How to do a size optimization with nonlinear material
Hello dear altair community,
I am a student who is at his final thesis. My topic is to analyize the optimization process (sizing) during the effects of small/ moderate material nonlinearity. I have some experiences with linear optimizations (shape, topology and sizing) as well as nonlinear analysis with moderate nonlinearity. But the main problem for me, is that the current version of hypermesh 2022 isnt supporting optimization with material nonlinearity:
*** ERROR # 5771 ***
Design optimization with nonlinear material is not yet supported.
Thats the reason I started with HyperStudy trying to finish my thesis that way, but the amount of knowledge/ tutorials/ examples in the web is very limited. I tried accomplish it a several times, but didnt success ... Thats why I am asking for help to find maybe a good tutorial or even a seminare (I would even pay for it). The main problems comes up during the evaluation (Test model) as well as the part of "Define output responses". My goal is to minimize the mass with a constrain of the total strain to =< 0.02 (2%). I have a lot of examples, because of the company secrets I am not allowed to share it. So I made up a structure myself. Therefore I made a notched cylinder with 3 areas (3 design variables), which all have the inital thickness of 1.5 mm (explicit restrictions 0.1 < 1.5 < 8.0) and a resulting strain of 0.0014 (0,14%).
Material S235/ Stress-Strain-Curve:
0 0
0.001 235
0.01 270
0.02 295
0.03 315
0.04 330
0.05 342
0.06 352
0.07 360
0.08 365
0.09 368
0.1 370
0.2 371
I added my example file. Maybe somebody could help or explain to me how to accomplish an sizing optimization with material nonlinearity using Hyperstudy. Thanks.
Greetings from germany.
Best Answer
-
Batur,
I ran a quick DOE study with all 3 Design Variables linked (so that they always take the same value). I then looked at a scatter plot of Shell thickness against plastic strain. There is a sharp discontinuity at about 1.5mm thickness, below which there is no plastic strain.
See attached image.
1
Altair EmployeeAnswers
-
Hi @Baturadding few resources that might help you
1 -
Jocelyn Renita Quadras said:
Hi @Baturadding few resources that might help you
Thank you for the advice.
After looking through the youtube channel and watching the only 2 videos about Hyperstudy, I still couldnt solve my problem. Furthermore, the Ask the Expert Series doesnt with this topic, eighter.
My last chance is to try out a face to face meeting. Thanks.
But if there is someone, who can help me solve my problem, I would be very thankful.
0 -
Hi Batur,
I believe that the issue you are running into here is that you are trying to use the OptiStruct input, complete with designvariable definitions, and response definitions for the OptiStruct optimizer, as input for HyperStudy. However, as OptiStruct will not run this model (due to non-linear material being defined in an optimization run), then HyperStudy cannot run this model either.
In order to use HyperStudy, you need to define the design variables and responses within the HyperStudy GUI. (Although HyperStudy can automatically identify shell thicknesses from OptiStruct input, as potential design variables, and automatically extract Volume, Mass and Max displacement results as responses. It also recognize DRESP1 definitions and extracts responses for those too.)
So you need to do the following:
1. Remove all the optimization input definitions (design variables, constraints, objectives, optimization controls, etc.) from your model.
2. Check that you have a running analysis model (run the analysis from HyperWorks)
3. Refer to the tutorial HS-1680: Set Up an OptiStruct Model to define the desired input variables and output responses.
Regards,
Greg Harte.
1 -
Batur,
I took a look at your model and recorded the process of setting it up with HyperStudy. See following link.
Greg.
1 -
2
-
Greg Harte_21286 said:
Hallo Mr. Greg Harte,
I cannot thank you enough. You saved my master thesis. Thank you a lot - honestly.
But I have a follow up question. I copied your tutorial and got the same results. As you can see in minitue 11:23 of your video the optimized variables went from 1.5 mm to 0.8894506 mm each.
If I start a FE-analyzation (not optimization) with t = 1.5mm each I get a total mass of 0.0049 tons as well as a plastic strain of 0.0012 as shown in minute 11:23. If I do it with the optimized thicknesses of 0.8894506 mm the mass wents down to 0.0029056 tons (that is correct), but the plastic strain increases to 0.0149 instead of the in minute 11:23 presented 0.0. This is logical, because by minimizing the mass and decreasing the wall thicknesses the plastic strain should increase instead of decreasing to 0. The target should be to minimize the mass and decrease the wall thicknesses until the plastic strain results to (nearly) 0.02 (2%).
- I added 2 pictures of both results for t = 1.5 mm as well as t = 0.8894506 mm.
I also made this optimization with other structures, which led to the same problem. Is there a way to fix this? Is there maybe a problem with my stress-strain-curve or did you forget something?
Thanks a lot Mr. Greg Harte, without you I couldnt event get to this point.
Greetings,
Batur Bulut.
