Hello Guest !!! Welcome to LearnCAx community forum. All the forums are open for view to everyone. If you wish to participate in any discussion or ask question, login using your LearnCAx account. If you are new to LearnCAx, create your FREE LearnCAx account now !!

Login


Create FREE LearnCAx Account Now !!

QUESTION: meshing of ventilated disc brake in ICEM CFD

meshing of ventilated disc brake in ICEM CFD 3 years 4 days ago #16

  • Praveen Kumar
  • Praveen Kumar's Avatar
  • OFFLINE
  • Moderator
  • Posts : 75
  • Thanks received : 50
  • Upvotes : 10
Hi,

Sorry to answer a question with another question :) Following are the list of questions that I have:

1) What is the objective of your CFD simulation? External Flow?
2) What is the CFD domain that you have considered for meshing in your initial trials?
3) Did you generate surface mesh first and then volume mesh? If yes, did you try 'All tri' Mesh type and 'Patch Independent' method for surface mesh generation?
4) What is the error message that you got while generating tetra/prism mesh?

Please post images of CFD domain the you have used (not the CAD model of component) and error message / mesh images

Note: The CAD model of disc brake needs to be simplified as suggested by Vijay in the previous post. Eg: Stampings on the disc should be removed. But in the recent geometry that you have uploaded, you have removed the complete plate surface instead.

Best Regards
Praveen Kumar
LearnCAx
www.learncax.com
The administrator has disabled public write access. Please login with LearnCAx account.
The following user(s) said Thank You: nikhil kuttamath

meshing of ventilated disc brake in ICEM CFD 3 years 3 days ago #17

sir,

here i am attaching the some images that regard the messages and errors that i have met during the meshing and the set up.

1.the model that i have used for meshing.
2.incomplete meshing while performing volume mesh.
3.during the first step of "setup" operation, took double series
4.during the "set up" took parallel

dsf.gif
Last Edit: 3 years 3 days ago by Vijay Mali.
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 3 years 3 days ago #18

sir, sorry, some failure occurred while sending the images.

Screenshot2015-09-1914.58.33.jpg


duringserialprecession.jpg


duringparallelprecession.jpg
Last Edit: 3 years 3 days ago by Vijay Mali.
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 3 years 3 days ago #19

  • Praveen Kumar
  • Praveen Kumar's Avatar
  • OFFLINE
  • Moderator
  • Posts : 75
  • Thanks received : 50
  • Upvotes : 10
Out of the four questions that was asked, I of got the answer(not exactly, but sort of) only for the 4th one.
1) What is the objective of your CFD simulation? External Flow?
2) What is the CFD domain that you have considered for meshing in your initial trials?
3) Did you generate surface mesh first and then volume mesh? If yes, did you try 'All tri' Mesh type and 'Patch Independent' method for surface mesh generation?
4) What is the error message that you got while generating tetra/prism mesh?

I need answers for the first question at least. Because your objective of the CFD simulation will decide your CFD domain.
Praveen Kumar
LearnCAx
www.learncax.com
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 3 years 2 days ago #20

sir,
1.objective is to find the heat transfer coefficient(h)for both straight vane and inclined vane disc brake rotor and correlation.
2.In early meshing what i have considered is the full part that have shown last message.
3.Yes,generated surface mesh before volume mesh with "All Tri" and Patch independent options.
4.I put global parameter max. element randomly as 32,then part mesh parameter max.size i put "3" and mini.size given as "0.5",also given prism height 1 and height ratio 1.2(note:actually i am unaware of giving these sizes)
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 3 years 2 days ago #21

  • Praveen Kumar
  • Praveen Kumar's Avatar
  • OFFLINE
  • Moderator
  • Posts : 75
  • Thanks received : 50
  • Upvotes : 10
There are three things I want to discuss with you

1) CFD Domain:
OK. If guess you are meshing a wrong domain. This needs to be corrected first.

I am assuming a Forced convection situation here. The component is at some hot temperature, and is exposed to cold air flowing around at a constant speed. The objective is to find htc of the component at a constant temperature.

In this case, we need to create a domain (bounding box) around the component representing atmosphere. So that we can assign air inlet, outlet and constant temperature wall boundary conditions. Also the volume mesh needs to be created outside the component and not inside the component. (if we fix the component temperature and assume steady state)

I would strongly suggest you to watch our webinar: CAD Repair for CFD Simulation and read our blog Introduction to CFD – Part II : Selecting the Domain

2)Surface to volume mesh:
Once you have created surface mesh using 'All tri' Mesh type and 'Patch Independent' method, we need to run 'Check Mesh' under 'Edit Mesh' tab. This will report all the errors in the domain. Once we fix the errors in surface mesh, then its a green signal for generating volume mesh.

3) Meshing parameters:
Global size sort of fixes your maximum tetra size in the volume/domain. Surface max size should be given based on, whether the no. of mesh elements are sufficient enough to capture the shape of the geometry and the flow physics.

For example: Take a case of flow through a circular pipe of 1m dia. Here you might need 25 to 30 tetras + 2x5 layers of prism cells in wall to wall direction. So, divide the dia by no. of cells i.e,. 1/25 = 0.04 could be a good max. size on the surface.

Alternate method: Calculate the first cell height required using Yplus calculator. To have an aspect ratio of 150, multiply first cell height by 150 and you get max. size on surface. But this might not work for all the scenarios.

