CFD Online Logo CFD Online URL
www.cfd-online.com
[Sponsors]
Home > Forums > STAR-CCM+

repair surface problem

Register Blogs Members List Search Today's Posts Mark Forums Read

Reply
 
LinkBack Thread Tools Display Modes
Old   June 17, 2012, 01:24
Default repair surface problem
  #1
Member
 
adam
Join Date: Oct 2011
Posts: 52
Rep Power: 5
sieginc. is on a distinguished road
I'm working with an imported geometry created in SolidWorks that looks something like this:



It is an air duct with two open ends as you can see. However, when I import it into star-ccm+ and do surface repair, star for some reason does not recognize the free edges at the openings as one would expect to find:



When I try to fill the holes at the inlet and outlet, star creates a cap that extends all the way to the outer edge instead of the inner. This results in non-manifold edges:



Obviously, I cannot mesh as it gives me an error that says the region pertaining to this part is non-manifold. I am confused as to why star does not think the open ends do not have free edges?
sieginc. is offline   Reply With Quote

Old   June 17, 2012, 04:40
Default
  #2
Senior Member
 
KHB
Join Date: Aug 2010
Location: Singapore
Posts: 107
Rep Power: 7
lava12005 is on a distinguished road
You can select the inner edge manually and create face based on those edges.
Then try to mesh again.
lava12005 is offline   Reply With Quote

Old   June 17, 2012, 12:08
Default
  #3
Member
 
adam
Join Date: Oct 2011
Posts: 52
Rep Power: 5
sieginc. is on a distinguished road
Quote:
Originally Posted by lava12005 View Post
You can select the inner edge manually and create face based on those edges.
Then try to mesh again.
This is what I tried to do, but like I said star does not make a face that touches those inner edges. It creates a cap that touches the outer ones which is why I now have non-manifold edges.
sieginc. is offline   Reply With Quote

Old   June 17, 2012, 21:04
Default
  #4
Member
 
adam
Join Date: Oct 2011
Posts: 52
Rep Power: 5
sieginc. is on a distinguished road
Well I seem to have fixed my previous problem by just capping it in SolidWorks, and then re importing it. I'd still like to know why Star-ccm+ didn't recognize those edges at the openings as "free" when they should have been.

On to a new problem: when creating interfaces, if you are supposed to have the same surface of a part show up in two different regions so you can select them both and create an interface, how do you do this? At first I thought you create duplicate parts, and then just send them both to regions and define one as fluid and one as solid for example. However, when I do this I get interference errors and connectivity errors when I try to mesh. When I erase one of the duplicate parts out of regions, this problem goes away, but now I can't create my interface. What is the proper way to do this?
sieginc. is offline   Reply With Quote

Old   June 18, 2012, 15:01
Default
  #5
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
As long as your imported body is a closed solid, there is no such thing like a free edge. And for me it looks like several closed bodies.

Regarding your second issue: What do want to simulate?
__________________
We do three types of jobs here:
GOOD, FAST AND CHEAP
You may choose any two!
abdul099 is offline   Reply With Quote

Old   June 18, 2012, 15:31
Default
  #6
Member
 
adam
Join Date: Oct 2011
Posts: 52
Rep Power: 5
sieginc. is on a distinguished road
Quote:
Originally Posted by abdul099 View Post
As long as your imported body is a closed solid, there is no such thing like a free edge. And for me it looks like several closed bodies.

Regarding your second issue: What do want to simulate?
I don't think it's a closed solid, if you look at my first picture you can clearly see the duct inlet and outlet are open. Unless I'm misinterpreting how star defines closed geometries.

I am trying to simulate a conjugate heat transfer problem. If you look in the first picture, that solid block generates heat and I want to have air passing through the duct to investigate the convective cooling of the block. I have repeatedly tried to create interfaces between the block surfaces and air, and between the contact of the block sitting on the base of the duct. In my parts tree I have the block and duct each as a separate part (they came in as an assembly from SolidWorks). I create a duplicate part for the block so there are now two, and then send all three parts to regions. I define one of the blocks as a solid, and one as air. Then I select all the surfaces and create interfaces. I thought this was how it was supposed to be done, but when I try to mesh I get errors saying things like "illegal connectivity" and "interference." When I delete one of the block regions (so now there is only one) this error goes away and I can mesh, but now I cannot create the interfaces because all of the block surfaces are in one region only.

What am I doing wrong? Thanks for your help Abdul.
sieginc. is offline   Reply With Quote

Old   June 18, 2012, 17:46
Default
  #7
Member
 
adam
Join Date: Oct 2011
Posts: 52
Rep Power: 5
sieginc. is on a distinguished road
Here is a download link to the sim file

http://www.sendspace.com/file/bj3gk7
sieginc. is offline   Reply With Quote

Old   June 18, 2012, 18:43
Default
  #8
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Quote:
Originally Posted by sieginc. View Post
I don't think it's a closed solid, if you look at my first picture you can clearly see the duct inlet and outlet are open. Unless I'm misinterpreting how star defines closed geometries.
Well, that's one of the issues. You seem to be misinterpreting it. Imagine a cube. I'm pretty sure, you'll agree it's a closed body. There's one volume surrounded by six faces.
Now imagine, you would drill a hole in the cube, you will have seven faces (the surface of the drilling plus the 6 cube faces). Then virtually coat all surfaces with a thin plastic layer and remove the metal. Now you've got a plastic shell. Trap a mouse inside. It would not be able to escape, right? So it's a closed body.

