Difficult to say without knowing the details of your application. Just a few points to consider:

- Is the mesh size appropriate for the highest frequency of interest in both materials?

- Is it necessary to analyze this problem in 3D?

- Can you make use of symmetry, e.g. by discretizing a quarter of the geometry only and apply symmetric boundary conditions?

- Higher-order spectral elements would drastically reduce the number of dof, particularly for simple geometries, but I dont know  whether they are implemented in Abaqus.

- Is the transition from smaller to larger element size appropriate? If the difference in element size is extremely big, one might consider using non-conforming meshes.

Good luck

Dear Negar,

What is your analysis type?If you run ABAQUS-EXPLICIT, the number of elements would not be any matter. If you use ABAQUS-EXPLICIT, your analysis will definitely be completed but its time can be very high (about 3-4 days) . Mass-scaling could be a good option to reducing run time, if you run a quasi-static analysis

"If you run ABAQUS-EXPLICIT, the number of elements would not be any matter"

That is incorrect - in an explicit analysis, the CPU time scales proportional to the number of nodes and inversely proportional to the size of the smallest element. In an implicit analysis, the CPU-time roughly scales as the square of the number of nodes.

Why do you need such an extremely fine mesh everywhere in the yellow region? Is there a strong inhomogeneity or something else that will prevent your solution from being smooth on a larger scale?

If there is only a small region of interest, try to partition the part more to get a graded mesh.

You can also start with a coarser mesh and gradually refine to see whether the meshdensity really needs to be as large as you suspect.

"If you run ABAQUS-EXPLICIT, the number of elements would not be any matter".

Here, I mean whatever the number of elements increase, since the ABAQUS EXPLICIT algorithm doesn't check any convergence,  analysis will not stop.

Dear Negar,

Have you considered applying symmetric boundary conditions?

If you notice the regular geometry of your specimen, you may be able to reduce to 1/4 of your current model size.

This is one practical way I see you can solve it easily.

Good luck!

Dear Negar,

Since Abaqus (and for that matter no commercial FEM software I am aware of) does not offer nodal-based finite elements with shape functions having a polynomial degree of three or higher you should at least you elements with quadratic shape functions. Due to the increased accuracy (improvedapproxiamtion of the geometry and the unknown displacement field) you can also increase the element size. The elevation of the polynomial degree of the shape functions is typically more advantageous for the efficiency (compare to papers concerning the p-FEM) than decreasing the element size. Since you cannot do much else in Abaqus except for exploiting symmetries in the model that might exist (mentioned also by Yanfeng) and using quadratic shape functions you are limited by your computational resources.

Best

Hallo Madam Kamali,

answere to your question is the attached picture. Please do pay atention to stress/strain effects. 

this meshing techniques was used in the 1985 for plate bending problem and is still valid for such issues.

(this answere is from meshing point of view). there are surely other possibilities where you can reduce the CPU time

Warm regards,

Tamer Qaimari

Dear Tamer,

You are certainly right. Nonetheless, I want to take the opportunity to point out a few things that are unfortunately often forgotten in FEA practice.

1) In three dimensions we have to include both tetrahedral and pentahedral finite elements in order to get a similar transition from a coarse mesh to a fine mesh. This is due to the fact that tetrahedral and hexahedral elements cannot be coupled without introducing constraints.

2) We always have to pay attention to the ratio by which we in-/decrease the element size. If this is done to abrupt we can loose accuracy and render the solution useless. Therefore, we have to partition the model in order to generate a regular mesh where possible and construct a "big enough" transition zone where the element size is gradually reduced.

3) Depending on the model it , however, could be dificult to implement such a transition approach. As I said weneed a transition zone of a specific size.

To give a final statement Tamer is right, we would need more information about the model.

But constructing a high quality mesh is always a good option to reduce the computational effort for the solution of the system equations.

Best

Dear Sascha,

This is clear that there should be  tetrahedral and pentahedral finite element no doubt about it. Thank you for for make it more clear to other users. As i clearfied in my answere this is from mesh technique point of view only. 

Offcourse as an FE analyst or Engineer, stress strain jumps from coarse to fine mesh should be carefully considered!. you are right many tend to neglect considering that.

i think Madam Kamali should give us more insght into the real mechnisim or physic behind this problem. i answered the question from meshing side. i think to judje if it works or not we should have more explanation from Madam Kamali regarding the BCs, loading and FE problem type in more detail.

thank you for your Notation, specially on transition zone. 

