How to describe the load shown in the attached image?

[Victor75]

Dear Abaqus experts,
I'm a novice user of Abaqus CAE.
I want to load a piece with the kind of load shown in the attachment, but I don't know how to do it. Any suggestions?
Thank U!

 

[MrMyers]

You could use a subroutine?
Or work out an equivalent pressure load and use the hydrostatic function?

 

[brep]

1. Go to the loads module
2. Create an analytical field (Tools-Analytical Field-Create...)
3. Type in an expression describing your distribution. In this case it is quite trivial ==> X*100/a where a is the length of your block. (Note that "x" is not the same as "X") Make sure you have a local csys (appropriately located at the "origin of your load) that you can reference for the expression.
4. Create a pressure load, choose the analytical field that you just created as the "distribution" (there is a pull down combo box)

Have a look at the attached image.

As you get more familiar with python expressions, you can get quite creative with these...

 

[Victor75]

Thank U, brep. Thank U, Mr. Myers. But I couldn't solve the problem:
I'm using Abaqus version 6.5, and I can't find the option "analytical field": just "temperature field", "velocity field" and "initial state field" are available.
Should I use a subroutine? How? I have never done it.
Please help!

 

[brep]

Analytical fields were introduced in V6.6 (released May 2006). Subsequently in V6.6EF, V6.7 and V6.7-EF there have been substantial enhancements to this capability, so it is well worth updating your software.

 

[corus]

In 6.5 you can define a pressure in the load module of CAE. One of the options is to apply a hydrostatic load, which is the equivalent of your load type.

You cna also define a User Defined pressure in the same options of the pressure load using a subroutine. A subroutine is fairly easy to do if you have a fortran comiler available. There are examples in the manual that you can follow. For this case you'd use DLOAD and set the variable F=a.COORD(?)+b, whatver a an b would be for you geometry and for whatever direction the COORD was in. The rest of the subroutine, declaration of variables etc., just copy and paste from an example. When you run the job just set job=.... user=fred where fred is the fortran source code for the subroutine.



corus