Error jacobian

Hi Aslan

Please have a check whether these forum posts can help you.

https://community.altair.com/community?id=community_question&sys_id=49a6c87a1b2bd0908017dc61ec4bcb34

https://community.altair.com/community?id=community_question&sys_id=1886883a1b2bd0908017dc61ec4bcb54

Thank you for reply @Pranav Hari

I looked at all the titles before asking.

I can't figure out it with these ways because it's not exactly the same problem as mine.

Are you getting this error while pre processing the model in HyperMesh?From above screenshot it seems, mesh is not connected and splitted at many location.Would be nice if you could share hm file.

Hi Aslan,

it looks like solid map went wrong. The outline and temporary nodes are automatically created around distorted elements.

You should delete the mesh and rebuild.

If the component does not have complex thickness variation it can easily be meshed: first in 2D and then extruded to 3D hexa mesh.

Also, considering only the displayed geometry splitting the part seems excessive, which also causes bad meshing around holes.

Thank you @Rahul R 

I must ask before sharing. but I can share  .out file. Maybe you can help me.

Unable to find an attachment - read this blog

Hi Aslan,

 

it looks like solid map went wrong. The outline and temporary nodes are automatically created around distorted elements.

You should delete the mesh and rebuild.

If the component does not have complex thickness variation it can easily be meshed: first in 2D and then extruded to 3D hexa mesh.

 

Thank you Ivan,

Actualy I can't get the proper mesh. And I think that's the problem.

Firstly I use Geom----Solid Edit and then 3D---Solid Map 

You said that firslty 2D then extruded to 3D heca mesh.

Can you explain in detail?

Sure, first create 2D elements with 2D Automesh panel (F12) on the top surfaces of solids.

Then use these 2D elements to create the 3D hexa mesh in two different ways:

-if the component has constant thickness you can use 3D>elem offset>solid layers panel

-for better mesh control in the thickness direction use the 3D>solid map>general panel and select 2D elements to drag

After Hexa mesh is created delete the 2D elements.

Is there a reason to split the solid in such a pattern? Otherwise, only washers should be split around holes.

Sure, first create 2D elements with 2D Automesh panel (F12) on the top surfaces of solids.

Then use these 2D elements to create the 3D hexa mesh in two different ways:

-if the component has constant thickness you can use 3D>elem offset>solid layers panel

-for better mesh control in the thickness direction use the 3D>solid map>general panel and select 2D elements to drag

After Hexa mesh is created delete the 2D elements.

 

Is there a reason to split the solid in such a pattern? Otherwise, only washers should be split around holes.

First of all thank you very much.

I think if I can do as you say, my problem can finish. 

I'm sorry I'll have a few questions.

1. should I apply 2d mesh to a single surface.

2. 3D----Solid Map---General---

<?xml version="1.0" encoding="UTF-8"?>

surf geom= should I choose the opposite of the mesh?

elems to drag = should I choose the entire region where I apply mesh?

1. The idea is to use the 2D mesh to impose a mesh pattern on hexa mesh. If you want a specific mesh pattern in the through-thickness direction you can also 2D mesh the sides and use nodes or elements as guides (elems to drag/match, along geom). Note that imposing mesh patterns in 2 directions requires well thought out meshing plan as it needs to be 2 directionally mappable. 

Maybe you will find videos on solid map helpful

.

2. surf geom in the case of provided screenshot can be set to none, because it is already defined by elems to drag.  Select the surface opposite to the 2D mesh as dest geom.

Please hit the like button on useful tips /emoticons/default_wink.png' srcset='/emoticons/wink@2x.png 2x' title=';)' width='20' />

Thank you @Ivan

I am so sorry /emoticons/default_sad.png' srcset='/emoticons/sad@2x.png 2x' title=':(' width='20' />

How can I fix the difference in geometry. 

the right figure must be like the base

<?xml version="1.0" encoding="UTF-8"?>

No problem /emoticons/default_smile.png' title=':)' width='20' />

Solid map applied on complex shapes can have issues with node associations between source and destination geom (like the 2nd picture with skewed mesh). Defining along geom might help.

Another option is to duplicate and project elements (tool>project>to surface) from source geom to dest geom and pick those elements as elems to drag and elems to match, respectively.

To model the difference in geometry through thickness I would trim the solid with sweep lines in the thickness direction using 2 lines forming the 'L' shape (at the tip of the arrow in the 1st picture). Basically, we want inner edges to be imprinted on outer surfaces to facilitate mesh transition. The solid should then be split using the trim with plane/surf panel into 3 longitudinal parts.

Then I would 2D mesh the side and bottom faces, which would be used in solid map panel to extrude all in one go (and delete the unwanted elements) or it can be done in three sequential steps through the thickness.

That part is challenging, because it is difficult to get good quality mesh and ensure mesh continuity near acute angles.

It is essential to start with good quality 2D mesh:

-create 2D elements with QI optimize on Automesh panel

-check and edit the mesh using quality index

-repair the mesh using elem cleanup or smooth panel

Even then some elements near sharp corners might be of bad quality. Use the triangular element at the tip, and if still unable to get good quality there are three options:

-refine the mesh in the area

-move the nodes outside geometry boundaries to satisfy quality criteria,  but losing geometric accuracy

-accept the bad quality mesh, if major stress/strain is not expected in that area. To bypass Optistruct element check:  Analysis>Control Cards>PARAM>CHECKEL>NO

Hı @Ivan

I am so sorry really:( 

But I cant.

I agree that bad mesh structure and I did PARAM--CHECHKEL--- NO but I still get the same error.

I just found that negative jacobian can't be bypassed.

So the only option is to reconstruct the mesh (starting from 2D).

It is difficult to give useful tips without direct access to the model. 

If you are unable to share the model due to proprietary reasons, maybe you can share only the part or change the proportions (using Hypermorph) or construct sample geometry with features similar to the problem.

Hı @Ivan

Can you share your private e-mail address?

OK, I will update you through e-mail

You may find useful this playlist about hexahedral meshing: