Table arrays

[RPSCHMITZ]

Is it possible to define a table array such that it may be used for displacement or force loading at element nodes? I've tried to define a table using 1 column and n-rows with the row indices being the node numbers. The column holds displacement or force loads. What happens, when using the GUI to apply the loads or displacements, is that all the nodes selected end up with the same load value. And that's the first one that was enter in the table. Any thoughts? Thanks.

Bob

 

[meshparts]

It is possible. The column 0 of the table must have the coordinates. The column 1 must have the loads.

Also take a look at

Basic Guide | Chapter 2. Loading | 2.5. How to Apply Loads | 2.5.14. Applying Loads Using TABLE Type Array Parameters

in the Ansys Help.

Regards,
Alex

 

[RPSCHMITZ]

Alex,

Thanks. I’ve been going thru the sections on arrays and tables and haven’t quite been able to figure it out totally. Asked the question of the ANSYS folks and got a similar reply and an example. Here are are few lines from an input file:
!* Create Table
*DIM,ddy,TABLE,10,1,1,X, ,
!*
*SET,DDY(1,0,1) , 0
*SET,DDY(1,1,1) , 0.001
*SET,DDY(2,0,1) , 0.1

When you try to edit it in the GUI all columns are filled with load data, none with coordinates. So, it looks like you have to use the *SET command to get the coordinate information and loads in. At this point it doesn't appear that there is a convenient way to read in the information from a text file. I guess one could create the table from an input file as the ANSY example does. One would have to combine commands, coordinate data and loads in a spreadsheet, create a text file and copy/paste it into the ANSYS input file. A little cumbersome, but I think it would work.

Bob

 

[meshparts]

Try this:

ddy=
*dim,ddy,table,5,1

ddy(1,0,1)=10
ddy(2,0,1)=20

ddy(1,1,1)=100
ddy(2,1,1)=200

It works!

 

[RPSCHMITZ]

Alex,

Thanks. I ran into some indexing problems but now think I have a handle on it. It's a bit more complicated than yours but it does what I want it to do. Again, what I’d like to do is enter either force loads or displacements explicitly at nodal points. What I was able to do was set up a table with LOADS=f(X,Z,Y) where X is the length (along a 48”long x 12” wide x 6” thick plain concrete beam), Z is the width and Y the thickness (the plane variable). Load values are then enter for the X,Z location at either the bottom Y=0 or top Y=6 (plane) location.

Here are the lines that create the entire table:
!* Create Table
*DIM,LOADS,TABLE,1,4,2,X,Z,Y
!*
*SET,LOADS(0,0,1) , 0 ! Y = 0, BOTTOM OF BEAM
*SET,LOADS(0,1,1) , 0 ! Z = 0, ALONG BEAM WIDTH - TYP
*SET,LOADS(0,2,1) , 4 ! Z = 4
*SET,LOADS(0,3,1) , 8 ! Z = 8
*SET,LOADS(0,4,1) , 12 ! Z = 12
*SET,LOADS(1,0,1) , 24 ! X = 24, ALONG LENGTH OF BEAM
*SET,LOADS(1,1,1) , 0 ! LOAD
*SET,LOADS(1,2,1) , 0 ! LOAD
*SET,LOADS(1,3,1) , 0 ! LOAD
*SET,LOADS(1,4,1) , 0 ! LOAD
*SET,LOADS(0,0,2) , 6 ! Y = 6, TOP OF BEAM
*SET,LOADS(0,1,2) , 0 ! Z = 0, ALONG BEAM WIDTH - TYP
*SET,LOADS(0,2,2) , 4 ! Z = 4
*SET,LOADS(0,3,2) , 8 ! Z = 8
*SET,LOADS(0,4,2) , 12 ! Z = 12
*SET,LOADS(1,0,2) , 24 ! X = 24, ALONG LENGTH OF BEAM
*SET,LOADS(1,1,2) , -10 ! LOAD @ Z=0
*SET,LOADS(1,2,2) , -20 ! LOAD @ Z=4
*SET,LOADS(1,3,2) , -30 ! LOAD @ Z=8
*SET,LOADS(1,4,2) , -40 ! LOAD @ Z=12

Once the table is created one could also use TREAD to input load and coordinate table values. Here are those lines:
0
0,4,8,12,24
0,0,0,0
6
0,4,8,12,24
-10,-20,-30,-40

The only caution is when applying the loads. You have to graphically select the individual nodes. If you select all the nodes or plot nodes at any thickness level you’ll get the loads applied to all of them. If you have the full load at the top level it proportions for nodes selected at a lower level. A way I believe to avoid this problem would to create an input table that has all the coordinate locations defined at the desired level and zero loads where none is desired. Then you could select and apply the loads all the nodes at the desired level. In this case the top of the beam.

Bob