ICEM CFD as a Data Compliant System in ANSYS Workbench

ICEM CFD is probably the most capable mesher on the planet. Not only do we here at PADT use it as our preferred tool for creating complex hex meshes, it has a whole host of other capabilities and controls that make it the power users choice. But one thing that has been frustrating for some time is that we could not easily add it into a project that automatically updates. At 14.5, ICEM CFD is now data compliant and you can use it in a project with parameters.

ICEM-CFD-System-ANSYS-Workbench

If you know ICEM CFD well you know that there are many aspects of it that do not fit into a project flow, but the most commonly used capabilities do: read in geometry, mesh it, output nodes and elements into a solver or node/element based pre-processor. Because it is node/element based it does not work with ANSYS Mechanical or other tools that require surface or solid geometry, but it does work with FLUENT, CFX, ANSYS Mechanical APDL (MAPDL) and Polyflow, the ANSYS solvers that can work directly with nodes and meshes. Once put into your system, you can modify geometry or ICEM CFD parameters and then update your system to get a new solution.

In this article we will focus on using ICEM CFD with ANSYS MAPDL. That is because 1) most of our readers are ANSYS Mechanical/MAPDL users and 2) it is what I know best. But most everything we are talking about will work with FLUENT, CFX, and Polyflow.

Why is this a Big Deal?

For the vast majority of users, this is not such a big deal because they can do all their meshing with ANSYS MAPDL, ANSYS Mechanical, ANSYS Meshing, or FLUENT (with TGrid meshing). But if you can not, then this is an awesome new capability. This is especially true if you need to use the blocking based hex meshing built into ICEM CFD.

Getting Started and Things to Know

Frist thing we recommend you do is read the help on the ICEM CFD System:

Workbench User Guide // User’s Guide // Systems // Component Systems

Click on ANSYS ICEM CFD and read the whole thing. There are lots of little details that you should be aware of.

The first thing you should note is that if you want to use it with Mechanical APDL you need to turn on Beta Features: Tools>Options>Appearance scroll down and check “Beta Options” to be on.

The next thing is to realize that from a project standpoint, you can feed an ICEM CFD system with any system that has a geometry module. Although ICEM CFD will read a mesh in and use the external surface of that mesh as geometry, that capability is not currently implemented in Workbench. This means if the source mesh changes, you can not automatically update your mesh if the “geometry” mesh changes. See below for a work around.

You do need to make sure that your ICEM CFD model is setup to output to your solver type. Make sure you check this when you are setting up your mesh.

If you have worked in Workbench with legacy mesh you know that named selections can be very important. I did not have enough time to play with all the different options, but it looks like named selections come in from DesignModeler, and if they define a solid, the resulting nodes that are in that solid get written as a component that goes to the MAPDL solver. However, surface, edge, and vertex named selections do not seem to get passed over at this time. I am contacting ANSYS, Inc. to see if there is a way to turn that on.

It also looks like if you are using blocking only the solid elements are written, and no corner, edge, or surface elements are output. I will also be checking on this.

The last, and most important thing to know, is that your ICEM CFD model needs to be robust. Anyone that spends a lot of time in ICEM CFD already knows this. If you make a change to geometry or a parameter, then it needs to update reliably. The key to success with this is to just do your meshing with updates in mind and make it as simple and flexible as possible, especially if you are blocking with HEXA.

A Simple Example

I made a very silly model, because these Focus articles are always about silly models, that sort of shows the process you can use. It is not a flat plate with a hole in it, but it is a block with a cylinder on top.

image

Nothing too fancy. I made the block dimensions, the cylinder diameter, and its offset parameters.

This system feeds the ICEM CFD system where it comes in as points, lines, and surfaces.

image

I then blocked it out:

image

And specified meshing sizes:

image

And generated the mesh:

image

Like I said, a simple model.

Parameters are supported for meshing controls, any user parameters you want to make that you will use in Tcl scripts, or meshing diagnostics.

I made the number of nodes across the width a parameter:

image

Values that you can make into parameters have little white boxes next to them. To make them workbench parameters click on the box and you get the “Blue P” that everyone should know and love from all of the other ANSYS, Inc. applications.

I also wanted mesh parameters so I went to Settings->Workbench Parameters->Workbench Output Parameters and set some of those:

image

Now when I go back to my project and check out the parameters for my ICEM CFD system I get:

image

Now it is time to add the ANSYS Mechanical APDL system. You will want to write a macro that defines material properties, constraints, and loads. Mine also has some output parameters and makes some PNG plots.

This is the mesh I get in MAPDL:

dp0_000

and here are the results. Exciting:

dp0_001

To try the whole thing out I made a design study:

image

Everything updated just fine and I got all my output parameters and my plots in my MAPDL directory for each design point (remember to tell it to save all the design points or it deletes them, or use a macro like the one discussed in the bonus article from this posting).

I made an animated GIF of the different meshes for fun:

DesignPoints_ICEM-CFD-1

Here is a link to an archive of the project I used:  ICEM-wb-1.wbpz

Doing more with ICEM CFD in a Project

This was a basic example. But the cool thing about the implementation is that it will do much more. If there is a replay file, it will execute the file and run whatever scripts you specify in the file. This is how you can get it to work with existing meshes as geometry. And you can do whatever else you want to do.

On an update ICEM CFD does the following:

  1. Update geometry if Tetin file changed
  2. Runs tetra default meshing, if no blocking file and no replay file
  3. If a replay file, run the replay file
  4. Runs Hexa default meshing if a Blocking file exists
  5. Convert any blocked mesh to unstructured mesh file
  6. Convert unstructured mesh file to solver input file
  7. Save the project

So you just need to be aware of this order and plan accordingly. There really is no limit to what you can do.

Next Steps

If there was ever a place to use Crawl-Walk-Run this is it. Make yourself a very simple model and get a feel for things. Then work with your real geometry doing some simple meshing, maybe just blowing a TET mesh on it, then set up you full run. Also, keep the simple model around to try stuff out when you are working with the big model.

The help was very helpful, I recommend that you read it once then reread it after you have played around with this feature a bit.

4 Replies to “ICEM CFD as a Data Compliant System in ANSYS Workbench”