Showing results for 
Search instead for 
Do you mean 
Solved! Go to solution

Element quality - Jacobian



Results acheived after the elemental quality of 0.9 Jacobian value is okay. or do we need less value..


Re: Element quality - Jacobian

Depends on whether you want to believe the results for that element..


Please read the documentation given in Femap on how the Jacobian is calculated.  Every pre-processor uses a different scale to make the results digestible.


In easy to digest terms, it is a measure of element distortion relative to an ideal element of the same topology. So if your'e looking at a quad element, it is comparing your quad to the ideal quadraliterial element.


The higher the distortion the less accurate the element stiffness matrix will be, also the value of the Jacabian determinant enters in many other FEM calculations. So using the FEMAP Jacobian fringe scale, it is best to have a Jacobian determinant near 0 for the most accurate results.


If the bad element is far away from areas where you want to read stress or strain values, you may be able to ignore it and not see much impact. But if the element is near an area of high stress gradient, or some place where you need to pull stresses, it should be fixed.





Re: Element quality - Jacobian



Well I am using 0.9 I have only 11 element distorted, when I use 0.8 I have 148 element and when I use 0.7 I have 585 Element distorted. Its  quite normal the more I go close to zero the more element will distorted.


but my question is sir, How can I resolve my problem. 

I want to have good element quality at 0.6. Could you please tell me how can I fix this issue.


Looking forward to hear from you soon.

Re: Element quality - Jacobian

First step is seeing if your model will pass the NX Nastran ELement Quality Check (assuming you will be using NX or MSC Nastran as your solver


Go to Tools > Check > Element Quality, then select all the elements in your model.


Select the NX Nastran Tab, select all the checkboxes, also select check fixup bad elements, run this check.


This will check your model using the same element quality checks NX Nastran will perform before running your model. If you get any failed elements using this check you can be sure you will have a fatal error in the real run.


If you could post a picture of your model that would help so we can see what element topology you are using: Quads, Tets?


Try moving around nodes using the Mesh>Locate option in the meshing toolbox. If you turn on the element quality fringe in the toolbox beforehand, it will update automatically as you move nodes arounds to fix the element distortion.

Re: Element quality - Jacobian

Sir, there are around 585 distorted element it will consume lot of time to repqir manully.


Is there any alternative way to fix all.


please attached find the pics

Re: Element quality - Jacobian

Sir, Any Idea and suggestion would be very much helpful for me.

Re: Element quality - Jacobian

When the geometry detail is difficult / or with small detail, the only way to improve the mesh quality is to use finer mesh. So if you don't want to address local areas individually (eg. using Combined Curves or Combined Surfaces or Feature Suppression), then you need to use finer mesh generally. There is no other way. If you have "thin" geometry compared to the mesh size, then the tetrahedral elements become more flat. The Jacobian is worse when the element is flatter. The Jacobian is improved when the element proportions are more equal. So if the geometry is complex / detailed / thin, then the elements can only be well proportioned when they are finer compared to the geometry.

Re: Element quality - Jacobian

Sir, I already have 1 millions node and 2 million element if I use more finer mesh then It will be more time consuming.


I am very confused how to solve this problem.

Re: Element quality - Jacobian

If you are new to FEA, then this was an extremely difficult problem as a starting problem. I see you have also asked questions about Advance nonlinear. Our best computer has 128GB RAM and 24 cores, and 2GB/sec SSDs, and I would not do Advanced Non-linear analysis for a model bigger than about 500,000 nodes. If it needs many thousands of time steps, then I would allow only 50,000 nodes. The size of an FEA problem is related to the ratio of the largest dimension to the smallest detail of interest. Your geometry is highly detailed and highly complex. You either need many, many elements, OR you MUST compromise a bit on mesh quality OR you MUST have a huge computer and lots of time to run the analysis, OR the physics MUST be reasonably simple (mild non-linear at worst)
Then, you should start with simpler cases to run Advanced Non-linear analysis, and then work up to more complex detail, or a bigger model or more complex physics.
I can say confidently, that if you have 2 million elements and need Advanced Non-linear, then you will need exceptionally powerful computing and runtimes will still be very long. Our record is 170 hours for a 150,000 node model for a 20g automotive load with material failure.(needed about 40,000 time steps to run). More commonly are 15 hour runtimes for 25,000 node explicit impact models which need 200,000 time steps.
By the way, our tests suggest Advanced Non-linear produces its fastest runs with only 4 to 6 cores. It actually slows down if more are selected (at least that is the case for explicit simulations).

Re: Element quality - Jacobian

[ Edited ]

I have system with 32 gb RAM and 4 gb invida graphics card.


I already performed simple linear and non linear static analysis test, both run successfully.


But when I check results, its not correct due to jacobian element 0.9. so thats why I wanted to choose 0.6 size but it says around 1500 element are distorted.


So If I m able to repair this 1500, then problem will be solved