[QCFD]

Hello,

I am working with a simulation that involves a repeating pattern of fluid passages in a solid, think of it as a heat exchanger. This pattern repeats ~50x and there are 2 different fluid and solid zones per layer (2 solid zones cause there are different material properties) which led me to set up the problem with interfaces which include as many as 100 2-d mesh zones on a side.

My mesh count is well below what I have run in the past on the hardware I am using, but I am having issues where simulation startup (after partitioner but before 1st iteration) takes about 6 hours, hung at the same spot... which is many times more than I am used to, even for meshes with 2x as many volume elements.

Once the problem starts iterating, it runs quickly enough assuming it doesn't crash.

Is anyone familiar with what CFX has to do between partitioning and solving on GGI (there are no outputs in the .out file for the 6 hour period after partitioning).

Additionally, does anyone have suggestions for a better setup of a model with a large number of zones?

Note: all my solid-solid interfaces are conformal, fluid-solid are not.

I know that was long winded, but thanks in advance for your input

[ghorrocks]

You will need to change some defaults to get something like this to work.

* In solver manager, turn on coupled partitioning. This may fix the problem by itself.
* For the conformal interfaces, consider making them 1:1 rather than GGI.
* You may need to increase stack sizes in the partitioner or solver - it will tell you if you need to do this.

[QCFD]

Originally Posted by ghorrocks

You will need to change some defaults to get something like this to work.

* In solver manager, turn on coupled partitioning. This may fix the problem by itself.
* For the conformal interfaces, consider making them 1:1 rather than GGI.
* You may need to increase stack sizes in the partitioner or solver - it will tell you if you need to do this.

I was reading documentation today and came across information about the coupled partitioner. enabling coupled partitioner seems to have fixed the problem (my simulation is also way more stable using this setup)

As for the memory stacks, I had to play with those just to get to the point I am at now, but it was definitely needed to run the model.

Another thing I tried which reduced the startup time of the problem is user specified direction partitioner. my overlap percentages are worse, but the model started up quite a bit faster. *Note: this model seems to take more iterations to converge vs. an identical run using R.C.B. I suspect the flow of information has been biased by adding partition boundaries all in one direction along the model but this is just a guess based on what I am seeing

I do not have CFX pre up at the moment but I seem to remember I could only set 1:1 as the connection type if the volume elements on either side of the interface are in the same domain. I will check tomorrow and see if I can switch that since it should only help.
* Note: I just checked and 1:1 is definitely selectible in my case... not sure where I got this idea (disregard it)

Thanks for the input