I'm looking for any kind of tutorial/instruction how to use a Design Optimization command.
To be more specific, I would like to know is possible to set the analysis in such way that the system will use pre-defined material thicknesses ("in stock")?. Second question, is there other way to export the results than a function graph?
Thanks in advance for any help.
In a post of my blog I explained the strong capabilities of the OPTIMIZATION module of NX NASTRAN (SOL200) recording a video with instructions to follow step-by step, here you are:
Please note that in FEMAP you can perform only "sizing optimization", not "shaping optimization" because unfortunately FEMAP is not parametric yet, then you can "play" for instance with Shell tickness for CQUAD4 elements, area for CROD, cross section dimensions for CBEAM, etc.. If you want to optimize the thickness of the material, then you must create a Shell model using midsurface extraction feature, OK?.
An finally, the capabilities of the OPTIMIZATION module included in FEMAP covers not only LINEAR STATIC ANALYSIS (SOL101) but also MODAL EIGENVALUE ANALYSIS (SOL103), and when used correctly is extremely prowerful, you can perform sizing optimization of a model including many load cases, this is impressing!!.
Nastran does offer the ability to input a table of allowed thicknesses, or any other design variable value. This not supported from the Femap interface, however the input is very simple and could be added via text input/editing.
In The NX Nastran documentation, see the DDVAL entry, it will be a table of allowed values. You will need to point to this entry on the DESVAR entry.
I have a few questions / problems with the module "Design Optimalization":
1. Constraints - enter the min and max, if we introduce in the case of von Mises stress of 300 min and max 350 the value of stress in the entire model, the optimization will be in the range of 300 - 350?
2. If we are looking for the minimum mass model which consists of a shell-type elements why the algorithm does not reduce the thickness of the shell type in this property even though the tension in this property are negligible eg. 30 MPa and
restraints are like point 1?
The expected response is so slim that the algorithm we all shell-type elements to be included in the specified range of stresses.
3. If we start optimization of value, eg. 1 mm (all properties are the same thickness = 1 mm) by optimizing the thickness is increased due to the stress test and obtain a new thickness for individual properties.
If you execute the same operations on the same model, but we will begin to optimize the thickness of eg. 2 mm we get the result from this corner we have received for the start of 1 mm.
In my opinion the optimization algorithm is a local minimum (different every time) instead find a global minimum.
Of course, if we start from the optimizations, eg. 30 mm thick and slim designs will embolden instead I get a third score.
How to avoid such a situation ?
4. The algorithm gives different results in the case where the structures and the weight loss situation, if we add the material to meet the criterion stress. Get a better result if we lightweight structures but it is not satisfied the criterion of stress and the algorithm adds to the thickness of the shell-type elements.
However, the result in this case is also far from ideal, 'manual' adjustment to the thickness gives better results than the work of the algorithm.
5. If the optimization was carried out and the algorithm performed eg. 20 steps, and the * .f06 optimum in 16 iterations are maps available of stress as a result of optimization refers to the iteration 20 or 16 ?? in my opinion to iteration 20, if it is true that the results are not seen, and so are not optimal !!!!
6. If the algorithm has performed 20 iterations, how can I export the model to the characteristics of properties for iteration 12 ? so as to allow the calculation of the model with the values of iteration 12. In the case of several variables eg. 3 properties change their values according to the results obtained is relatively simple and that in a situation where these variables is 50 or more?
Is there somewhere procesdura available describing the algorithm work in the module Design Optimalization?
Thanks in advance for any help.
First, I would suggest reading the NX Nastran Design Sensitivity and Optimization User's Guide. You can find this Nastran documentation under Feamp Help/NX Nastran. As well as discussion of theory and input, it has example problems to help understand the concepts.
In regards to your questions:
1. Setting the constraint does not guarantee that all stresses fall in that range. It might be better to view that as a target, but that could be impossible given the problem setup(variables,responses,iterations, etc). The problem must contain design variables that have enough sensitivty to these contraints so that this goal can accomplished. Convergence mesages in the F06 file should help understand how the problem is progressing and meeting the goals.
2.Nastran starts optimization by calculating sensitvity of varaibles to responses. If our responses are not sensitive to the design variables, then you might not see any changes to those variables. Also, sometimes numerical issues have to be considered. Sometimes with certain units, the changes in varibles and the responses are numerically too small and scaling must be used to help make sensitivity calaculations meaningful.
3.Yes you can get different results with different starting points. A solution can represent a local minimum. You should always use multiple starting points to understand if this is happening. I do not know of any technique to guarantee a global minimum solution.
4.I do not understand the question here, need some clarification.
5 and 6.Yes you can control the amount of output to better understand the progression from iteration to iteration. Again, see the Nastran documentation for the many options. These are not directly supported by Femap, you will need to add/edit via "Start Text". Femap only writes a basic DOPTPRM entry, you may want to edit this with options to increase the output available in the F06 file.
The param DESPCH controls when Nastran writes the updated model to the punch file, the default is only the final results. See Nastran documentation for options. Also see param DESPCH1 which is related to the data written to punch file.
If you have a particlar example problem that does not seem to follow what you expect, then please post it so we can understand exactly what optimizaton problem you have posed.
Hope this helps,
Thanks for the very helpful and interesting information in the thread. I was looking for the optimization guide and I came across the extensive MSC Nastran 2012 Design Sensitivity and Optimization User’s Guide. However I cannot find a corresponding document for NX Nastran. Does anyone know where such a document is available or are the solvers so similar in this respect that the MSC guide is vailed for NX?
Also, I wonder if multi-objective optimization is possible with this procedure. In my case it would necessary to minimize weight and center of gravity at the same time (a light ship with high cog is not optimal because it will capsize ). It is clear the FEMAP Optimization GUI does not support multi-objective optimization but does Nastran?
If using the latest Femap 11.1.2: In Femap Help, open the NX Nastran document, then you need to select NX Nastran 9(not 9.1) and then you should see the full NX Nastran documentation set. There you will find the Design Sensitivity and Optimization Guide.