Warm Regars,

Tamer Qaimari 

Dear all,

Many thanks for all your helpful insights. I'm going to give a more detailed explanation here.

The model should be 3D because I have already modeled a 2D and it's not accurate enough. I have used symmetric boundary conditions. Originally, the model is a dog bone specimen which we're trying to propagate a wave exactly at the middle point perpendicularly, therefore it's important that we retain the thickness of the specimen. but the other 2 dimensions are already cut to the smallest. Since this a wave propagation problem, I have to make sure BCs don't affect it. 

Also, the material is heterogeneous.  Other than symmetric BC's, I don't have any BC. And I have to do a STATIC analysis first ( just a tensile test) , then I use these results for my EXPLICIT analysis. (Standard --> Explicit ) The frequency of the load is very high and the mesh size should be very fine in the yellow region. I have used different partitions and using sweep to gradually refine it but the mesh ends up being very messy or it ends up being OK at 2 surfaces and not so good at two others. 

My problem is that the program wouldn't even run the static case. (which is probably only one increment) .

Dear Tamer, 

does Abaqus support pentahedral elements? since those are what needed to be used in the transition zone.

Thank you all again,

Negar

Dear Negar,

Abaqus supports both 6-node (linear shape functions) and 15-node (quadratic shape functions) pentahedral finite elements.

If you want to model wave propagation than why is the mesh only in one part of the model fine?

Could you use non-reflecting boundary conditions for the wave propagation? Or are the reflections essential for your model? Non-reflecting or absorbing boundary conditions are often used to decrease the model size in wave propagation analysis.

If even the Static case is not run, what kind of error messages do you get? There must be a bug somewhere or your RAM is to small.

Best,

Sascha

Dear Sascha,

Thanks for your reply. I guess I can probably use non-reflecting BC. I only needed the green part to make sure the wave wouldn't reflect but the size of elements could be coarser (reasonably). But still the number of elements for the yellow part is more than a Million and I can not have coarser mesh in that region because that would affect the info that I need. 

The error message is as follows:

An error occurred during a write access to /tmp/job-1. Check the disk space

on your system.

Specs on my PC are 32 GB RAM and 1 TB Hard drive. core i7. 

Bests,

Negar

Dear Negar,

answere to your question was given by Sacha, abaqus do support such elements. 

-have you done sensitivity Analysis for such case  inorder to  know how fine or how much element do you need e.g in thickness direction? 

regarding the Error it is clear that you do not have space!, i belive you need a troubleshooting strategy:

First, try to make your problem simple possible with the output you get from Sensetivity analysis where you know how much fine you should be. 

Second, i would try to minmize the length not the thickness and see if it gives result in static analysis. Becuase simulation is abroted due to space!, so you do not really know if it would converge or not if you have a space.

These two steps tells you where you are. Share with us what you get, then we can discuss it further.

Negar,

Generally, wave propagation problems need 10-20 nodes per wavelength. Is there anyway to play with number of nodes to make it coarser or it's a fixed number?

Regards,

Dear Ashkan,

You are correct but for nonlinear wave propagation, you have to have at least 20 elements per  wave length. Now if the frequency is too high and specially if one wants to detect higher harmonics, the mesh size should be 20 element per that harmonic's wavelength. I'm looking for some ways to reduce the computational cost.

Bests,

Negar

Dear Negar,

the error message actually says that you do not have enough space on your hard drive. Did you check that? In the directory abaqus is writing the results in you have to make sure that there is enough space left. Have you partitioned your hard drive? you can specify the scratch directory for abaqus when starting a batch job as

abaqus job=Job-1 interactive scratch=C:\Temp

If you have enough space left I do not know why abaqus should encounter this error.

Best

Dear Sascha,

Thanks for your comments, but I have done all of those in fact I have almost 900GB free space in Abaqus' working directory. I also do not know if this is normal for approximately 1 Million elements and a nonlinear analysis or there is a problem with my PC.

Bests,

Negar 

Negar,

My model has almost 100,000 elements and 20,000 time increments. Abaqus writes just displacements and velocities to .odb file. However the .odb file is 150GB!

Ashkan,

Ok!!! now I can see why my model's odb file will not fit in an almost 1 TB hard drive. 

Thanks!

Negar