Jump to content
francesca

Optistruct_Free Size Optimization_Warnings

Recommended Posts

Hi everybody,

 

I'm trying to run a free size optimization. In the report there are some warnings I can't understand.. I don't know if there are some errors in my model or if I have to change something in the optimization.

Can someone help?

 

HyperMesh model file      https://www.dropbox.com/s/0x8vtw5q9s8q4yf/carro con momenti-CASOB.hm?dl=0

 

HyperView H3d file           https://www.dropbox.com/s/lxtxqbjzk3smg5z/carro con momenti-CASOB_des.h3d?dl=0

report.pdf

Share this post


Link to post
Share on other sites

I realize I've made some confusion in the organization of load collectors and load steps.. So I've updated the model and then I've re run the optimization, but the warnings are the same (for example #1662, #5628).  What do they mean? Where do I have to focus on, in order to make my model correct? (model updated attached, if needed)

 

 

 

https://www.dropbox.com/s/l40vv707llu12dv/carro con momenti-CASOB.hm?dl=0

 

https://www.dropbox.com/transfer/AAAAAJfUDNgP1A_AvVRiY9JRwEX5uBTw03MuufHJK4G66A_b_ZyQgcI

 

 

 *** WARNING # 1662
 Constraint reduced AUTOSPC DOF(s) listed below usually are related
 to a modeling error. Please review the model.
     GRID  1548434 DOF 4
     GRID  1548495 DOF 4
     GRID  1548502 DOF 4
     GRID  1548973 DOF 4
     GRID  1549974 DOF 4
     GRID  1550044 DOF 4
     GRID  1550414 DOF 4
     GRID  1552259 DOF 4
     GRID  1552762 DOF 4
     GRID  1552981 DOF 4
     GRID  1553895 DOF 4
     GRID  1554101 DOF 4
 Number of constraint reduced AUTOSPC DOFs = 12

 *** WARNING # 5628
 The compliance is negative or large 1.32897e+08.
 The rotational displacement has large magnitude, -198.591 degrees (larger than 180).
 The rotational degree of freedom may not be constrained properly in the model.
      subcase id = 2
         grid id = 1403405
       component = 5

report II.pdf

Edited by francesca
update errors

Share this post


Link to post
Share on other sites
6 hours ago, Rahul R said:

Could you please try running this with OptiStruct 2019 or higher version?If possible please share the required .Fem file available in my signature.Files uploaded in dropbox is not working.

Thanks for your reply.

I've shared the file using the link in your signature. Let me know if you receive those files and if they are the right files. In the "from" box I've wrote my university mail, I hope it will work.

 

Thank you.

Share this post


Link to post
Share on other sites

Francesca - 

Does this model run as an analysis run?  I suspect the problem is in the analysis model itself, not necessarily the optimization setup.  It could be a semi-infinite number of problems.  I can't DL the model to look though -- I think only Rahul R can see what comes into the dropbox.

- Robert

francesca likes this

Share this post


Link to post
Share on other sites

Compliance is negative or large, generally this warning comes for modelling error.In your shared file, i see you meshed some 3d enclosed voulme section with 2d mesh/penetraion because of overlap of thickness.

francesca likes this

Share this post


Link to post
Share on other sites
2 hours ago, Rahul R said:

Compliance is negative or large, generally this warning comes for modelling error.In your shared file, i see you meshed some 3d enclosed voulme section with 2d mesh/penetraion because of overlap of thickness.

I don't understand very well.. My model is a shell, I've made the mid surfaces of all the parts of the geometry and then I've connected all the mid surfaces each other with other surfaces. Then I've assigned the thickness to all surfaces. Yes, In some areas the thicknesses overlap.. How can I correct my model in order to have better results in the optimization?

 

Thank you for your time.

Share this post


Link to post
Share on other sites
6 hours ago, Robert Lawson said:

Francesca - 

Does this model run as an analysis run?  I suspect the problem is in the analysis model itself, not necessarily the optimization setup.  It could be a semi-infinite number of problems.  I can't DL the model to look though -- I think only Rahul R can see what comes into the dropbox.

- Robert

The static analysis runs.. But for sure there are some errors in the model my untrained eye cannot see.

I would share the model if only I found a way to.. I don't know why dp doesn't work! If you have an alternative way to share files, please tell me.

 

Thank you.

Share this post


Link to post
Share on other sites

Hi,

 

The model can be downloaded by copy-pasting the link in the browser's address bar. It is easier to debug a smaller, coarsely meshed model. 

