Problems with EXPLICIT

[ferro1001]

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

 

[harry123456]

hey,
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

 

[ferro1001]

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

 

[harry123456]

Hey,
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

 

[ferro1001]

Hello,

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

 

[charlesbreen]

Ferro

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.