Learning Forum

[Jeje]

Hello,

I have a real problem and i don't know how to figure it out.

I am doing simulation about a simple system (composed of 2 plates united by a tube) with 20 parameters (all of them are about plates's thickness varying from 0.5 to 5 mm). And as i want first result, i perform calculations by using Screeening Method and my objective is to reduce the mass of my system.

The problem is that calculation takes at least 2 days and for a simple system composed of 2 plates and a tube, it's really weird.......

If one can help me to fix it, it would be great. At the beginning i thought it was because of my meshing size or the thickness plage (o.5 to 5mm), but it seems that not at all. By the way i changed the methods, but things went worse. 

thanks in advance for your answers !

[peteroznewman]

To do optimization, you need a model that solves in a short time. I expect your model is all solid elements, and takes a long time to solve.  If you change your model to be all shell elements, it will solve in a much shorter time. I recommend you convert your solid bodies into Midsurface sheet bodies, and create a shell element model of your optimization.  Please show your geometry.

If you can't use a shell model for some reason, then you must make the mesh as efficient as possible. If your mesh is Tet elements, you can reduce the number of nodes by about half if you replace that with Hex elements. Please show your mesh.

Another idea is if you have turned on Large Deflection, but the deflections are small, turn off Large Deflection and the solver will do fewer iterations to get to the solution.

[Jeje]

Thanks for the reply !

I have already tried to change the model to shell element by using Midsurf but i get an error message when meshing (image1)

I have replace also the Tet by Hex elements like you suggest, but doesn't get better.

And i turned off Large Deflection. 

 

[peteroznewman]

Please attach a Workbench Project Archive .wbpz file to your reply after you post it, and say what version of ANSYS you are using.

[Jeje]

I am using Ansys 17.0 

 

[peteroznewman]

In DesignModeler, slice the the disks off the stem using a plane on the inside face of each disk. Use Midsurface on each disk to replace the solid body with a sheet body.

In Mechanical, use Bonded Contract to connect the two disks back to the stem.  Mesh this and you will have a large reduction in solution time.

[Jeje]

I have followed all the steps, but it still takes time and some error message during calculation .....

[peteroznewman]

It still takes time, but does it take less time?

If you want help with the error messages, please upload a new copy of your archive with the shell mesh modification.

[Jeje]

Not really, calculation are still going since yesterday....

Here is the attached file and the error message

[peteroznewman]

Jeje,

You have 22 variables you are requesting to do Direct Optimization. This is too many variables for Direct Optimization.

The error message is saying you don't get a valid model when changing these parameters.  The computer is spending all its time sending data to DM and getting nothing back to analyze.

I had a closer look at it seems your model is building disks to unite onto the base disk as shown below.

You can't midsurface a solid like that, so you are going to have to delete the midsurface feature.

I suggest you recreate the disk and use a spherical surface for the face and vary the radius of the sphere to thicken the center and offset the sphere to control the thickness of the edge, that way, you only have two parameters for each disk.

Another suggestion, the two disks are both supported by a Fixed base.  Instead of including the support, just imprint the support outline onto the disk and support the face on the disk and suppress the solid body base.

Finally, both disks have similar shapes and supports. Can you run the optimizer on just one disk?

[Jeje]

Hi Peter,

i have finally run the optimization for only one disk with the support and effectively it takes less calculation time and no error message

Recreating the disk by using Spherical surface didn't help as i want to know the thickness discretization of each disk

I just have some questions that throw in my mind :

Why cannot i use Midsurf to my geometry ? And what are the common examples of using Midsurf in simulation ? 

And you said that : ''22 parameters is too many for Direct Optimizer'', is it mean that Direct Optimizer can be used only with few parameters (10 or less?) ? Which Design Exploration Ansys sytem is able to run the optimization with 22 parameters (Response Surface ?) ? 

Which one between Tet et hex elements is better for meshing and provide accurate solution? As i know Tet requieres many elements and Nodes, more than Hex. So i guess Tet ? 

Any other further explanation would be great !

Thanks !

 

 

[peteroznewman]

Midsurface only works on a uniform wall thickness part.  The most common example is for structures made from sheet metal.

Trying to run a direct optimizer over 22 parameters is just too slow!  The model starts at some initial value of those 22 parameters, then it has to decide which direction to move. That takes 22 solutions each time it has to decide on a direction to search, which is done over and over.

Another approach is to sample the design space. With just 2 values per parameter, that is 2^22 = 4.2 million possible designs to sample from. Compare that with 7 parameters which is 2^7 = 128 possible designs.  You can see that you can easily afford to sample half the design space if you only have 7 parameters.

That is why the Design Exploration toolbox has tools to help you decide which parameters might be important and which ones might be insignificant, so you can pare down the list to a few important parameters.

To fill a 10 mm cube with 1 mm elements takes 1000 Hex elements or 2000 Tet elements. The node spacing in each case is equal, 1 mm, so the accuracy might be considered equal, but there were more Tet elements.

[Jeje]

It's clear now,

Thanks you !