## Problems with EXPLICIT

## Problems with EXPLICIT

(OP)

Hello, I am doing a dynamic essay of a bus in explicit, but I just can get solutions for little times like 0.004 s, not enough time for me to impact the bus with the floor. My model has about 2500 nodes or even greater:

P R O B L E M S I Z E

NUMBER OF ELEMENTS IS 545

NUMBER OF NODES IS 1590

NUMBER OF NODES DEFINED BY THE USER 456

NUMBER OF INTERNAL NODES GENERATED BY THE PROGRAM 1134

TOTAL NUMBER OF VARIABLES IN THE MODEL 2868

My PC is an AMD 1200 Mhz with 512 RAM memory, is it enough for this problem? How much shoud I have?

Thanks in advance

P R O B L E M S I Z E

NUMBER OF ELEMENTS IS 545

NUMBER OF NODES IS 1590

NUMBER OF NODES DEFINED BY THE USER 456

NUMBER OF INTERNAL NODES GENERATED BY THE PROGRAM 1134

TOTAL NUMBER OF VARIABLES IN THE MODEL 2868

My PC is an AMD 1200 Mhz with 512 RAM memory, is it enough for this problem? How much shoud I have?

Thanks in advance

## RE: Problems with EXPLICIT

run the input file for datacheck and then chive you then check in the dat file. it should give you the size and memory requirements for the problem

harry

## RE: Problems with EXPLICIT

Hello Harry,

The dat file of my last try says this:

P R O B L E M S I Z E

NUMBER OF ELEMENTS IS 716

NUMBER OF NODES IS 2105

NUMBER OF NODES DEFINED BY THE USER 637

NUMBER OF INTERNAL NODES GENERATED BY THE PROGRAM 1468

TOTAL NUMBER OF VARIABLES IN THE MODEL 3930

(DEGREES OF FREEDOM PLUS ANY LAGRANGE MULTIPLIER VARIABLES)

END OF USER INPUT PROCESSING

JOB TIME SUMMARY

USER TIME (SEC) = 1.4000

SYSTEM TIME (SEC) = 0.30000

TOTAL CPU TIME (SEC) = 1.7000

WALLCLOCK TIME (SEC) = 4

If I choose datachek instead of full analysis (in the job menu)with the time I think I need to calculate,will ABAQUS calculate that problem or it will just say how much memory and how long it will take to calculate it?

Thanks in advance

## RE: Problems with EXPLICIT

It was my mistake for the dat file. If you solve the problem in standard then abaqus will give you the memory requirements in the dat file. In explicit the dat file wont do that.

In datacheck abaqus will just go through your einput file and give you the dat file what you have shown but in explicit it wont give you memory estimates

When you start to solve the problem you can get an estimate of the time required for explicit to solve by looking at the time increment explicit assumes at the start of the step.

I think you shouldnthave a problem solving with explicit. Look at the abaqus examples manual for dynamic problems. they have lot of examples for impact problems.

harry

## RE: Problems with EXPLICIT

I have been reading the tutorial and there I have seen that in explicit analysis the mesh should be uniform because of the stability limit. My mesh was finer in some areas and coarse in others, and , as it is said in the tutorial in the .sta file appears the first ten elements whose stability limit is quite different from the rest of the elements. Should I mesh the structure with a uniform meshing in all the elements (there will be more nodes than before), mesh regularly and finer in certain parts (the size of the smaller element affects to the stability limit too) or try to remesh those elements that appear in the .sta file?

9.3.2 Definition of the STABILITY LIMIT:

Based on the element-by-element estimate, the stability limit can be redefined

using the element length, , and the wave speed of the material, :

At=L/c

For most element types—a distorted quadrilateral element, for example—the above

equation is only an estimate of the actual element-by-element stability limit

because it is not clear how the element length should be determined. As an

approximation the shortest element distance can be used, but the resulting

estimate is not always conservative. The shorter the element length, the smaller

the stability limit. The wave speed is a property of the material. For a linear

elastic material with a Poisson's ratio of zero

c=SQRT(E/DENSITY)

9.3.6 Effect of mesh on stability limit

Since the stability limit is roughly proportional to the shortest element

dimension, it is advantageous to keep the element size as large as possible.

Unfortunately, for accurate analyses a fine mesh is often necessary. To obtain

the highest possible stability limit while using the required level of mesh

refinement, the best approach is to have a mesh that is as uniform as possible.

Since the stability limit is based on the smallest element dimension in the

model, even a single small or poorly shaped element can reduce the stability

limit drastically. For diagnostic purposes ABAQUS/Explicit provides a list in

the status (.sta) file of the 10 elements in the mesh with the lowest stability

limit. If the model contains some elements whose stability limits are much lower

than those of the rest of the mesh, remeshing the model more uniformly may be

worthwhile

What is the limit in nodes number for an explicit analysis for about 0.02-0.05 s with a PC? How long would it take?

Thanks in advance,

ferro

## RE: Problems with EXPLICIT

As you pointed out, the time it takes for an explicit job to solve depends on the smallest element dimension, so the number of elements in the model is not necessarily going to change the cost of the solution. A Uniform mesh is OK, but then if your global element size is still small then youve still the same problem. So mesh finely where you need to for accuracy, and then what you do with the rest is less important.

Once you start the job (with interactive) ABAQUS tells you the estimate of the critical element, and the increment size you can estimate the number of increments required by dividing the total job time period required (say 0.5s) by the critical increment time size. The actual time required you will be able to estimate when the job starts as it will tell you the cpu time taken per given number of increments.

If your models are taking too long to run you could choose mass scaling, look in the manuals for more info, but basically is changes the mass of your model so the critical time period goes up hence fewer increments and shorter job time. Never used it myself, it sounds like a bit of a fudge to me but could be good. Also you could redefine your model so that the start of the job is the instant before impact, and give an initial velocity in the load module, create field.

Not sure if that all makes sense. Hope it helps.