Regarding your geometry: Don't think in terms of "parts I got from CAD". Think in terms of "parts I want to simulate". You want to simulate your air flowing through the duct. And you want to simulate the block. So you need ONE air part and ONE solid part.
I'm currently not sure if you want to simulate the air inside the block as well since it seems to be hollow. So maybe there's a second air part.

Anyway, the outer air part represents the whole air volume inside the duct WITHOUT the block. The block is some solid material, so it can't be filled with air, right?
And you need the solid part, representing the solid material of the block.

To get this, follow this steps:

First get rid of the assembly. Right-click on the assembly, choose explode. Delete "cube 2" and "Part5 3" and "Base", you don't need them anymore. Combine "Cube Base" and "cube". This will result in a part representing the block volume. Go to the surface repair with this part and run a diagnostics. Select all free edges and zip them. Now you should have an error free part.
Now exit the surface repair, enter it again with both remaining parts (one representing the complete air volume in the duct and one the solid). Select "Merge/Imprint" from the drop down menu. Select Multi-part imprint. Hit the "find pairs" button. Make sure, the air volume is marked red (if it isn't, click that button on the left with the two arrows, one pointing up, the other one down). Then hit the "imprint pair" button.

Now choose "surface repair" again from the drop down menu and run a diagnostics. When it's error free, exit the surface repair. Now select both parts, right-click and choose "Boolean -> subtract". The target part is the part representing your air volume, in my example it's "Part5 3". Rename the new body to a name of your choice. Then Right-click it and select "split non-contiguous". When it complains about a patch spanning multiple parts, find this part surface and choose "split non-contiguous" on this part surface first.

After the split you will have four parts: One representing your solid block. This one will still be needed. One representing the old air volume. You don't need it anymore. You can delete it or not, that's up to you. I usually delete it when I'm absolutely sure I don't need it anymore. And you've got two parts, one representing the air volume minus your solid block and one the air inside the hollow solid block. I assume, you don't need the internal air of the hollow solid, so I've deleted it. Now there are two parts remaining.

Select both parts, right-click and select "create regions from parts". Make sure to select "one region per part" and "one boundary per part surface".
Now you should have two regions. Assign the solid physics continuum to the solid part, choose the appropriate boundaries of both parts and create the interfaces. You will have the same surface in both parts due to the Boolean -> Subtract you performed earlier.

When you need other solids as well like the duct, make sure you've got a closed geometry (all faces together building this mouse trap without any holes) representing exactly the duct, not more and not less. The same when you need the air volume inside the hollow block.

As a general hint: Your setup tells me, you don't really now what you're doing and why you should do it. This is frustrating and time consuming, although it doesn't need to be. When you know what to do and how to do it, it's a quick job not taking more than 20 minutes. So I recommend to try some of the tutorials you can find in the user guide. Try to understand the principle behind!
__________________
We do three types of jobs here:
GOOD, FAST AND CHEAP
You may choose any two!
abdul099 is offline   Reply With Quote

Old   June 18, 2012, 18:54
Default
  #9
Member
 
adam
Join Date: Oct 2011
Posts: 52
Rep Power: 5
sieginc. is on a distinguished road
Thank you so much for your help. One problem I'm having as I'm following your steps is that when I try to zip edges, it deforms my geometry. It says I have 32 free edges, and I zip them, and it goes down to 6, but the inside of my duct looks like it gets warped slightly. Also, what about the inlet and outlet? I need each to have a surface so I can define an incoming velocity and pressure outlet. I get what you are saying about closed geometry. I think star assumes that the fluid region is the small space that is my duct wall thickness which it's not, this is technically just a solid piece of aluminum sheet metal.
sieginc. is offline   Reply With Quote

Old   June 18, 2012, 18:57
Default
  #10
Senior Member
 
Join Date: Oct 2009
Location: Germany
Posts: 637
Rep Power: 12
abdul099 is on a distinguished road
Hm, then you're zipping the wrong edges... I will try to post some screenshots what to do tomorrow, for today it's too late.
__________________
We do three types of jobs here:
GOOD, FAST AND CHEAP
You may choose any two!
abdul099 is offline   Reply With Quote

Old   June 18, 2012, 19:27
Default
  #11
Member
 
adam
Join Date: Oct 2011
Posts: 52
Rep Power: 5
sieginc. is on a distinguished road
Nevermind my mistake I fixed it and got the simulation running. The results match well with my actual test, thank you so much for your help.

Last edited by sieginc.; June 19, 2012 at 02:18.
sieginc. is offline   Reply With Quote

Reply

Thread Tools
Display Modes

Posting Rules
You may not post new threads
You may not post replies
You may not post attachments
You may not edit your posts

BB code is On
Smilies are On
[IMG] code is On
HTML code is Off
Trackbacks are On
Pingbacks are On
Refbacks are On


Similar Threads
Thread Thread Starter Forum Replies Last Post
[ICEM] Problem making structured mesh on a surface froztbear ANSYS Meshing & Geometry 4 November 10, 2011 09:52
Problem about a 2D surface rotation skyblue_mech Main CFD Forum 0 June 8, 2010 04:49
surface orentation problem in icemcfd jeevan kumar CFX 0 August 18, 2008 04:25
Surface orentation problem in icemcfd jeevan kumar CFX 0 August 13, 2008 01:54
Surface tension problem. Kes FLUENT 0 May 19, 2008 22:49


All times are GMT -4. The time now is 19:47.