Best Regards
Praveen Kumar
LearnCAx
www.learncax.com
Last Edit: 3 years 2 days ago by Praveen Kumar.
The administrator has disabled public write access. Please login with LearnCAx account.
The following user(s) said Thank You: nikhil kuttamath

meshing of ventilated disc brake in ICEM CFD 3 years 1 day ago #22

sir,
how can i select the domain which includes the vanes.Also i am having heat flux of the surface,so whether i have to create the block.
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 3 years 13 hours ago #23

  • Praveen Kumar
  • Praveen Kumar's Avatar
  • OFFLINE
  • Moderator
  • Posts : 75
  • Thanks received : 50
  • Upvotes : 10
Normally for external flow cases, we import the object/component from CAD file and create a bounding box (atmosphere) in ANSYS ICEM CFD using geometry options/tools.

Still the objective of CFD simulation is not clear to me. Although you have mentioned
objective is to find the heat transfer coefficient(h)for both straight vane and inclined vane disc brake rotor and correlation.
There are doubts like:
Is it natural / forced convection?
Component temperature is fixed? i.e., steady state or unsteady

And by saying,
i am having heat flux of the surface,so whether i have to create the block
you have given a different dimension to the problem :)
Do you have the heat flux W/m2 (constant/varying?)value of the component?

Best Regards
Praveen Kumar
LearnCAx
www.learncax.com
The administrator has disabled public write access. Please login with LearnCAx account.
The following user(s) said Thank You: nikhil kuttamath

meshing of ventilated disc brake in ICEM CFD 3 years 5 hours ago #24

Sir,
Problem is a wheel decelerates from 100-0kmph with initial temp.40c .heat flux calculated from given condition and weight of the vehicle and got in W/m2....Fluid is air with velocity 11m/s.
1.heat flux is constant
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 2 years 11 months ago #25

sir,
please help me for blocking the brake rotor.
1. i have done initialize blocking, but how can i provide inlet and outlet surface to the block?
I searched many videos but did'nt get anything related to the complete blocking for external analysis
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 2 years 11 months ago #26

  • Praveen Kumar
  • Praveen Kumar's Avatar
  • OFFLINE
  • Moderator
  • Posts : 75
  • Thanks received : 50
  • Upvotes : 10
Hi,

This geometry is complex for creating structured hexa mesh using Multi-Block method. I would strongly suggest you to go for unstructured tetra meshing with prism layers near the wall.

As a first task, lets create the CFD domain, before meshing.
  • Check if the component geometry is in the origin (0,0,0). You can use transform geometry tools to move it to origin.
  • Create a rectangular box around the component, representing surrounding/environment. The size of the domain can be 7.5D (D-Diameter of disk) on front, top, bottom, sides and 15D on the back. You can use standard shapes - surface creation option in the geometry tab, to do this.

Once you are done with above share the details. Then we can move to next steps.
Best Regards
Praveen Kumar
LearnCAx
www.learncax.com
The administrator has disabled public write access. Please login with LearnCAx account.
The following user(s) said Thank You: nikhil kuttamath

meshing of ventilated disc brake in ICEM CFD 2 years 11 months ago #27

sir,
the box created and provided name inlet and outlet as in below shown figure.
Attachments:
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 2 years 11 months ago #28

  • Praveen Kumar
  • Praveen Kumar's Avatar
  • OFFLINE
  • Moderator
  • Posts : 75
  • Thanks received : 50
  • Upvotes : 10
Any particular reason, why the shape of the domain is not rectangular? Inlet and Outlet are of different size?
Praveen Kumar
LearnCAx
www.learncax.com
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 2 years 11 months ago #29

sir,
I am confused with the size of the domain.Here i am attaching the recreated domain.
Attachments:
The administrator has disabled public write access. Please login with LearnCAx account.

meshing of ventilated disc brake in ICEM CFD 2 years 11 months ago #30

  • Praveen Kumar
  • Praveen Kumar's Avatar
  • OFFLINE
  • Moderator
  • Posts : 75
  • Thanks received : 50
  • Upvotes : 10
Hi,

Now the inlet and outlet surfaces looks good. But, I am finding it difficult to judge the location and orientation of disk w.r.t outer boundaries. Can you please, post all three views (front, top, side) or you can share the .tin file

Meanwhile you can follow this:

Global Mesh Parameters:
  • Scale Factor = 1
  • Specify 'Max element' based on the no. of cells needed in any one direction of volume.
Use 'Display' to judge the cell size
  • Shell Meshing Parameters: Mesh type - All Tri ; Mesh method - Patch Independent
  • Volume Meshing Parameters: Mesh type - Tetra/Mixed ; Mesh method - Quick (Delaunay) ; Spacing scale factor = 1.2 or 1.3
Surface Mesh Setup:
  • Specify Maximum size : Based on the no. of cells needed in any one direction of the surface.
  • To display the specified tetra size on surface : under display tree Geometry ----> (right click) Surfaces ----> Tetra Size
  • Save Geometry: All the sizing and meshing parameters get saved in the geometry file.
Shell Mesh:
  • Compute Surface Mesh
  • Smooth Mesh to get quality above 0.3
  • Check Mesh under Edit Mesh tab
  • Save Surface Mesh
Volume Mesh:
  • Compute Volume Mesh
  • Smooth Mesh to get quality above 0.2 or 0.3 (if possible)
  • Save the mesh file
Best Regards
Praveen Kumar
LearnCAx
www.learncax.com
Last Edit: 2 years 11 months ago by Praveen Kumar.
The administrator has disabled public write access. Please login with LearnCAx account.
The following user(s) said Thank You: nikhil kuttamath

Browse Knowledge Base

Recommended By

Get Instant Updates

Subscribe to get instant updates about CFD courses, projects, blogs, webinars, software tutorials & CFD jobs

Search Knowledge Base

By Keyword

By Author

By Tag