Distribution Table

[vax2005]

Good Morning,
I am trying to assign specific young's modulus and poisons ration to element numbers. I would like to use the distribution table feature but I am having trouble with the syntax. I create a simple case and make the inp file. Then I modify the inp file to include the distribution table and launch the inp with matlab. According to the latest documentation the syntax should look like this
*DISTRIBUTION TABLE, NAME=tab1
MODULUS, RATIO
*DISTRIBUTION, NAME=dist1, LOCATION=element, TABLE=tab1
, E0, 0
element set or number, E1, 1
element set or number, E2, 2
…
*MATERIAL, NAME=MAT
*ELASTIC
dist1
*PLASTIC
…
*SOLID SECTION, ELSET=elset3, MATERIAL=MAT
My question is where to insert these lines? I've been placing them in the model section just above the material call out. The solid section line needs to go in the part section. And it is already created and in the right place. I've also tried putting the *DISTRIBUTION in the part section with no success.
I have attached the inp file i'm using as a test case. I get this error " ***ERROR: in keyword *DISTRIBUTION, file "TryCase1Job.inp", line 82: Unknown assembly id 1.
I put this code just after the assembly.
*DISTRIBUTION TABLE, NAME=tab1
MODULUS, RATIO
*DISTRIBUTION, NAME=dist1, LOCATION=element, TABLE=tab1
, 68900, 0.33
1, 999900, 0.33
2, 999900, 0.33
3, 968900, 0.33
4, 968900, 0.33
5, 68900, 0.33
6, 68900, 0.33
7, 68900, 0.33
8, 68900, 0.33
9, 68900, 0.33
10, 68900, 0.33
11, 68900, 0.33
12, 68900, 0.33
13, 68900, 0.33
14, 68900, 0.33
15, 68900, 0.33
16, 68900, 0.33

*MATERIAL, NAME=ALmm
*Density
2.69e-09,
*ELASTIC
dist1

Any insights or ideas on how to get this to work for a simple case would be appreciated. Have a great day.
Regards,
Peter Phelps

 

[FEA way]

It seems that *DISTRIBUTION is placed correctly (according to the documentation distribution of material property should be specified with material definition) but *DISTRIBUTION TABLE seems misplaced as it belongs to the model level and thus should be placed in similar way as *IMPERFECTION. Try placing it after the boundary conditions.

 

[Mustaine3]

Your input file is written in a part- and assembly structure. This means that the node and element numbers have their own namespaces and the number alone is not enough. The easiest way to fix it is to say to Abaqus/CAE to write a flat input file.
Model -> Edit Attributes

 

[vax2005]

Thanks everyone for the input. I was able to get it working. *Distribution table and *Distribution were placed just after the material section started so in the model section. And I updated the element to reference the assembly instance like Mustaine3 suggested. One other problem i was having was that I left blank lines in the input file. I didn't realize that would cause an issue. I won't make that mistake again. I have attached my working input file that uses a distribution table to modify the elastic modulus ratio and density.
Regards,
Peter