 

Element Quality Check reports a warning that 56 elements exceeded the recommended range. Use the following tools to obtain a better quality mesh: 
Geom>autocleanup to clean up the geometry 

  • 2D>automesh (F12)>QI optimize>edit criteria to define element quality criteria
  • 2D>elem cleanup can be used to clean up a group of elements 
  • 2D>qualityindex where element quality can be checked visually and edited using cleanup tools one at a time. The failing elements can be saved to later be retrieved in elem cleanup or automesh again 
  • tool>check elems>2D (F10) to check elements 

The warning 5628 is due to large compliance. The "t8" tub is so thin and unsupported it sags excessively (710mm). The analysis results are invalid because large displacements and rotations violate the linear static assumptions. 

 

The "vincoli" constrains the Z translational degree of freedom at the bottom, but the "carichi2" has a force acting in the same DOF so it does not have an effect. 

displ.gif

francesca likes this

Share this post


Link to post
Share on other sites

Thanks for reply.

 

I've noticed that the big tube is a problem and so the result of the static analysis is not reliable and consequently the optimization is nonsense...

For this reason I've built a simplier model (modify the original model) only for the frame (at the moment with only one load step), and I've put more loads where the frame connects with the big tube and the "front sheet metal". (I think it would be more clear if you took a look at the model..). I share the updated files (model and results) on dropbox. 

 

What do you think about it? I think that now is a bit better than before.. But there's still a #1662 warning in the optimization report...:unsure: 

 

So sorry if my problems may seem trivial, but at university I struggle to find someone able to help and to give me good corrections.

thank you again.

 

 

2 hours ago, Hyperman said:

Hi,

 

The model can be downloaded by copy-pasting the link in the browser's address bar. It is easier to debug a smaller, coarsely meshed model. 

 

Element Quality Check reports a warning that 56 elements exceeded the recommended range. Use the following tools to obtain a better quality mesh: 
Geom>autocleanup to clean up the geometry 

  • 2D>automesh (F12)>QI optimize>edit criteria to define element quality criteria
  • 2D>elem cleanup can be used to clean up a group of elements 
  • 2D>qualityindex where element quality can be checked visually and edited using cleanup tools one at a time. The failing elements can be saved to later be retrieved in elem cleanup or automesh again 
  • tool>check elems>2D (F10) to check elements 

The warning 5628 is due to large compliance. The "t8" tub is so thin and unsupported it sags excessively (710mm). The analysis results are invalid because large displacements and rotations violate the linear static assumptions. 

 

The "vincoli" constrains the Z translational degree of freedom at the bottom, but the "carichi2" has a force acting in the same DOF so it does not have an effect. 

displ.gif

 

https://www.dropbox.com/s/kmtmtpc8my5cs2x/carro only frame.hm?dl=0                                         .hm model

 

 

 

https://www.dropbox.com/s/sbionjngv2yje0p/statica_solo telaio.h3d?dl=0                                     .h3d results static analysis

 

 

 

https://www.dropbox.com/s/yidbjdixm21fahp/ottimizzazione_solo telaio_des.h3d?dl=0           .h3d results optimization

 

 

https://we.tl/t-rjbW4KWWgU        files above, but I used wetransfer

 

 

 

 

report_optimization.pdf

Share this post


Link to post
Share on other sites

Glad to help. 

 

There are free nodes in your model. Either apply autocorrect in model checker or remove by Analysis>preserve node>clear all preserved.

 

The 1662 warning is due to PARAM>AUTOSPC>YES (by default) Automatically constrains degrees-of-freedom with no stiffness- in your case it applied to free nodes:
GRID 1417172 DOF 6
GRID 1549910 DOF 4

 

Use Tools>Model Checker>Optistruct to find & correct modeling errors and warnings.

https://insider.altairhyperworks.com/wp-content/uploads/2017/09/T-T-1248-HyperMesh-Model-Checker.pdf

 
francesca likes this

Share this post


Link to post
Share on other sites

here the model and the results (pdf) of the static analysis and of the free size optimization. What do you think about it? In your opinion, are they realistic/reliable?

 

And for the result of the free size.. How can I "read" correctly the result? I mean.. Is it possible a frame of for example 0.1 or 1 mm thickness from the original 10 mm? How can I "use" this result in the practice?

 

Have I to run another optimization with different constraints?

 

I don't know what to do with those results.. My work would have been to optimize the frame after the free size, but I wasn't expecting such a difference among thicknesses.

 

hope to receive some tips.. Thank you in advance

carro-rev_27-11-2019.hm results.pdf

Share this post


Link to post
Share on other sites

You have shared the model and static analysis results- please share also the optimization results (run_name_des.h3d file). Unfortunately, the model is again so big my computer has trouble even displaying let alone running.


The displacements are small so the small displacements/rotations linear static assumption is valid. However, there are high stresses 800 MPa in "t15" component, possibly exceeding the yield stress and invalidating linear elastic material assumption. There are some bad quality elements (use QI optimize when meshing and quality index & elem cleanup to correct). Everything else looks fine at first sight. Correct boundary conditions are essential and should be carefully considered.


