🎉Community Raffle - Win $25

An exclusive raffle opportunity for active members like you! Complete your profile, answer questions and get your first accepted badge to enter the raffle.

Join and Win

Best alternatives to overcome error # 7004 - Free-size optimization with OptiStruct

Joao_Almeida · 2025-05-27T15:14:43+00:00

There was an error rendering this rich post.

Joao_Almeida

Hi there,
I am currently doing a master thesis project with the main goal of creating an optimized composite laminate version for a specific structure. In my case, I created, in a manual approach, a initial standard laminate (ply-based) for the component and now I would like to optimized it, particularly in terms of mass decrease while maintaining certain levels of displacement in specific node sets.

For the project, I created 7 load sets in which the optimization should be based on. When simulating a linear static analysis of those load steps, optistruct ran successfully and provided the expected results, however, when applying a free-size composite optimization of the laminate, the following errors occur:

*** WARNING # 7007
Automatic memory expansion failed.
Currently allocated memory is 881 MB.
Automatic expansion failed to expand to 69341 MB.
Solver will try to use more external storage.

*** WARNING # 3477
Solver out-of-core memory requirement 70225 MB exceeds host physical
memory 7060 MB. Please reduce number of processes per host or use more hosts.

My personal pc has the following specs: Intel(R) Core(TM) i7-9750H CPU @ 2.60GHz 2.59 GHz with 16 gb of RAM. Given that, I would to know what are the main alternatives in order to run the optimization with no issues:

- I have an external SSD disk where I usually put the simulations directory folders. Should I use the SSD as an out-of-core scratch storage, instead of RAM? If yes, how can I do it? Will it increase the simulation time largely?

- I have also the possibility of using a non-portable pc. If I try to run the simulation in that pc, what amount of RAM should be enough to comfortably run the optimization?

If there is any other solution, please feel free to purpose it! Thank you in advance.

(I am using a student license version and already try to simplify the overall model - bigger size mesh, decrease the amount of sets that are associated with the optim. constraints, etc.)

Find more posts tagged with

OptiStruct

Optimization

Accepted answers

All comments

Adriano_Koga

Hi João,

if no enough RAM memory is available, then out-of-core mode will kick-in with the minimum memory possible and using scratch in the hard-drive.

Running the model in a SSD location will be better, compared to regular hard drives, but still slower than if you had enough RAM.

If you have some other machine with more RAM memory available, it owuld be better.

But anyway, could you share the .out file here? or at least the memory stimation part of it, and model summary..

Joao_Almeida

Hi Adriano,

Thank you for your response. While I was waiting to get some response regarding my questions, I tried using other machine with more RAM and worked out perfectly (at least until now) so I am assuming that my problem is resolved. Neverthless, some other issues came out and I think it would be great to see if you could help me out:

Complementing my master thesis project, I was aiming to make some comparisons regarding different approaches for a certain scenario: application of a push test in a composite plate. This test basically consists in a application of a load in the center of a ball joint that would contact with a pad that, consequently, would be in contact with the composite plate. In practical terms, the simulation is composed of two consecutive contacts.

While, in a more simplified approach, I supressed both the ball joint and the respective pad and sonly utilized a rigig body constraint between the composite plate contact area and an indepedent node that would be the application point for the load, I would like to increase the accuracy of the load case and use the contact parameters.

The main goal is to evaluate the composite plate behaviour, assuming the ball joint as a rigid body (no deformation) and the pad composed of a rigid foam. In this case, both the ball joint and the pad should not slide largely and should be almost constraint to the load direction (normal to the plate). Given that, I would to like if you could provide me some insights regarding the contact definition and, in your opinion, what should be the best path to proceed with this simulation - contact or a tie; slide or freeze or stick; etc …

Thank you in advance!

Adriano_Koga

IMO you could try to keep the model linear, for the sake of computational efficency.

You could use TIE contact in places where no sliding is expected, and glueing the parts would be so bad.

Additinally, for some regions, if you define a SLIDE contact, it is still possible to run a linear analysis, BUT with only sliding movement allowed. SLIDE contact in a linear loadcase won't allow change in normal direction. If at the beginning it is in touch, it will be closed for good, and if not in touch, it woun't change to closed contact. So you need to take this into consideration.

The advantage here is taht a linear case is much quicker, specially for an iterative optimization process.

Now if you require a better contact representation, while allowing the contact to be updated, you could use regular NL Contact. This would increase computational time, but with more realistic behavior.

For non-friction contact, you could benefit of running a "semi" linear case, by using PARAM,FASTCONT, which allow you to run a linear model, but still get contact behavior for small slidings.

If not possible, then you should go to full NL contact in a NL Loadcase.

Another question is if the blue pad is stiff enough, you should probably be able to apply an enforced displacement over its top layer, and keep a sliding or tie contact witht he composite plate. It shouldn't be so different from the real case…needs to be compared…