0 -
Hello Mr. Greg Harte,
this is my second reply because my first one wasnt posted - I dont know why. So ...
I cannot thank you enough for your tutorial video how to optimize with hyperstudy. Thanks to you I can go on and complete my thesis.
But I have a last question. I have copied your steps of the tutorial and got to the same results. The problem is the rationality of the results. You can see a decreasing of the designvariables von t=1.5mm to t=0.8894506mm, which leads to a minimization of the mass from 0.0049 tons to 0.0029 tons (see video 11:22 min).
The problem is that the plastic strain should increase by decreasing the wall thicknesses, but that doesnt happen. The plastic strain ends up on 0.0. Therefore I made a FE-Analysis with t=1.5mm as well as t=0.8894506mm (see on the added attachments). There you can see, that the plastic strain is logically increasing. Why does the optimizer ignore that and put the strain to 0.0?
My target is to minimize the mass until the (plastic) strain reaches 0.02, so the contraint becomes (nearly) active.
I also optimized another structures which led to a decrease of the variables von t=3.5mm and t=5.5mm to the lower bound of t=0.1mm because the constraint of the plastic strain also turned to 0.0.
Did I do sth wrong with my stress-strain-curve or my property definition oder sth else?
Thank you a lot Mr. Greg Harte even if you dont reply to my next problem.
0 -
Batur,
There must be something different in the FE-Analysis model that you ran to generate the t=0.8894506.png image, because HyperStudy is running the FE-Analysis at each iteration and you can view the analysis results from any of the iterations in HyperView, and it clearly shows that the plastic strain is going to 0.00 (as reported by HyperStudy).
Can you share the model you used to generate the t=0.8894506.png image?
Thanks,
Greg.
1 -
Greg Harte_21286 said:
Batur,
There must be something different in the FE-Analysis model that you ran to generate the t=0.8894506.png image, because HyperStudy is running the FE-Analysis at each iteration and you can view the analysis results from any of the iterations in HyperView, and it clearly shows that the plastic strain is going to 0.00 (as reported by HyperStudy).
Can you share the model you used to generate the t=0.8894506.png image?
Thanks,
Greg.
Hello Greg,
I only changed the properties from 1.5mm to 0.8894506mm and startet the nonlinear static analysation with optistruct. I added the files.
I made many other structures and got the same problem. They all went after a few iterations to a plastic strain of 0.0.
0 -
The Plastic strain goes to 0.0 for many of the design points, because the part becomes very soft and doesn't resist the load. You can look at the HyperView animations to see what's happening.
1 -
Greg Harte_21286 said:
The Plastic strain goes to 0.0 for many of the design points, because the part becomes very soft and doesn't resist the load. You can look at the HyperView animations to see what's happening.
Yes, I have seen the deformations, but would you really say its correct to let the optimizer set the (plastic) strain to 0.0?
The point is, I was trying to minimize the mass of structures so the walls get thinner until the plastic strain goes UP to 0.02 (2%). Now in this way it gets down to 0.0 so the walls get thinner and thinner for each iteration until they reach the lower bound. So the restriction of the strain doesnt affect the optimization anymore. Maybe do you have any idea how to "correct" the optimization process to consider the effects of the plastic strain or is just "normal" and correct that the plastic strain goes down to 0.0? I just doesnt make sense to me, that the thickness goes down to 0.1mm for every wall and still the plastic strain is at 0.0.
Greetings,
Batur.
0 -
Batur,
HyperStudy is reading the results from the analysis. Within the allowable range of the design variables that you have defined, there are many designs where the plastic strain is below 0.02 and the mass is very low (with the optimum being to set all walls at their lower bounds). HyperStudy is doing what is asked of it.
You need to add other constraints to your study, if this is not what you want. For example the deflections in the model are comparatively large for those designs where plastic strain is 0.0, so you may want to constrain the displacement of certain points.
Regards,
Greg.
1 -
Batur,
I ran a quick DOE study with all 3 Design Variables linked (so that they always take the same value). I then looked at a scatter plot of Shell thickness against plastic strain. There is a sharp discontinuity at about 1.5mm thickness, below which there is no plastic strain.
See attached image.
1 -
Greg Harte_21286 said:
Batur,
I ran a quick DOE study with all 3 Design Variables linked (so that they always take the same value). I then looked at a scatter plot of Shell thickness against plastic strain. There is a sharp discontinuity at about 1.5mm thickness, below which there is no plastic strain.
See attached image.
Hello Greg,
thank you for all your help. Thanks to you I am able to do an optimization with hyperstudy eventhough there are problems with the strain restriction. I talked to my professor about this problem and we found a good compromise to put 2 restrictions into the optimization
strain < 0.02 as well as strain > 0.0
So the optimizer sees the iterations with 0.0 strain result as violations and finds an optimum with strain > 0.0 and < 0.02 eventhough the 0.0 results are partly false.
Thank you
0