[Anna Tian]

I run CFX simulation by workbench. After I start to run the simulation, the simulation stuck at the message:

‘The MeTiS partitioning method allocates additional memory. Total memory usage will therefore exceed the values shown above.’

Then the simulation doesn’t proceed anymore.

I’m quite sure that I shall have enough memory (128 GB) available for that simulation (16 millions structured grids from ICEM, steady state SST).

The bad thing is: it doesn't give any error information. So that I have no clue what causes the problem and how to solve it.

I’m wondering what’s the reason of it? And how to solve this problem? Any hint?

[Whitebear]

Do you have enough parallel licenses? Have you try to change memory allocation factor? 1.2x or 1.5x in solver option? Do you solve multiphase or multicomponent problem?

[Anna Tian]

Originally Posted by Whitebear

Do you have enough parallel licenses? Have you try to change memory allocation factor? 1.2x or 1.5x in solver option? Do you solve multiphase or multicomponent problem?

I have checked with another simulation that my machine has enough parallel licenses. I'm solving single phase problem with 2 domains defined (GGI as interface). Another simulation with 2 domains could run without problem.

I haven't tried memory allocation factor, because i never got a hint that tells memory is not enough.

[Anna Tian]

Originally Posted by Whitebear

Do you have enough parallel licenses? Have you try to change memory allocation factor? 1.2x or 1.5x in solver option? Do you solve multiphase or multicomponent problem?

Just tried memory allocation factor of 0.8 and 1.5. Not working

[Whitebear]

Do you have many interger interfaces? What is the differences between the two problems?

[Anna Tian]

Originally Posted by Whitebear

Do you have many interger interfaces? What is the differences between the two problems?

There are two domains (named domain1, domain2) connected by a GGI interface. This is what I want to run. I run it, get problem specified above.

So I did the tests as below.

I run only domain1, no that problem.

I run only domain2, no that problem.

I create a simple domain3. Connect domain1 and domain3 by GGI. Working.

[Anna Tian]

Originally Posted by Whitebear

Do you have many interger interfaces? What is the differences between the two problems?

This is another problem i found out at the same time. It might be related to this one.

http://www.cfd-online.com/Forums/cfx...rted-icem.html

[Anna Tian]

Originally Posted by Whitebear

Do you have many interger interfaces? What is the differences between the two problems?

I figure out that the 'problematic' simulation could run actually. It is not stuck there as I said before. But it takes more than 5 hours to start. Too slow.

Never got this 'slow' problem before at the same workstation. So it shall not be caused by hardware.

[ghorrocks]

Very complex configurations can take ages to start. For instance lots of GGIs or boundaries, lots of CEL, lots of additional variables.

[Anna Tian]

Originally Posted by ghorrocks

Very complex configurations can take ages to start. For instance lots of GGIs or boundaries, lots of CEL, lots of additional variables.

Is there a good way to reduce the too long starting time besides reducing these factors you mentioned?

[ghorrocks]

ANSYS has already worked hard to make simulations start as quickly as possible. There are no quick fixes to make it go faster, if there were they would already be in the software.

There must be something about your simulation which is causing the very long start time. If you want us to help you you will have to describe what you are doing.

For instance: How many nodes in your mesh? How many boundaries, GGIs and anything else you have set up?

[Anna Tian]

Originally Posted by ghorrocks

ANSYS has already worked hard to make simulations start as quickly as possible. There are no quick fixes to make it go faster, if there were they would already be in the software.

There must be something about your simulation which is causing the very long start time. If you want us to help you you will have to describe what you are doing.

For instance: How many nodes in your mesh? How many boundaries, GGIs and anything else you have set up?

17millions structured grids nodes. 15 boundaries. 30 expressions.

[ghorrocks]

17 million grids (elements?) is getting large, but should not take 5 hours to start unless you have run out of memory or some other problem.

I would do some basic fault finding. Take a simple simulation (like a tutorial example) and make it 17 million elements. Does it run quickly? Remesh your simulation with half the number of elements - does it start quickly?

[Anna Tian]

Originally Posted by ghorrocks

17 million grids (elements?) is getting large, but should not take 5 hours to start unless you have run out of memory or some other problem.

I would do some basic fault finding. Take a simple simulation (like a tutorial example) and make it 17 million elements. Does it run quickly? Remesh your simulation with half the number of elements - does it start quickly?

Yes. I tried. It would be much faster if I coarsening grids.

By the way, once I have run the simulation and use its result file as initial solution of a new simulation. The simulation would start very fast without any problem.

So I guess maybe that's because the initial solution grids of the 'too slow' simulation do not correspond to the new simulation.

I asked the question below as well for this reason.

http://www.cfd-online.com/Forums/cfx...nning-cfx.html

[ghorrocks]

Yes. I tried. It would be much faster if I coarsening grids.

No, you have missed the point. It is trying to work out whether it is simply the size of the simulation which is the problem or your problem specifically, regardless of the size.

So I guess maybe that's because the initial solution grids of the 'too slow' simulation do not correspond to the new simulation.

If you are using an initial condition which requires interpolation this can be very slow, especially for large grids. That would explain the problem.

[Anna Tian]

Originally Posted by ghorrocks

No, you have missed the point. It is trying to work out whether it is simply the size of the simulation which is the problem or your problem specifically, regardless of the size.


If you are using an initial condition which requires interpolation this can be very slow, especially for large grids. That would explain the problem.

Then how to avoid slow interpolation in workbench?

[ghorrocks]

Do not specify an initial condition results file. Leave it blank.

[Anna Tian]

Originally Posted by ghorrocks

Do not specify an initial condition results file. Leave it blank.

Yes. I the default setting of Workbench cfx pre is blank as shown in the figure attached.

But it actually uses one as I got the following lines in the output file.

‘
INITIAL VALUES SPECIFICATION:
INITIAL VALUES CONTROL:
Use Mesh From = Solver Input File
Continue History From = Workbench Initial Values
END
INITIAL VALUES: Workbench Initial Values
Option = Results File
File Name = 20_fine_019.res
END
END
END
‘

If I change the setting, i will get the error message as stated in the thread below.

http://www.cfd-online.com/Forums/cfx...nning-cfx.html

[singer1812]

Lets go back to your original warning. Did you increase the amount of memory for the "partitioner" (not the run, there is a difference)?

I dont use Solver Manager to start my jobs but in command line it is:

-size-part <factor>

I have had to increase this with 2 domain GGI runs before as CFXs estimate is low.

The command -size will just increase the solver memory, but not alter the allocation for the partitioner.

[Anna Tian]

Originally Posted by singer1812

Lets go back to your original warning. Did you increase the amount of memory for the "partitioner" (not the run, there is a difference)?

I dont use Solver Manager to start my jobs but in command line it is:

-size-part <factor>

I have had to increase this with 2 domain GGI runs before as CFXs estimate is low.

The command -size will just increase the solver memory, but not alter the allocation for the partitioner.

Yes. I once tried by increasing the allocation factor to 1.5. It still reacts slow if it use another simulation's result file as the initial solution.

According to the discussions above, there's no hint that the problem is caused by lack of memory up to what we see now.