Concept optimization results have to be interpreted considering manufacturability. The thickness reduction is expected since optimization formulation has volume fraction constraint. The smallest thicknesses that can not be manufactured could be interpreted as void.


In your case, I would first run topology concept optimization to understand the load paths- where the material is not needed and where reinforcements should be placed and interpret accordingly. In the detailed design phase size and/or shape optimization would target local stress concentrations. The free-size optimization is used for machined plates and composites, usually in aerospace where higher manufacturing costs can be offset by better performance:

Free-size Optimization.pdf

Share this post


Link to post
Share on other sites

In the PDF: slides 5-6-7-8 are the results of the free size optimization (on component t50 with property t10), slides 1-2-3-4 are the results of the static analysis. (yesterday I tried to attach the _des.h3d file but it was too big, now here it is). 

 

First: Is it correct to view the signed von mises stresses results? I refer to signed von mises, but I don't know if it's right.

 

The high stress in t15 component I think is probably due to constraints/loads.. I put a constraint in t28 leaving rotational dofs free (because of y-moment..).. When I visualized the deformed shape, I realized in this region (component t28 and t15) the deformation could not be ignored (and consequently the stress is high). I don't know how to work out this problem.. It's a problem with boundary conditions, as you say. The t28 rotates around y axis..

 

The moments I put in the model come from a very simple model I made in motionview.

I apply a vertical displacement on two wheels (ant-sx and post-dx, see pdf) and then motionview give me the forces/moments on the frame.. I try to use the moments (those indicated in the pictures of the pdf) on the frame in the hypermesh model (as you can see also in the model file you downloaded).

Maybe I’ve made mistakes in setting up boundary conditions.. I attach the results from motion view and 3 slides in order to be more clear. 

 

So free size optimization is not appropriate in my case of study.. I believe I'm going to give up with the optimization.. I can't find support at university, no one corrects me errors and I haven't enough experience with this program.. I don't know if I'm trained enough to run and understand an optimization, for sure it will take a lot of time.. I think it will be a great result if I'd manage to make the static analysis work properly! 

However, I'll think about your suggestions about optimization process..

 

Thank you very much again for the corrections and the help!

 

 

carro-rev_27-11-2019_des.h3d carro_carico_mw_2Jack.h3d B.C..pdf

Share this post


Link to post
Share on other sites
10 hours ago, francesca said:

The high stress in t15 component I think is probably due to constraints/loads.. I put a constraint in t28 leaving rotational dofs free (because of y-moment..).. When I visualized the deformed shape, I realized in this region (component t28 and t15) the deformation could not be ignored (and consequently the stress is high). I don't know how to work out this problem.. It's a problem with boundary conditions, as you say. The t28 rotates around y axis..

I load (on dropbox, here I can't because of the size) the h3d with the result of the static analysis so you can see what I've tried to explain above:   

 

https://www.dropbox.com/s/4whuo2cvxtgdlr3/carro-rev-rinforzi-mesh-statica-1LoadStep.h3d?dl=0

 

the pdf contains a possible solution..? I've thought about putting another constraint in component t28..

 

 

component_t28.pdf

Simon Križnik likes this

Share this post


Link to post
Share on other sites

Sorry, I overlooked the shared pdf had multiple pages. 


The signed von mises stress basically displays the tensile (+) and compressive (-) von mises stress.


There are two issues:
-If I understood the mechanism correctly there should be loads acting on the other end of the pin (as you sketched in the latest post, also see image below). Extract these counterbalancing forces and moments from MBD.
-applying loads on the same nodes as constraints is not recommended. In cases like this, inertia relief (Analysis>control cards>PARAM>INREL>-2) should be used to constrain the model.  

constraint.jpg
You should not give up so easily- I think you are actually doing great. You can find support on this forum, but you will also have to study on your own. I suggest you go through free Altair e-books, start with  Practical Aspects of Finite Element Simulation and for optimization refer to: Practical Aspects of Structural Optimization with Altair OptiStruct

 

You can learn from learning and Certification program. Please follow below link.

https://certification.altairuniversity.com/  > (Learn Modeling and Visualisation)

 

Check the following youtube channels:

AltairUniversity

Altair India Student Contest

ELEATION By Apoorv Bapat

francesca likes this

Share this post


Link to post
Share on other sites

Join the conversation

You can post now and register later. If you have an account, sign in now to post with your account.

Guest
You are posting as a guest. If you have an account, please sign in.
Reply to this topic...

×   Pasted as rich text.   Paste as plain text instead

  Only 75 emoji are allowed.

×   Your link has been automatically embedded.   Display as a link instead

×   Your previous content has been restored.   Clear editor

×   You cannot paste images directly. Upload or insert images from URL.


×
×
  • Create New...