During our webinar held at noon on 9/27/2012 we promised to provide a link to the recording, a PDF of the PowerPoint, and some answers to a few questions. Here is that information:
State Variables
I was a bit confusing on state variables. The problem is with my use of them, not with the variables. The test model only had one integration point. My code is still not working right, the default USERMAT is overwriting my flag somewhere and I don’t have time to figure it out. It’s killing me but I have to do some real work.
But anyhow, my assertion that the state variables are per integration point is correct.
Debugging
I am not aware of any way to use a debugger with ANSYS. There is nothing in the documentation, and to be honest, I’ve not used a real debugger in years. So there may be a way to do so, and see your routine in the debugger since you have the source code, but I have no idea on how to do that. Perhaps someone with more debugging experience can comment below.
Other UPF’s
Someone asked about other routines that are available and we ran out of time before I could go over them. Here is a list.
User elements defined that access the program database directly
USEROU.f
Stores user-provided element output
USERAN.f
Modify orientation of material properties
USERRC.f
COMBIN37 (control/thermostat/spring/damper/resistor) user routine.
UEIMatx.f
Access to an elements matrix or load vector
UTHICK.f
Sets thickness at integration points
UsrFictive
Sets “fictive” temperature (I have no idea what that is)
UFLEX.f
Calculates pipe flexibility for PIPE288/289
UsrShift.f
Allows user to specify time shift
Materials
UserMat.f
User material models
UserHyper.f
User defined hyperelasticity models
UserCreep.f
User defined creep model
user_tbelastic.f
Allows definition of elastic stiffness at a given integration point based on user model. TB,ELASTIC,,,,USER
USERFC.f
User defined failure criteria
USERSWTRAIN.f
User defined swelling, for TB, SWELL,,,,USER
USERCK.f
Helper routine that passes material properties for a user material in
USERFRIC.f
User defined friction calculation. Not just friction but all values calculated in contact calculations with friction turned on.
LOADS
USERFL.f
Changes scalar field values (temp, fluence, heat generation, moisture content, magnetic virtual displacement), by element.
USERPR.f
Calculates element pressure, by element
USERCV.f
Calculates element face convection.
USERFX.f
Calculates element face heat flux
USERCH.f
Calculates element face charge density surface values
USERFD.f
Computes complex load vectors for frequency domain logic
USERPE.f
Calculate the rotation of an elbow pipe element caused by internal pressure
USRSURF116.f USER116Cond.f USER116Hf.f
Modifies the conduction, film coefficient, bulk temp for SURF151/152
userPartVelAcc.f
Ocean wave particle acceleration calculation for PIPE288/289
userPanelHydFor.f
Calcs hydrodynamic loading on SURF164 from ocean loading
USER Commands
USER01.f-USER10.f
Create your own ANSYS commands that are accessed through /UCMD,cmd,num where num refers to the subroutine number and cmd is the command name you want to assign it. Put this in your startxx.ans file to give regular access.
As you will remember from memorizing the previous article, a common use for tables is the set them up to give you a value for a given “primary variable” that is determined by the solver at a given point in the solution. Possible primary variables are: TIME, FREQ, X, Y, Z, TEMP, VELOCITY, PRESSURE and SECTOR. But what if you want to use one of those primary variables to look up a value, then use that value to then interpolate a second value?
A good example is that you have a piece of rotating equipment and the value of the heat transfer coefficient (HF) is a function of RPM and the radius of a given element face. But RPM varies over time. What you can do is make the HF table point to and RPM table that is based on the primary variable time:
So at a given substep, the program will take time and figure out what RPM needs to be. Then it will use RPM and the radius (X in CSYS 1) to figure out the convection coefficient for each node.
As you can imagine, you can get pretty sophisticated with this. The key is that the name of the table you use for the calculated value is input into the variables to interpolate on for the second table, using the *DIM command.
Another common use is scaling tables based on some value. Let say you have a pressure table and the total pressure is scaled over time, based on time. You would make a pressure table that is dependent on say X and y. It would have two planes. One with 0 values and one with the max values. Then you would make a scale table that scales from 0 to 1 based on time. It would look like this:
*DIM,pscl,table,5,,,time !Row label is CPTAB, the table of Cps *taxis,pscl(1,1),1,0,1,5,10,30 pscl(1,1) = .25,.5,1,1,.333
As always with tables, double check things and make sure you have your rows and columns correct. Start simple, and then add more detail. Testing out on a 2x2 or 3x3 tables is a good way to start.
4 and 5 Dimension Arrays and Tables
This section applies to both arrays and tables, so it is a bit beyond the scope of the title, but I hope you will forgive me.
Most users will simply use a one, two, or even three dimension array or table (row, column, plane). However, both arrays and tables support two more dimensions: books and shelves. Because this capability is a later addition to the program, it behaves a little differently. You need to add values for the size of the book (KMAX) and the shelf (MMAX) as well as variable names for each: VAR4 and VAR5
The first difference is in the *DIM command. For normal arrays and tables you use:
It is important to be aware of this because if you look at the manual entry for *DIM it only lists the 3 dimension version of the command, and these variations are covered in the notes.
Once the array or table is defined you have to fill it using APDL commands, this size is not supported in the user interface. The same commands are used, but instead of supplying one, two or three indices values, you supply four or five.
The following is an example of defining a table in terms of location (X,Y,Z), Time, and Temperature. This is the most common usage of a five dimension table:
*dim,ldval,tab5,3,3,3,3,3,X,Y,Z,TIME,TEMP ! table *taxis,ldval(1,1,1,1,1),1,-2.3,0,3.4 ! X Range *taxis,ldval(1,1,1,1,1),2,-1.2,0,1.8 ! Y Range *taxis,ldval(1,1,1,1,1),3,-3.6,0,4.5 ! Z Range *taxis,ldval(1,1,1,1,1),4,0,5,10 ! Time Range *taxis,ldval(1,1,1,1,1),5,32,320,500 ! Temp Range
*do,ii,1,3 *do,jj,1,3 *do,kk,1,3 *do,ll,1,3 *do,mm,1,3 !silly made up equation to fill the table with ldval(ii,jj,kk,ll,mm) = ii*.123+jj/.2+ll*kk+mm*JJ*JJ *enddo *enddo *enddo *enddo *enddo
Writing a Table to a File
For simple 2D tables with up to 10 columns, I use a cheesy macro I wrote called wrttbl.mac. It was used above. It is a bit of a brute force method, because it has code blocks for from 0 to 10 columns. A more general approach would build the actual *VWRITE commands with *VWRITES… It should also be expanded to do Planes. Maybe for a future article.
Anyhow, here it is, maybe you will find it useful.
State Variables
