose Ansys Fluent as the solver, and exported it as CAE. Then, when I try to open the file in Fluent, I get the attached Error message.

I tried the tips in this thread and changed the orientation of the different domains. Like Scott, I couldn't quite see the i, j, k labels due to the white domain so I changed the orientation twice randomly and saved it. Then, as I opened it in Fluent, I received two different domains, but never the complete mesh file!

What can I do?

cnsidero December 19, 2014 11:06

Quote:

Originally Posted by daenerys (Post 524688)
Hi, bringing back forgotten memories...

I have the same problem. I'm using Pointwise to mesh a certain Geometry (attached), I chose Ansys Fluent as the solver, and exported it as CAE. Then, when I try to open the file in Fluent, I get the attached Error message.

I tried the tips in this thread and changed the orientation of the different domains. Like Scott, I couldn't quite see the i, j, k labels due to the white domain so I changed the orientation twice randomly and saved it. Then, as I opened it in Fluent, I received two different domains, but never the complete mesh file!

What can I do?

First, you'll definitely need to get the orientation correct. Randomly swapping them is ... well ... random. Read my second, longer reply in this thread to be able to get it right. You can see the red and yellow arrows at the edge of the white domain. They are indicating the topological I, J directions.

Second, "I think" you need to assign the domains to a single volume condition (in Pointwise) otherwise Fluent will treat them as separate cell zones. Go to CAE, Set Volume Conditions, create a new VC and add all the domains to it.

-Chris

daenerys December 19, 2014 12:04

4 Attachment(s)
I read your reply, I'm just not quite sure what I'm seeing in your picture, and the explanation didn't help. I'm attaching photos of the domains, can you tell me whether I need to reverse anything?

As for the VC, it is relevant for 2D geometries as well? If so, is it correct, the way I did it?

Cheers.

cnsidero December 19, 2014 12:43

Quote:

Originally Posted by daenerys (Post 524699)
I read your reply, I'm just not quite sure what I'm seeing in your picture, and the explanation didn't help. I'm attaching photos of the domains, can you tell me whether I need to reverse anything?

As for the VC, it is relevant for 2D geometries as well? If so, is it correct, the way I did it?

Cheers.

Your pictures are a little smaller so its tougher to tell but here's the steps:

- Select all three domains, go to Edit>Orient
- While in Edit>Orient, deselect them all except the largest one
- change the orientation such the red arrow head is pointed in the same direction as the X axis and change the yellow head is pointed in the same direction as the Y axis (using some combination of Swap and/or Reverse)
- Click Set Master
- deselect large domain and select the remaining domains
- Click Align
- Click OK

Now all the domains will have a positive orientation. Note: the above steps only work for 100% structured domains that all connect to each other.

The term "Volume Condition" is generic and meant to represent cell zones, which in 2D is a plane. Yes, your VC setup is correct. The name and type you give it will be recognized and show up in Fluent.

daenerys December 19, 2014 13:07

2 Attachment(s)
Hmmm... My mesh is not all structured. The left bit is Unstructured.
Which explains why I can't select all 3 domains and choose orient, as in that case, orient is greyed out.
I can only select the two structured domains and orient.

cnsidero December 21, 2014 15:55

Quote:

Originally Posted by daenerys (Post 524705)
Hmmm... My mesh is not all structured. The left bit is Unstructured.
Which explains why I can't select all 3 domains and choose orient, as in that case, orient is greyed out.
I can only select the two structured domains and orient.

You'll have to set the orientation on the unstructured domain separately. Although it's much easier because it has arrows indicating the direction.

daenerys December 23, 2014 08:28

Quote:

Originally Posted by cnsidero (Post 524864)
You'll have to set the orientation on the unstructured domain separately. Although it's much easier because it has arrows indicating the direction.

Hallelujah! It worked!
Thanks a lot mate.

imen March 19, 2015 10:38

need a help
 
hi I Imen, I need someone who can help me.
I do not know how to work on pointwise I urgently work on this software, please if anyone can help me, and thank you.

dgarlisch March 20, 2015 10:35

imen,

I strongly suggest you create a NEW posting for this question. Adding an unrelated question to a very old post is contrary to good posting policy.

Since you are new to Pointwise, the best place to start is by doing one or more of the following things:
  1. Go to the Help / Tutorial Workbook... menu and run the tutorials included with Pointwise.
  2. View the numerous DIY, webinar, and Let's Talk Meshing videos on the Pointwise website.
  3. Call technical support (be sure to have your customer ID ready).
  4. Attend one of our Pointwise training classes.

If you have any specific questions after watching the videos and following the tutorials, please start one or more new posts.

Good luck!


All times are GMT -4. The time now is 09:29.